Part Design
CATIA V5 Training
Foils
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Part Design Expert
Instructor Notes:
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Version 5 Release 19 September 2008 EDU_CAT_EN_PDG_AI_V5R19
Part Design
About this course Objectives of the course
Upon completion of this course, you will be able to: -Use 3D reference Elements to create a part -Create advanced Sketch-Based Features -Apply Advanced Dress-Up Features -Design using Boolean operations -Share Designs by working in Multi-Model environment -Analyze Parts -Annotate Parts for review
Targeted audience
CATIA V5 Mechanical Designers
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Prerequisites
Students attending this course should have the knowledge of CATIA V5 Fundamentals, Getting started with CATIA V5, Sketcher, Part Design Fundamentals
Instructor Notes:
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1.5 Days
Part Design
Table of Contents (1/3) Using 3D Elements to Create a Part Introduction to Using 3D Elements to Create a Part Local Axis 3D Wireframe Elements Holes/Pads not Normal to Sketch Plane Creating Pads and Pockets from Surfaces Surface-Based Features 3D Constraints Using 3D Elements To Create Parts Recommendations Using 3D Elements to Create a Part: Recap Exercises Angle Bracket Sum Up
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Sketch-Based Features Introduction to Sketch-Based Features Creating Ribs and Slots Creating Stiffeners Creating Multi-sections Solid Sketch Based Features Recommendations
Instructor Notes:
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6 7 8 15 25 28 32 39 44 47 49 50
51 52 53 62 67 103
Part Design
Table of Contents (2/3) Sketch Based Features: Recap Exercises Sum Up
Part Manipulations Introduction to Part Manipulations Scanning a Part Design Using Boolean Operations Cut, Paste, Isolate, Break Sharing Geometries Sketch Selection with Multi-Document Links Part Manipulations Recommendations Part Manipulations: Recap Exercises Sum Up
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Dress-Up Features Introduction to Dress-Up Features Advanced Drafts Thickness Removing Faces Replacing a Face with a Surface
Instructor Notes:
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110 112
113 114 115 123 149 158 166 172 178 179
180 181 182 197 202 205
Part Design
Table of Contents (3/3) Dress Up Features Recommendations Dress-Up Features: Recap Exercises Sum Up
Part Analysis Introduction to Part Analysis Analyzing Threads and Taps Draft Analysis Surfacic Curvature Analysis Part Analysis: Recap Exercises Sum Up
Annotations
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Introduction to Annotations Text with Leader Flag Note with Leader Annotations Recommendations Annotations: Recap Exercises Sum Up
Instructor Notes:
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207 211 214
215 216 217 221 226 229 230
231 232 233 236 241 246 247
Part Design
Using 3D Elements to Create a Part
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You will learn how to use 3D elements to create solids based on
Introduction to Using 3D Elements to Create a Part Local Axis 3D Wireframe Elements Holes/Pads not Normal to Sketch Plane Creating Pads and Pockets from Surfaces Surface-Based Features 3D Constraints Using 3D Elements To Create Parts Recommendations Using 3D Elements to Create a Part: Recap Exercises Angle Bracket Sum Up
Instructor Notes:
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Part Design
Introduction
Part creation is frequently based on 3D wireframe elements like lines or planes or on surfaces :
You will see how to create 3D wireframe elements and how to create local axis used to position geometries.
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You will see how to create solid based on existing surfaces and how to position 3D geometries with regards to planes or surfaces.
Instructor Notes:
In this section, you will see how to use Wireframe and Surface elements to support the development of Solids and how to exploit 3D Planes and Local Axis systems in Part Design…
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Part Design
Local Axis
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You will learn how to create a local axis in order to define local coordinates
Instructor Notes:
In this part, you will learn how to create a Local Axis system…
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Part Design
What is a Local Axis ? It is possible to create a local axis in order to define local coordinates. For example, it is, sometime, easier to build a point by coordinates in a local axis rather than creating it in the absolute coordinates system
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Point created in the local coordinates system
Instructor Notes:
Explain how a Local Axis system allows you to work with a Coordinate System that may be more useful than the Absolute Coordinate system for certain aspects of your design. In this example, we see a Local Axis system defined relative to a tangency point on a non-planar face of the solid part. New points can easily be input relative to this location by using the Local Axis system.
Let’s see how we can create a Local Axis system…
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Part Design
Local Axis : Creation It is possible to create a local axis in order to define local coordinates. For example, it is, sometime, easier to define point coordinates with respect to a local axis rather than to the absolute coordinates system
1
Select the Axis System icon
2
Select the local axis origin point
3
Select the OX direction
(2)
(3)
4
Select the OY direction
5
Select OK in the dialog box
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You get :
(4)
(5)
Instructor Notes:
Explain how to access the Axis System tool and use the dialogue box or the Local Axis geometry to complete the Axis System creation.
Let’s see how to use a Local Axis System once it is created…
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Part Design
Local Axis : Use It is possible to create a local axis in order to define local coordinates. For example, it is, sometime, easier to define a point coordinates with respect to a local axis rather than to the absolute coordinates system Set the axis system As the Current one with the contextual menu
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1
(1)
2
Using the Point function (Coordinates options), create a point with X=0, Y=0 and Z=100
You get :
Instructor Notes:
Explain that many different Axis Systems can be defined within a Part Document. Activating (or Set As Current) an Axis System is done through a Contextual Menu. The Contextual Menu can be accessed by right-clicking in the Specification Tree or in Geometry View. Note that Deactivating (or Set As Not Current) is achieved in the same way. When a Local Axis System is Set As Not Current, new input Coordinates are then referenced to the Absolute Axis System.
Let’s look at some Global Settings that affect the creation of a Local Axis System…
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Part Design
Local Axis-System Setting (1/3) Check the ‘Create an Axis-System when creating a new part’ option if you wish to create a three axis-system which origin point is defined by the intersection of the default planes that are plane XY, plane YZ and plane ZX Select Tools -> Options
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1
Instructor Notes:
Tools -> Options provides a switch for automaticall creating an Axis System whenever you create a New Part…
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Part Design
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Local Axis-System Setting (2/3) 2
In the Options dialog box, select Infrastructure > Part Infrastructure > select Part Document tab
3
Select the Create an Axis System when creating a new part option
4
Select OK
Instructor Notes:
This Switch is found under the Infrastructure -> Part Infrastructure -> Part Document tab. By default this switch is turned off, but you may activate it…
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Part Design
Local Axis-System Setting (3/3) 5
Select the File -> New command
6
Double click on Part in the dialog box
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The local axis is automatically created:
Instructor Notes:
When the switch is activated, a Local Axis System is automatically created when you create a New Part. Explain that by default the Axis System is positioned on the Absolute Origin and is oriented the same way as the Absolute Axis when the New Part is created. However, you can modify the location and orientation of the Local Axis System by double-clicking it in the Specification Tree or Geometry View. Note that the Abosolute Axis Planes are Hidden by default when the New Part is created under this Option.
Solicit questions from the students on the creation, modification and purpose of Local Axis Systems.
When questions have been answered, continue on to Working With 3D Elements in the Part Design workbench…
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Part Design
3D Wireframe Elements
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You will learn more about 3D wireframe elements and how to use them to construct your part.
Instructor Notes:
You will now learn how to create 3D Wireframe Elements while in the Part Design workbench to assist you in the development of Solid Features…
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Part Design
What are 3D Wireframe Elements ? In the Part Design workbench, you can create points, lines and planes without using the Sketcher workbench but by using the “Reference Element” toolbar. Points ,lines and planes created using reference toolbar are 3D elements can be used for reference purpose. For Instance, you can use this toolbar to create a plane at an angle ,and sketch on this plane when existing surfaces of the part do not provide an appropriate sketch plane for the creation of a feature. You can use the 3D reference line to create a pad in a direction other than the direction normal to the sketch.
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The Specification tree: When Points and lines are created in sketcher workbench using profile toolbar.
Point and line created in sketch
The Specification tree: When Points lines and planes are outside the sketcher workbench using reference elements toolbar
Point and line created using reference elements
Instructor Notes:
Explain that the Reference Element toolbar provides access to a very small subset of Wireframe elements that are usually accessed through the Wireframe and Surfaces or Generative Shape Design workbenches. These commonly used 3D Wireframe Elements (Point, Line and Plane) are accesible through the Part Design workbench because it is more efficient than switching back and forth between two workbenches when you need them. Note that since these 3D elements are not Solid Features, they are stored in Open Bodies rather than in Part Bodies. This is true even if you create them from the Part Design workbench. Point out that explicit 3D Wireframe and Surface elements can be used in many ways to develop Solids.
Let’s look at some of the ways these elements help support the design of Solids…
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Part Design
3D Reference Elements (1/4) 3D reference elements are used mainly to reduce the impact of deletions and optimize the designing of parts and their modifications. They are used to ensure consistent parent children relationships. First case
Create a Base Pad from the sketch shown.
Create a sketch on the top face of Base Pad. Constrain the sketch completely using the edges of the Pad. Using this sketch a Upper Pad.
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Create a sketch on the top face of Upper Pad. Create a Pocket
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Create the holes on the top face of the Upper pad. Dimension the holes with respect to the Pad edges.
Part Design
3D Reference Elements (2/4)
The upper pad is dependent on the Base Pad.
The Pocket is dependent on the Upper Pad.
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Now when we try to delete the Upper Pad, an update error is displayed.
Instructor Notes:
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On deletion of Parent feature, the children features are affected.
Part Design
3D Reference Elements (3/4) Second case Top Reference Plane
Create a Base Pad from the sketch shown. Create a ‘Sketch’ for ‘Upper Pad’ on the bottom reference plane. Dimension the Sketch with reference to standard Planes. Create ‘Upper Pad’ using this ‘Sketch’.
Bottom Reference Plane
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Create a ‘Sketch’ for ‘Pocket’ on the top reference plane. Dimension the Sketch with reference to standard Planes. Create ‘Pocket’ using this ‘Sketch’.
Create the holes on the top face of the ‘Upper Pad’. Dimension the holes with respect to the standard Planes.
The sketch created is independent of the parent Pad but is created with the help of reference elements
Instructor Notes:
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Part Design
3D Reference Elements (4/4) The upper Pad Sketch is created on reference Plane and independent on the Base Pad.
The Pocket Sketch is created on reference Plane and independent on the Upper Pad.
On deletion of the first feature Upper Pad, the pocket is not affected.
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So parts created using reference elements are more stable.
Instructor Notes:
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The upper pad is created on Reference elements and is independent of first feature.
Part Design
Creating 3D Wireframe Points 1
In the Reference toolbar, select Point by clicking on the icon
2
A dialog Box is displayed
3 Notice that you can choose from several options from the drop down menu
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The created point appears under part body.
Instructor Notes:
Explain how to access the 3D Point tool and the various options available in the dialogue box for creating points. Note the option to select a Reference Point other than the Default (Origin). Point out the resultant 3D Point in the Open Body of the Specification Tree.
Let’s now see how to create a 3D Line in support of our Solid…
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Part Design
Creating 3D Wireframe Lines 1
In the Reference toolbar, select Line by clicking on the icon
2
A dialog Box is displayed
Notice that you can choose between several types of line
The created line appears under part body due to hybrid nature
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3
Instructor Notes:
Show how to access the 3D Line tool and explain the various options available for creating this feature. Point out that a Contextual Menu is available to support creation of necessary geometry (e.g. Points) if they have not been created earlier. Explain the purpose of the Start, End and Mirrored Extent options. Note the Line feature in the Open Body.
Let’s now see how to created 3D Planes to support our Solid design…
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Part Design
Creating 3D Wireframe Planes 1
In the Reference toolbar, select Plane by clicking on the icon
2
A dialog Box is displayed
Notice that you can choose between several types of planes
The created plane appears in the part body because of hybrid nature
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3
Instructor Notes:
Show how to access the 3D Plane tool and explain the different methods for creating planes. Point out that a Contextual Menu is available to create necessary support geometry if it has not been created earlier. Explain the purpose of the Repeat Object After OK check box. Note the 3D Plane under the Open Body in the Specification Tree.
While the Part Design workbench makes only Point, Line and Plane elements available, you can always switch to another workbench to build more complex 3D Wireframe or Surface elements to support your Solid development. Let’s see an example of this…
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Part Design
Using 3D Wireframe Elements to Create a 3D Curve
1
You can create points according to their coordinates by using the Points tool in the Reference Element tool bar 2
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This curve can now be used to extrude a rib or create a slot
Create the 3D curve by using the 3D Curve tool in the Free-Style workbench
Instructor Notes:
Explain that in this example the Free-Style workbench is accessed to create a 3D Curve through 3D Points defined earlier in the Part Design workbench. Note that the 3D Points could just have easily been created using the Free-Style workbench– they are the same points, using the same dialogue box and ending up in the same location of the Specification Tree. Emphasize that these elements are available in the Part Design workbench simply for convenience. Note that a 3D Spline could also have been created using the Wireframe and Surfaces or Generative Shape Design workbenches to support development of the Rib or Slot feature in Part Design.
Solicit questions from the students on the use of Reference Elements in the Part Design workbench.
When questions have been answered, continue on to Solid Extruded Features Not Normal to the Sketch Plane…
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Part Design
Holes/Pads not Normal to Sketch Plane
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You will learn how to create Holes, Pockets or Pads with a direction of extrusion not perpendicular to their sketch
Instructor Notes:
In this section, you will learn how create Holes, Pockets and Pads that have an Extruded Direction that is Not Normal to the Sketch Plane…
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Part Design
What are Holes/Pockets/Pads not Normal to the Sketch Plane ?
Some Key Points:
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• When creating a hole, a pocket or a pad, the default result is perpendicular to the sketch you have selected to get these features • It is possible to define another direction. You specify it in the Direction field • The selected direction must neither be in a plane parallel to the sketch plane nor in the same plane
Instructor Notes:
Remind the students that the default behavior for many Sketch-Based extruded Solid Features is to assume the Extruded Direction is Normal to Surface (Sketch Plane or Planar Surface of the elements being extruded). This behavior can be changed by unchecking the Normal to Profile option. Point out that by unchecking this option, you must select an appropriate 3D Reference Element (Plane or Line) that defines the desired direction. Note that the Reference Element cannot be one that is positioned Parallel to the Sketch Plane or in the same Plane as the Sketch Plane (resulting in impossible extrusion or zero length extrusion).
Let’s look at using Reference Elements for defining Extruded Direction in a little more detail…
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Part Design
Holes/Pockets/Pads not Normal to Sketch Plane 1
If a Pad or Pocket, select Profile sketch to be used
2
Select the appropriate icon
3
For this geometry, modify definition to include type “Up to Plane” and select
4 Changes the extrusion direction
You get:
Select limit surface on part
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5
De-Select “Normal to Sketch” and select reference
Instructor Notes:
Use this graphic to explain how a Pad is extruded from a Sketch using a 3D Line to establish the Extruded Direction. Point out how the Up to Plane option is used to dress up the First Limit of the new Pad. Explain to the students that in these examples, we have used the Pad feature to highlight how the Reference Direction for Extrusion can be modified. This same functionality applies to Pockets, Holes and other extruded Sketch-Based features.
Solicit questions from the students about modifying the Extruded Direction of SketchBased features.
When questions have been answered, move on to Creating Pads and Pockets from Surfaces…
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Part Design
Creating Pads and Pockets from Surfaces
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You will learn how to create Pads and Pockets from Surfaces
Instructor Notes:
In this section, you will learn how to develop a Pad or Pocket solid feature directly from a Surface…
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Part Design
How to Create Pads and Pockets from Surfaces ? You can extrude surfaces in any direction. Images below show you how to create pads from surfaces. The same method can be applied to pockets.
Up to Plane
Up to Last
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Pocket from a Surface (Up to Plane)
Up to next
Instructor Notes:
Explain the different methods of defining a Pad or Pocket Limits. Point out how a Surface can be selected as the Profile element for a Pad or Pocket and be Extruded to create the Solid feature. Note that when a Non-Planar Surface is selected for creation of the Pad or Pocket, you will be asked to define the Reference Direction for extrusion.
Let’s examine this process in more detail…
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Part Design
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Creating Pads and Pockets from Surfaces (1/2) 1
Select the Surface to be extruded.
2
Select the Pad icon.
3
The Pad Definition dialog box appears. Select the “Up to surface” limit and the surface of your choice. According to the example, you can use another limit type (Dimension limit, Up to next, Up to last, Up to plane …)
Instructor Notes:
Explain how the Extruded Surface is used to Create the Pad. Note that since this is a Non-Planar Surface, you will be asked to define a Reference Direction for the Pad extrusion. After the Reference Direction has been defined, all options for Limit Type are available for use (Dimension, Up to Next, Up to Last, Up to Plane, Up to Surface).
Let’s see one of this options being enforced…
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Part Design
Creating Pads and Pockets from Surfaces (2/2) Expand the dialog box. Click the Reference Field and select the extrusion direction.
5
Enter the first and the second limit values and click OK to confirm.
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4
Instructor Notes:
Explain how the Pad is extruded from one Surface to another Suface using the Up to Surface Limit Type. Point out that while you have been looking at the creation of Pads using Surfaces, the same process applies to creating Pockets from Surfaces.
Solicit questions from the students about Creating Pads and Pockets from Surfaces.
When questions have been answered, move on to Creating Surface-Based Features…
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Part Design
Surface-Based Features
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You will learn how to create advanced types of Surfaced-Based feature: Split, Thick Surfaces, Close Surfaces and Sew Surfaces.
Instructor Notes:
You will now learn how Surfaces can be incorporated into Solids during your Part Design processes…
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Part Design
What is a Surface Based Feature and When to Use It (1/2) ? There are four Surface Based Features • Split: Used to split a solid with either a plane or a surface.
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• Thick Surface: Used to create solids from surfaces. Material can be added from either or both sides of the surface
Instructor Notes:
Explain the four different types of Surface-Based Features and how they are accessed from the Part Design workbench. On this page, you see two of these features: Split and Thick Surface…
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Part Design
What is a Surface Based Feature and When to Use It (2/2) ? • Close Surface: Used to take a closed surface and turn it into a solid.
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• Sew Surface: Used to glue a surface feature to an existing 3D solid.
Instructor Notes:
Explain the purpose of Close Surface and Sew Surface in the development of Solids. Let’s look at each of these four Surface-Based Features in more detail…
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Part Design
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Split 1
Select body to be split
3
Select the splitting element
An arrow pointing to the material to keep appears. Click on it to reverse the direction if needed
2
Select Split icon
You can split a body with a plane, face or surface. A typical use is where the internal structure must be trimmed and associated to an outer aerodynamic shape to allow rapid future change
Instructor Notes:
Explain the purpose of Split in modifying a solid so that it matches a surface. Point out that a Split is a feature that is stored in a Part Body even though the Splitting Surface is stored in an Open Body. Note that the Split operates against all Solid Features that come before it in the Part Body– any new solid features created after the Split are not subjected to the Split. Also note that the Splitting Element can be a plane or face.
Now let’s look at the Thick Surface feature…
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Part Design
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Thick Surface 1
Select the surface to be thickened.
2
3
Enter the offset thickness values.
4
Select the Thick Surface icon.
Second thickness value. First thickness value. The resulting feature does not keep the color of the original surface.
Instructor Notes:
Explain how Thick Surface is used to create a solid feature from a 3D Surface by applying thickness to it. Point out that the direction of applied thickness is normal to the surface in either of two directions. This direction cannot be overridden. Note that there is a First Offset and Second Offset field in the dialogue box that allows for different thicknesses to each side. Note the feature in the Specification Tree.
Let’s now look at the Close Surface feature…
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Part Design
Close Surface Select Close Surface icon
3
Closed Surface appears in specification tree
2
Select surface to be closed
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1
Instructor Notes:
Explain the purpose of the Close Surface in creating a solid by filling in a Surface. Point out that if any openings in the surface are not Planar, you cannot create a Close Surface from it. In this case, you would have to create another surface that accounts for the nonplanar opening using the Wireframe and Surfaces or similar workbench. Note the Close Surface feature in the Specification Tree.
Let’s now look at Sew Surface…
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Part Design
Sew Surface 1
3
Select the Sew Surface icon
2
Select the surface to sew
The Final solid is as follows
An arrow pointing to the material to keep appears. Click to change the direction if needed.
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Two options are available in the Dialog Box : Intersection and Simplify geometry. After clicking on the Intersection option, the Surface will be glued to the existing 3D Solid even if this Surface intersects the Solid.
Sewing means joining together a surface and a body. This capability consists in computing the intersection between a given surface and a body while removing useless material
Instructor Notes:
Explain the purpose of Sew Surface. Point out that this illustration uses the Intersection option. Point out the effect of this “Glued” method for development of the solid. Note that using this feature will not only remove useless material, but will also add material between the reference surface and the solid if any gaps exist.
Let’s practice creating these Surface-Based Features…
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Part Design
3D Constraints
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You will learn how to use 3D constraints
Instructor Notes:
Now you will learn how to use 3D Constraints to position Part features…
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Part Design
What is a 3D Constraint ? A 3D Constraint is the same as any other constraint only that it is applied in the 3D model itself. Basically you will note that some are reference type constraints and others are regular constraints. Creation is the same as in the Sketcher, so we will concentrate on their usage here
Reference constraints are shown in parenthesis and cannot be modified
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They are references because there are other constraints that are constraining the geometry
Normally, 3D constraints are modifiable and can be linked and driven as others are in the Sketcher
Instructor Notes:
Explain the nature of 3D Constraints and note that they are the same constraints as you apply in Sketcher except that they are created in the 3D environment instead of on a Sketch Plane. Point out that many 3D features are already constrained in the way they were created (based on Sketch Planes or other dependencies) and so cannot be further constrained using 3D Constraints. Note that where a feature is already constrained in other ways, the 3D Constraint is created as a Reference. Further emphasize that Isolated features that have no other constraints are candidates for positioning with 3D Constraints.
Let’s see where it is appropriate to use 3D Constraints…
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Part Design
When to Use 3D Constraints ? They can be used whenever you have 3D geometry that you want to link to some type of 3D datum plane or surface
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They are also useful when you need to drive the location of a piece of geometry created earlier in the design from a piece of geometry created later in the model. Thus this will limit some of the need to re-ordering of the part You may also find it useful when you are using Copy and Paste to locate the pasted piece of Geometry from where you wish
Instructor Notes:
Review some of the mentioned instances where 3D Constraints may be used. Point out that 3D Constraints are also useful for positioning different Part Bodies relative to each other. Also note that when a Sketch-Based featur has its Sketch Isolated from the orginal Sketch Plane, then that feature can be positioned with a 3D Constraint.
Let’s see how to create some 3D Constraints…
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Part Design
Creating 3D Constraints 1
Select the Constraint icon and create a constraint between the left side face and the hole on the left side of the part
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2
Now, Create one more 3D constraint between the same face and Hole on right side
The first dimension created was not a ‘reference’ dimension. No Parenthesis were on the value. The second dimension was a ‘reference’ dimension because the sketch of right side hole is constrained from right side face.
Instructor Notes:
Explain that the first hole is not constrained by Sketch Constraint, so it is available to be driven by a 3D Constraint. Point out that the only benefit of the 3D Constraint in this case is to make it easier to adjust the Hole position without having to access its underlying Sketch. Note the Reference Constraint generated for the second hole since it is already constrained by its Positioning Sketch.
Let’s look at 3D Constraints a little further…
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Part Design
Using 3D Constraints 1
You will drive the location of Pocket.1 from Hole.2 created after it in the tree
2
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3
Create the two constraints shown below from the center line of Hole.2 to the edges of the Pocket.1
Modify the constraint indicated in red to 25mm and the Pocket.1 is now driven from the Hole.2 location
Note: This capability will allow you to drive location of features in the tree from features created after them without having to do re-location of features in the tree.
Instructor Notes:
Explain the process of driving the Pocket and Hole features using 3D Constraints. Point out that these features are not constrained on their Sketches and that is why 3D Constraints can be used in this case.
Let’s practice creating some 3D Constraints…
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Part Design
Using 3D Elements Recommendations
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You will see some hints, tips and advices about tools seen in the lesson
Instructor Notes:
You will now review some recommendations to make your use of 3D Elements in Part Design more efficient…
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Part Design
Defining Local Axis Local Axis dialog box
To define the axis system origin To define the OX axis To define the OY axis To define the OZ axis
To reverse the OX axis
To reverse the OY axis To reverse the OZ axis
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To expand the dialog box
Instructor Notes:
Explain some of the options available for defining a Local Axis System. Point out that Contextual Menus are available for creating support geometry to define the Origin and any Axis. Note the More button that provide more fields to adjust the position and orientation of the Local Axis.
Let’s look at some more recommendations…
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Part Design
Creating Midpoint or Endpoint to Define Axis System Origin You can define Endpoints or Midpoints as origin points of Axis Systems.
1
Select the Insert -> Axis System command or click on the Axis System icon.
3
2
The Axis System Definition dialog box is displayed.
5
With the option Create Endpoint : the origin point corresponds to the endpoint detected by the application after selection of a geometrical element.
Use the contextual commands available from the Origin field to define the origin point. You can see that two new options have been added in V5R10 : Create Midpoint and Create Endpoint.
4 With the option Create Midpoint : the origin
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point corresponds to the midpoint detected by the application after selection of a geometrical element.
Instructor Notes:
Explain the use of these Contextual Menu options when defining a Local Axis System. Note the value and efficiency of Contextual Menus to aid in the Part Design process.
Solicit final questions from the students on the use of 3D Elements in Part Design.
When questions have been answered, summarize what you have learned in this section…
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Part Design
Using 3D Elements to Create a Part: Recap Exercises You will Practice the concepts learnt in this lesson to build a exercise following a recommended process.
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Curved Mating Piece
Instructor Notes:
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Part Design
Curved Mating Piece Using 3D Elements to create a part: Recap Exercise 25 min
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In this exercise you will: Design the part to connect two different components. A reference surface is provided. Create a pad using the surface provided. Create 3D wireframe elements to assist designing of the mating Rib. Create Axis system and 3D points to locate tapered holes. Apply fillets.
Instructor Notes:
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Part Design
Angle Bracket Part Design Fundamental Exercise 40 min
In this exercise you will build the Angle Bracket by following a recommended process. You will first understand the design intent of the Angle Bracket and identify its functional features. You will then study its Drawing in detail to understand the dimensions and specifications. Finally,you will design the various functional features of the Angle Bracket according to specifications and by making use of wireframe elements. Here you will :
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Design the base pad. Design the thin pad. Apply Fillets. Design bracket pad. Design pilot and Bracket Holes.
Instructor Notes:
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Part Design
To Sum Up This concludes the lesson on Using 3D elements to create Part
Local axis is used to define local co-ordinates . It is helpful create elements in reference with local system rather than absolute system. Points,Lines and planes are used as reference elements to facilitate design.They also used for effective parent-children management. You have seen how to create holes in a direction other than the direction Normal to sketch using 3d elements and also how to generate Pads and Pockets from surfaces. In surface based features you have seen close surface,split surface,Thick surface and fill surfaces.
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Split Surface :Used to split solid with a surface or a plane. Thick surface:Used to create solids from surfaces by adding material in both the directions. Close surface :Used to create a solid by closing a surface . Sew surface:Used to glue a surface to a solid.
Instructor Notes:
Summarize what you have learned in the use of 3D Elements to create a part.
Continue on to the next section: Dress-Up Features…
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Part Design
Sketch-Based Features You will learn how to create advanced sketch-based features
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Introduction to Sketch-Based Features Creating Ribs and Slots Creating Stiffeners Creating Multi-sections Solid Sketch Based Features Recommendations Sketch Based Features: Recap Exercises Sum Up
Instructor Notes:
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Part Design
Introduction Following advanced tools are Sketch Based and allow you to create complex parts:
Ribs and Slots: These tools allow you to create complex ribs and slots on existing solids or to create pipes:
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Stiffeners: This tool is useful when you want to rigidify a thin solid:
Multi-sections Solids This tool is used to create complex solid using a set of sections
Instructor Notes:
In this section of the course, we will review a variety of advanced sketch-based features. This include Ribs, Slots, Stiffeners and Lofts. We will also look at how we can create a Combine solid feature that uses two or more sketches for its definition.
Let’s look at these solid features in more detail…
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Part Design
Creating Ribs and Slots You will learn how to create Ribs and Slots
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RIB
SLOT
Instructor Notes:
We will now review the process of creating Rib and Slot solid features…
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Part Design
What is a Rib A Rib is a profile swept along an open or closed Center Curve to create a 3D feature The profile can be swept along an open or a closed center curve to create the feature.
Profile Center curve
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The profile of the Rib can be controlled by simply using one of the 3 choices under the Profile control section of the window
The center curve does not have to extend to the end, merge Ends can be used to extend or shorten the rib to its proper wall.
Instructor Notes:
A Rib is similar to a Pad in that a positive solid feature is created. However where a Pad can be extruded along only a single direction, a Rib is swept along a Center Curve. This provides you with a means of deriving a more complex solid feature than can be created with a Pad. The Center Curve can be defined using a second sketch or it can be a curve created using the Wireframe and Surfaces workbench. The Center Curve can be defined as open or it can be closed. The Merge Ends option provides a means of extending the Rib to adjacent solid features if the Center Curve does not intersect them. Note that if the Center Curve is planar (such as with a sketch) then the elements that comprise the curve do not have to be continuous in tangency. However if the Center Curve is not planar (such as with 3D curves) then the elements comprising the curve must be continuous in tangency. As the Profile is swept along the Center Curve, there are three options for controlling the Pulling Direction that will affect the resultant solid feature: Keep Angle (default): keeps the angle value between the sketch plane used for the profile and the tangent of the center curve. Pulling Direction: sweeps the profile with respect to a specified direction. Reference Surface: the angle value between axis h and the reference surface is constant. Now let’s see what a Slot feature is and how it’s created…
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Part Design
What is a Slot A Slot is a profile that is swept along an open or closed Center Curve to remove material from a solid
The profile can be swept along an open or a closed center curve to remove the material.
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The profile of the Slot can be controlled by simply using one of the 3 choices under the profile control section of the window
The center curve does not have to extend to the end, merge ends can be used to extend or shorten the slot to its proper wall
Instructor Notes:
A Slot is to a Pocket what a Rib is to a Pad. In this case, a negative solid feature is created that removes material. As with the Rib, a Slot is a profile that is swept along a Center Curve. The Center Curve can be defined using a second sketch or it can be a curve created using the Wireframe and Surfaces workbench. The Center Curve can be defined as open or it can be closed. The Merge Ends option provides a means of extending the Rib to adjacent solid features if the Center Curve does not intersect them.
Note that if the Center Curve is planar (such as with a sketch) then the elements that comprise the curve do not have to be continuous in tangency. However if the Center Curve is not planar (such as with 3D curves) then the elements comprising the curve must be continuous in tangency.
As the Profile is swept along the Center Curve, there are three options for controlling the Pulling Direction that will affect the resultant solid feature: Keep Angle (default): keeps the angle value between the sketch plane used for the profile and the tangent of the center curve. Pulling Direction: sweeps the profile with respect to a specified direction. Reference Surface: the angle value between axis h and the reference surface is constant. Note that both Rib and Slot provide the Thick option to create Thin features as is also available with other Part Design solid features. Let’s find out when we might use Ribs and Slots to aid in the development of solids…
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Part Design
When Should We Use Ribs and Slots You will find Ribs useful when you need to sweep profiles from one surface to another. Ribs and Slots will also be useful to create complex walls of parts that have many details in them. Here you can control complexity in one sketch and does not require many small sketches or geometric features to work with.
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Also a Rib can be used to create a pipe by sweeping a profile along a center curve.
Instructor Notes:
Explain how Ribs and Slots provide a means to create more complex solid shapes using a couple of inputs (Profile and Center Curve) and Pulling Direction controls. This means that more complex geometry can be created and later modified in a more efficient manner by reducing the number of inputs required to manage the result. While CATIA also has Tubing, Piping and other distributive system design tools, Ribs can be used to create solids that can be used in their stead. The Thick option would allow you to even create hollow pipes, tubes, etc. In Mechanical Part Design, the use of Ribs and Slots means fewer steps to create certain part features.
Let’s look at the creation of Ribs and Slots in a little more detail…
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Part Design
How to Create a Simple Rib 1
2
Set the Pulling direction by selecting the indicated surface
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3
Select the Rib icon.
4
Select the Profile to be swept and the 3D center curve along which it will be swept.
Click OK to validate the Rib
The 3 Dimensional curve was created in the Wire Frame workbench.
Instructor Notes:
Have the students create a simple Rib using this part document. Point out that the Center Curve (Join.1) was created using the Wireframe and Surfaces workbench. This curve could also have been created using an Extract from the solid (with Tangency Propogation) to get the same result.
Let’s now create a Simple Slot...
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Part Design
How to Create a Slot 1
Select the Slot icon
2
Select the Profile to be swept and also the path along which slot will be creates.
The depth of the profile must be equal to or less than the radius of the Center Curve.
The Result is:
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3
Instructor Notes:
Have the students create a simple Slot using this part document. Point out that the Center Curve is planar (Sketch.3) but could have been created using the Wireframe and Surfaces workbench as a 3D curve. Note that since material is removed by the Slot feature, the Profile depth must be equal to or less than the radius of the Control Curve in order to render a valid result.
Let’s now look at using the Thick option to create Thin Ribs and Slots...
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Part Design
Creating Thin Ribs and Slots (1/3) Thin Ribs and Slots are resulting features from adding thickness to both sides of Rib’s and Slot’s profiles.
You then obtain your Thin Rib or Slot.
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You can create a Thin Rib or Slot after checking the Thick Profile option
Instructor Notes:
Point out the use of the Thick Profile option that is available in the Rib and Slot dialogue boxes. This option works the same as for Pads, Pockets and other Part Design solid features...
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Part Design
Creating Thin Ribs and Slots (2/3) 1
Select the Rib icon
2
Select the Profile you want to sweep and the Center curve in the Rib definition Dialog Box.
3
Enter values for Thickness1 and Thickness2. You can see that material is added on both sides.
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4
To define Thin Rib check Thick Profile option
Instructor Notes:
Note that the Thick Profile option allows you to add different Thickness values to each side of the Profile (Thickness1 and Thickness2).
Let’s see some more options that affect the Thick Profile...
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Part Design
Creating Thin Ribs and Slots (3/3) 5
To add material equally to both sides, check Neutral Fiber. The thickness1 you defined is now distributed equally. Note that Thickness2 is not available.
If you click on the “Merge Ends” option, you will trim the Rib to existing material.
6
Click OK to create your Thin Rib.
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This task can also be applied on Slots . The Thin Slot looks like this.
Instructor Notes:
Note that when the Neutral Fiber option is checked, Thickness 1 is equally applied to both sides of the Profile. Point on the purpose of the Merge Ends option in trimming a Rib or Slot.
Now let’s complete a final practice of creating Ribs and Slots...
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Part Design
Creating Stiffeners
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You will learn how to create Stiffeners
Instructor Notes:
In this section, you will learn how to create Stiffener features to support your development of Part designs…
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Part Design
What is a Stiffener ? A Stiffener is a brace or rib that is added to a wall or a stand-off to strengthen them so as to prevent breakage. It is commonly found on molded plastic parts or castings
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These two arrows are used to control the width of the part, which can be either symmetrical or only on one side.
As with most features you can now access the sketch directly by selecting this button. The other arrow is used to control the direction of the rib.
Instructor Notes:
Explain the purpose of the Stiffener tool in creating solid features such as braces, brackets, etc. to strengthen the wall or other aspect of a part. Note that these features could also be created using the Pad tool or other Part Design tools, but the Stiffener tool provides a creation method specific to these types of part features. Note that Stiffeners only use Open Profiles for their definition. Depending on the Mode of creation selected, the Stiffener will automatically trim to the adjacent solid features.
Let’s see where the Stiffener feature might be used…
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Part Design
When Should we Use Stiffeners ?
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They can be used when you have a thin wall that you want to be more rigid without increasing the thickness of the wall
They can also be used for tall objects that are used to locate or support other objects and you want to prevent them from breaking off the surface they are attached to
Instructor Notes:
Explain Stiffener features are most commonly used to support the development of plastic or casted parts where additionally rigidity to support thin walls, long standoffs, etc. may be necessary.
Solicit feedback from the students as to where this feature might be used in the types of parts that their company designs and/or manufactures.
Let’s look in more detail at how Stiffeners are created…
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Part Design
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Creating Stiffeners (1/2) 1
Select the Stiffener Icon
2
3
The Stiffener Definition Dialog box is displayed. Two Creation Modes are available : ‘From Side ‘and ‘From Top’.
Select the sketch
You will find that in many cases you need to add a small line segment on to the top of the angled line used to create your stiffener. This allows for a coincidence constraint to be created between the rib and the part.
Instructor Notes:
Explain how an Open Profile is used in the creation of the Stiffener. Emphasize how constraints applied to a Sketch Profile can maintain the validity of the Stiffener feature when changes are made to the surrounding wall features. Also point out how the profile could be comprised of a Wireframe curve feature. Note the default option for Neutral Fiber and explain its interaction with the Thickness1 and Thickness2 parameters.
Let’s look at the two Mode options for creating a Stiffener…
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Part Design
Creating Stiffeners (2/2) 4
The ‘From Side’ option is the default one in CATIA. It is used to create “former” Stiffeners. The extrusion will be made in two Directions if the Neutral Fiber is uncheked, otherwise in three Directions. Select the thickness value. If the direction is correct select OK to create the Stiffener.
The option ‘From Top’ allows you to create Stiffeners from a Network. It is never done with respect to the Creation order Profile. The extrusion is performed normal to the Profile’s Plane and the Thickness is added in the Profile Plane.
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Instructor Notes:
Explain the two different Modes of Stiffener creation: From Side: the extrusion is performed in the profile' s plane and the thickness is added normal to the plane. From Top: the extrusion is performed normal to the profile' s plane and the thickness is added in the profile' s plane.
Let’s practice creating Stiffener features…
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Part Design
Creating Multi-sections Solid You will learn how to create Multi-Sections Solids and Removed Multi-Sections Solids
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Creating Simple Multi-sections Solids Remove Multi-sections Solids Coupling Changing the Closing Point
Instructor Notes:
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Part Design
Creating Simple Multi-sections Solids
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You will learn how to create Multi-sections Solids
Instructor Notes:
Now we will learn how to create simple Multi-sections Solid features in Part Design…
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Part Design
What is a Multi-sections Solid? A Multi-sections Solid can be a Positive (add material) or Negative (subtract material) solid that is generated by two or more planar sections swept along a spine. In P1 configuration, only two sections Multi-sections Solid can be created.
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Directional arrows are provided to get the proper orientation of the Multi-sections Solid. The Planar sections can be connected with Guide Lines. Note that Closing Points on the sketch must be aligned to get the proper orientation of the sections otherwise the Multi-sections Solid gets twisted.
Instructor Notes:
Review the process of defining Multi-sections Solids and point out that the Multi-sections Solid can be a positive solid feature or a negative solid feature (Removed Multi-sections Solid). Explain that a Multi-sections Solid is swept through a series of Planar Sections. A Spine for the Multi-sections Solid is automatically computed, based on the postions of the Sections relative to each other. A Spine can also be created to override the Computed Spine. Guides, Couplings and Relimitation can also be defined to give finer control over the resultant Multi-sections Solid. Explain to the students the relationship of Closing Points and Direction on each Profile.
Note that the P1 Configuration provides for Multi-sections Solid creation through two Sections only.
Let’s look at when you might use a Multi-sections Solid in Part Design…
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Part Design
When to Use Multi-sections & Removed Multi-sections solids Multi-sections Solids can be used for several reasons: To create complex solids.
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To create some transition geometry between two existing solids in a part
Removed Multi-sections Solids are used the same way when you want to subtract a transitioned surface from another solid.
Instructor Notes:
Explain the different reasons why a Multi-sections Solid or Removed Multi-sections Solid might be created. Point out the use of Multi-sections Solids to provide a transition solid feature between the planar faces of two other solid features within a part.
Let’s see how Guides affect the definition of a Multi-sections Solid or Removed Multisections Solid…
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Part Design
Multi-sections Solid Creation: Guide Lines 1
Select the Multi-sections Solid icon
3
Select the Guide tab from the dialog box
2
Select the sections through which the Multisections Solid is going to pass. The order in which you select the sections is important, it will define the order of connection between the sections
(2a) (2b)
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4
(2c)
Select the Guide lines
The Multi-sections Solid passes through the sections and it is limited by the guide lines
Instructor Notes:
Explain the effect of Guides on the definition of the Multi-sections Solid feature as it passes through its Sections. Note that a Guide must intersect each Section of the Multisections Solid. Point out the relationship between Guides and the Spine in computing how the Multi-sections Solid is formed through the Sections. Note that Guides can be Replaced, Removed or Added at any time.
Let’s take a closer look at how the Spine controls the Multi-sections Solid definition…
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Part Design
Multi-sections Solid Creation : Spine 1
Select the Multi-sections Solid icon
2
Select the sections the Multi-sections Solid is going to pass through. The order in which you select the sections is important, it will define the order of connection between the sections
(2b) (2c)
(2a)
3
Select the Spine tab from the dialog box
4
Select the Spine
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Spine
From the first to the last section, the solid is generated by doing a sweep along the spine. The sections always stay fix in space
Instructor Notes:
Explain how the Spine is automatically computed from the Sections you select to make the Multi-sections Solid. This example shows a Computed Spine connecting the Origin Points of each Sketch profile. Note how you can create a Spine element (or other type of Curve) and use it to override the Computed Spine. Point out that Spines can be replaced at any time to modify the Multi-sections Solid. If a selected Spine is removed, the Multi-sections Solid will revert to a Computed Spine.
Let’s look at how Closing Points and Orientation control the Multi-sections Solid…
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Part Design
Multi-sections Solid Creation: Closing Point & Orientation
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Closing point of the section
Orientation of the section
To change the closing point of a section, select another point on this section
When selecting another section, it might happen that the section is orientated in the other direction than the previous one, so, to reverse the section orientation select the arrow which indicates the section orientation
Instructor Notes:
Explain how Closing Points are used to control the sweep of the Multi-sections Solid through the Sections. Note the importance of Orientation in preventing a twisted Multisections Solid. Point out that a Contextual Menu is available to change the default Closing Points if necessary.
Let’s look at how Tangent Surfaces can be used to develop the Multi-sections Solid…
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Part Design
Multi-sections Solid Creation : Tangent Surfaces
1
Select the first section
2
Select the surface (corresponding to the first section) the Multi-sections Solid will be tangent to
3
Select the intermediate sections
4
Select the last section
5
Select the surface (corresponding to the last section) the Multi-sections Solid will be tangent to
6
Validate
You get : Result with the same sections but without any tangent surfaces (2)
(3)
(4)
(5)
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(1)
Instructor Notes:
Explain the use of Tangent Surfaces to develop the Multi-sections Solid. Note that Tangency can be defined on any Section but can conflict with Guide or Spine definitions. In this example, no Guides havfe been defined and the Spine is computed.
Solicit questions from the students about the Multi-sections Solid feature.
Once questions have been answered, move on to Removed Multi-sections Solids…
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Part Design
Removed Multi-sections Solids
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You will learn how to create Removed Multi-sections Solids
Instructor Notes:
Now we will look at how we can use Multi-sections Solids to Remove material from a Part Body…
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Part Design
What is Remove Multi-sections Solid Material ? The Removed Multi-sections Solid capability generates Multi-sections Solid material, by sweeping one or more planar section curves along a computed or user-defined spine, and then removes this material. The material can be made to respect one or more guide curves
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In P1 configuration, only two sections Multi-sections Solid can be created.
Instructor Notes:
Explain how Removed Multi-sections Solid is identical to the Multi-sections Solid previously discussed, except that it is a negative feature that removes material from the solid. Note that all aspects of a Multi-sections Solid (Planar Sections, Guide Curves, Spine, etc.) are present in the Removed Multi-sections Solid feature.
Let’s look at this process in a little more depth…
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Part Design
Remove Multi-sections Solid Material
1
Select the Remove Multi-sections Solid Material icon
2
3
Select OK
Select the sections the Multi-sections Solid is going to pass through. The order in which you select the sections is important, it will define the order of connection between the sections (You could have defined a spine or several guide lines, if no spine is selected, the system computes a spine for you)
(2a) (2b)
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(2c) (2e)
(2d)
Instructor Notes:
As with the Multi-sections Solid feature, Removed Multi-sections Solid automatically computes the Spine through the selected Sections. Explain that you can define Guides or a non-computed Spine as you did with the Multi-sections Solid feature.
Let’s look at Closing Points and Orientation on the Removed Multi-sections Solid…
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Part Design
Closing Point & Orientation: Remove Multi-sections Solid
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Closing point of the section
Orientation of the section
To change the closing point of a section, select another point on this section
When selecting another section, it may happen that the section is orientated in the other direction than the previous one, so, to reverse the section orientation select the arrow which indicates the section orientation
Instructor Notes:
Explain that the use of Closing Points and Orientation direction around each Section is identical to the way these are defined in Multi-sections Solids.
Let’s look at Tangent Surface definitions that can be applied to Removed Multi-sections Solids…
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Part Design
Remove Multi-sections Solid Material : Tangent Surfaces
1
Select the first section
4
Select the last section
2
Select the surface (corresponding to the first section) the removed Multisections Solid will be tangent to 5
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You get :
(2)
(3)
(1)
(4)
3
Select the intermediary sections
Select the surface (corresponding to the last section) the removed Multisections Solid will be tangent to
6
Validate
Result with the same sections but without any tangent surfaces
(5)
Instructor Notes:
As was the case with the Multi-sections Solid features, Tangent Surfaces can be referenced by the end Sections to change the direction of the Multi-sections Solid at the ends. Explain that depending on the Spine and Guides definition, you may or may not be able to use a Tangent Surface on an end Section.
Let’s now look at how Couplings can change the development of a Multi-sections Solid or Removed Multi-sections Solid feature…
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Part Design
Coupling
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You will learn how to use Coupling when creating Multi-sections Solids
Instructor Notes:
You will now learn how to use Couplings to control the definition of a Multi-sections Solid or Removed Multi-sections Solid…
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Part Design
What is Coupling when Creating Multi-sections Solids? A Coupling tab in the Multi-sections Solid and remove Multi sections Solid functions allows you to compute the Multi-sections Solid using: The total length of the sections (ratio). The vertices of the sections. The curvature discontinuity points of the sections. The tangency discontinuity points of the sections.
Vertices, Curvature Discontinuity, Tangency Discontinuity
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Vertices, Curvature Discontinuity
Vertex
Instructor Notes:
Explain that Coupling curves can be generated between the Sections of the Multisections Solid in different ways: Ratio: the curves are coupled according to the curvilinear abscissa ratio. Tangency: the curves are coupled according to their tangency discontinuity points. Tangency then urvature: the curves are coupled according to their curvature discontinuity points. Vertices: the curves are coupled according to their vertices. If they do not have the same number of vertices, they cannot be coupled using this option. Point out that by default, Multi-sections Solids are coupled by the Tangency method. If the sections do not have the same number of Tangency Discontinuity Points, then this method cannot be used. Also note that Tangency then Curvature or Vertices methods also require that the sections be consistent in the number of points.
You can access all of these methods from the Coupling tag in the Multi-sections Solid or Removed Multi-sections Solid creation dialogue box…
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Part Design
Coupling when Creating Multi-sections Solids The Coupling tab in the Multi-sections Solid and Remove Multi-sections Solid functions allows you to specify the Multi-sections Solid computation type: - on the total length of the sections (ratio) - between the vertices of the sections - between the curvature discontinuity points of the sections - between the tangency discontinuity points of the sections 1
Activate the Multi-sections Solid icon and select and orient the sections. (2)
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(1)
2
Select the Coupling tab from the dialog box
3
Select the desired kind of coupling from the combo
4
Select OK
(3)
(4)
Instructor Notes:
Use this example to show the different options available for Section Coupling.
Let’s look at each of these options in more detail…
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Part Design
Coupling when Creating Multi-sections Solids: Ratio The Coupling tab in the “Multi-sections Solid” and “Remove Multi-sections Solid” functions can be used to compute the Multi-sections Solid using the total length of the sections (ratio) 1
Activate the Multi-sections Solid icon and select and orient the sections.
(1) (2)
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You get :
2
Select the Coupling tab in the dialog box
3
Select Ratio from the combo
(3)
(4) 4
Select OK
The solid is passing through the sections and the variation between the sections is computed by a ratio corresponding to the length of each section
Instructor Notes:
Explain the Ratio method of Section Coupling. Point out the resultant Multi-sections Solid solid from using this method.
Let’s look at this same Multi-sections Solid using the Tangency method…
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Part Design
Coupling when Creating Multi-sections Solids: Tangency The Coupling tab in the Multi-sections Solid and Remove Multi-sections Solid functions can be used to compute the Multi-sections Solid between the tangency discontinuity points of the sections 1
Activate the Multi-sections Solid icon and select and orient the sections.
(1) (2) You get:
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2
3
4
Select the Coupling tab from the dialog box Select Tangency Discontinuities from the combo
Click OK
(3)
(4)
The solid is passing through the sections and each section is split at each tangency discontinuity point. The solid is computed between each split section
Instructor Notes:
Explain the Tangency method of Section Coupling. Point out the resultant Multi-sections Solid solid from using this method and how it difers from the previous example.
Let’s look at this same Multi-sections Solid using the Tangency then Curvature method…
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Part Design
Coupling in Multi-sections Solids: Tangency then Curvature The Coupling tab in the Multi-sections Solid and Remove Multi-sections Solid functions can be used to compute the Multi-sections Solid between the curvature discontinuity points of the sections 1
Activate the Multi-sections Solid icon and select and orient the sections.
(1) (2)
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You get :
2
Select the Coupling tab from the dialog box
3
Select Curvature Discontinuities from the combo
4
Select OK
(3)
(4)
The solid is passing through the sections and each section is split at each curvature discontinuity point. The solid is computed between each split section
Instructor Notes:
Explain the Tangency then Curvature method of Section Coupling. Point out the resultant Multi-sections Solid solid from using this method and how it difers from the previous examples.
Let’s look at this same Multi-sections Solid using the Vertices method…
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Part Design
Coupling when Creating Multi-sections Solids: Vertices The Coupling tab in the Multi-sections Solid and Remove Multi-sections Solid functions can be used to compute the Multi-sections Solid between the vertices of the sections 1
Activate the Multi-sections Solid icon and select and orient the sections.
(1) (2)
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You get:
2
Select the Coupling tab in the dialog box
3
Select Vertices from the combo
4
Click OK
(3)
(4) The solid is passing through the sections and each section is split at each vertex. The solid is calculated between each split section
Instructor Notes:
Explain the Vertices method of Section Coupling. Point out the resultant Multi-sections Solid solid from using this method and how it difers from the previous examples.
Let’s take a closer look at Point Discontinuity (Tangency or Curvature) that is used in Coupling…
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Part Design
Coupling creation: Points of Discontinuity There are different types of point that CATIA can use to split the sections when creating Multi-sections Solids using coupling To have a look at the different types of discontinuity, we have sketched the profile shown below :
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Segments
Two arcs
These two points are tangency and curvature discontinuity points. They are also vertices
These two points are curvature discontinuity points. They are also vertices
This point is a tangency and curvature continuity point. This point is a pure vertex
Instructor Notes:
Use this example to explain how Tangency and Curvature discontinuities are detected when employing the different Coupling methods.
When these four methods of Coupling do not produce the desired Multi-sections Solid, then you can also Manually Couple the Sections…
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Part Design
Multi-sections Solid Manual Coupling (1/2) When the sections to be Multi-sections Solid ,do not have the same number of vertices you can define manual coupling instead of changing or creating additional closing points. 1
Activate the Multi-sections Solid icon, select the sections and the guide curves (if necessary, change the section orientation)
Section 3
2
Select the Coupling tab then set the Sections coupling to Ratio
Guide 2 Guide 3
Guide 1 Section 2 Section 1
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3
You get:
Double click in the Coupling field to display the Coupling window
Instructor Notes:
Explain how Manual Coupling gives you additional flexibility in creating a Multi-sections Solid between Sections that do no have the same Vertices, Tangency Points or Curvature Points. Show how to access and create Manual Couplings in the Multisections Solid or Removed Multi-sections Solid dialogue boxes.
Double-clicking in the Coupling definition window gives access to another dialogue box where you can define Manual Couplings…
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Part Design
Multi-sections Solid Manual Coupling (2/2) When the sections to be Multi-sections Solid ,do not have the same number of vertices you can define manual coupling instead of changing or creating additional closing points. 4
For each section select the vertex for the coupling. selection must be made in the same order in which the sections were selected.You can visualize the coupling curve if the corresponding option is checked.
Coupling curves are displayed in green
c b a Click OK to end Multi-sections Solid surface definition
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5
Instructor Notes:
Use the illustrations to explain how Manual Coupling is achieved. Note that more than one Manual Coupling can be defined. Point out the Display Coupling Curves check box and explain its purpose.
Not all points need to be coupled when using the Ratio mode of Section Coupling. Let’s see how we can visualize points that are not Coupled…
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Part Design
Manual Coupling: Displaying Uncoupled Points(1/2) For each coupling mode, the points that could not be coupled are displayed in the geometry with specific symbols 1
Select the two sections which have different number of vertices and have some discontinuity in curvature and tangency Section 2
Apply the different coupling modes one by one
Section 1
An error is issued every time
For each coupling mode, the points that could not be coupled are displayed in the geometry with specific symbols
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3
2
Instructor Notes:
Use this graphic to explain how to visualize Uncoupled Points on the Sections of a Multisections Solid. Explain how this is useful when performing Manual Coupling between Sections that do not have the same number of points. Since you can couple a point on one Section to more than one point on another Section (i.e. create multiple Couplings from a single point), you can then use Tangency, Vertices, etc. as Multi-sections Soliding modes between dissimilar Sections.
Finally, let’s look at how Relimitation can be affect the Multi-sections Solid…
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Part Design
Manual Coupling: Displaying Uncoupled Points(2/2) For each coupling mode, the points that could not be coupled are displayed in the geometry with specific symbols
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4a
Tangency mode
Tangency mode : uncoupled tangency discontinuity points are represented by a square
4b
Tangency then curvature mode
Tangency the Curvature mode : Uncoupled curvature discontinuity points are represented by an empty circle
4c
Vertices mode
Vertices mode : uncoupled vertices are represented by a full circle
Instructor Notes:
Use this graphic to explain how to visualize Uncoupled Points on the Sections of a Multisections Solid. Explain how this is useful when performing Manual Coupling between Sections that do not have the same number of points. Since you can couple a point on one Section to more than one point on another Section (i.e. create multiple Couplings from a single point), you can then use Tangency, Vertices, etc. as Multi-sections Soliding modes between dissimilar Sections.
Finally, let’s look at how Relimitation can be affect the Multi-sections Solid…
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Part Design
Multi-sections Solid Relimitation (1/3) By default the Multi-sections Solid surface is limited by the start and end sections. However you can choose to limit it on the spine or on the guide lines extremities
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When the limitation option is checked, the Multi-sections Solid is limited to the start or (and) end sections even is a larger spine or guide curves have been used
Note: This is also possible with the Remove Multi-sections Solid command
Instructor Notes:
Explain how the Multi-sections Solid or Removed Multi-sections Solid is limited to the Start and End Sections by default. Use this illustration to show a default Multi-sections Solid Relimitation.
When you uncheck the default Limitation option, the Multi-sections Solid will relimit on the Spine or Guides…
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Part Design
Multi-sections Solid Relimitation (2/3) By default the Multi-sections Solid surface is limited by the start and end sections. However you can choose to limit it on the spine or on the guide lines extremities
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When the limitation option is unchecked, and when a spine has been used, the Multi-sections Solid is limited by the spine extremities
Note: This is also possible with the Remove Multi-sections Solid command
Instructor Notes:
Explain how the Multi-sections Solid will relimit on the Spine, if it has been defined. This will not work with the Computed Spine, since it is calculated between the Sections. If no Spine or Guides exist, then you must Relimit on the End Sections.
If Guides do exist…
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Part Design
Multi-sections Solid Relimitation (3/3) By default the Multi-sections Solid surface is limited by the start and end sections. However you can choose to limit it on the spine or on the guide lines extremities
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When the limitation option is unchecked, and when guide lines have been used, the Multisections Solid is limited by the guide lines extremities
Note: This is also possible with the Remove Multi-sections Solid command
Note: If a spine an guide lines have been used the Multi-sections Solid will be limited on the shorter line
Instructor Notes:
If Guides exist in the Multi-sections Solid definition and the Section Relimitation options are deactivated, the Multi-sections Solid will relimit along the Guides. Point out that if both a Spine and Guides exist, then the Multi-sections Solid will Relimit on the shorter element.
Let’s see how Changing the Coupling Point affects the Multi-sections Solid…
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Part Design
Changing the Closing Point
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You will learn how to change the closing point when creating a Multi-sections Solid
Instructor Notes:
Let’s see how Changing the Closing Point affects the Multi-sections Solid definition…
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Part Design
What is Changing the Closing Point when Creating Multisections Solids ?
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When selecting the sections to create a Multi-sections Solid (or remove Multi-sections Solid), you can change the closing point after the selection of the sections and you can create a closing point anywhere on a section profile
Instructor Notes:
Explain how to change Closing Points during the process of selection the Sections that define the Multi-sections Solid. Note that any point on a Section profile can be used as the Closing Point for that Section. Orientation is indicated by a Direction arrow from the Closing Point. Orientations between Sections must be consistent in order to derive a Multi-sections Solid.
Let’s look at Closing Points in more depth…
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Part Design
Changing the Closing Point in Multi-sections Solids (1/6) 1
Activate the Multi-sections Solid icon and select the first section
2
Select the second section
3
Select the third section
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First section
Instructor Notes:
In this example you will learn how to change the Closing Point when creating a Multisections Solid. As each Section of the Multi-sections Solid is selected, a default Closing Point and Orientation direction is established. These may not be consistantly located or oriented between the Sections, depending on how the Profiles were created…
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Part Design
Changing the Closing Point in Multi-sections Solids (2/6) 4
Click on Section2 (Label)
5
Select Replace Closing Point in the contextual menu, then select a new closing point (5)
6
Click on Section3 (Label)
7
Select Replace Closing Point from the contextual menu, then select a new closing point (7)
8
Select the arrows to reverse Section2 and Section3
(8)
(5)
(7)
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(6)
(4)
Instructor Notes:
Explain that a Contextual Menu is available in the dialogue box when you right-click on the name of a Section. This Contextual Menu gives access to the Replace Closing Point menu. A new Closing Point for the Section can now be selected…
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Part Design
Changing the Closing Point in Multi-sections Solids (3/6) 9
Check that the coupling is at Ratio then Select Preview in the dialog box
You can see that the solid is twisted because the default closing point of Section1 is not aligned with the closing points of the other sections
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(9)
Instructor Notes:
Explain the relationship between Closing Points between Sections and the importance of that relationship in generating a satisfactory Multi-sections Solid…
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Part Design
Changing the Closing Point in Multi-sections Solids (4/6) 10
In order to create a closing point on Section1, select the Section1 label with MB3, then select Remove Closing Point
11
Then again, select Create Closing Point in the contextual menu
A new dialog box is displayed corresponding to the point creation on a curve
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(11)
The point appears in blue before validation
(10)
Instructor Notes:
Explain how the Contextual Menu also gives access to menus that allow you to Remove, Replace or Create a Closing Point. The Create Closing Point menu takes you into the Point Definition dialogue box where you can then create the necessary geometry to support a new Closing Point…
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Part Design
Changing the Closing Point in Multi-sections Solids (5/6)
Select the Distance on curve option
13
Select the Geodesic option and Enter 100 as the Length
14
Select OK
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12
Instructor Notes:
Self-Explanatory dialogue for creating the new Closing Point…
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Part Design
Changing the Closing Point in Multi-sections Solids (6/6)
16
Select the Coupling tab
17
Select Vertices option from the combo
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You get :
18
Select OK
Instructor Notes:
The end result of the Multi-sections Solid after Changing the Closing Point. Now, let’s practice creating a Multi-sections Solid and adjusting its Couplings…
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Part Design
Sketch-Based Features Recommendations
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You will see some hints, tips and advices about tools seen in the lesson
Instructor Notes:
This final section will give students some hints, tips, short-cuts and tricks to make creation of the Sketch-Based Features more efficient…
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Part Design
Editing sketch during Rib or Slot Creation or Edition You can edit the sketches of the profile and the center curve during the rib or slot creation or edition Access to the profile’s sketch
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Access to the center curve’s sketch
Instructor Notes:
Profiles can be created or modifed by clicking the Sketcher icon within the feature’s dialogue box. This is more efficient than exiting the dialogue box and accessing the Sketcher tool from the workbench. After exiting Sketcher, you are returned to the original dialogue box…
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Part Design
Creating Sketch During Rib or Slot Creation
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If no sketch has been created when activating the Rib or Slot icon, you can access the Sketcher by selecting the Sketcher icon. When you have completed the sketch, you can exit the Sketcher and return to the Rib or Slot creation
Select the Sketcher icon in the dialog box
You could have used the same method to define the Center curve
Instructor Notes:
New Sketches can also be created after clicking the Sketcher icon in the dialogue box…
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Part Design
Using Sketch Sub-Elements to Create Ribs
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You can use sub-elements of a sketch to create ribs, like for pads or pockets
Instructor Notes:
Right-clicking in the Profile definition field will allow you access to the Profile Definition where you may select sub-elements of a Sketch rather than use the entire Sketch…
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Part Design
Using Sketch Sub-Elements to Create Slots
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You can use sub-elements of a sketch to create slots, like for pads or pockets
Instructor Notes:
The Sub-Elements Dialogue under Profile Definition…
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Part Design
Using Sketch Sub-Elements to Create Stiffeners
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You can use sub-elements of a sketch to create stiffeners, like for pads or pockets
Instructor Notes:
Sub-Elements in a Complex Profile Definition can be used in a wide variety of Part Design solid features. Let’s now summarize what we have learned about Sketch-Based features…
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Part Design
Using Several Closed Profiles to Create Ribs and Slots You can create Ribs and Slots from sketches including several closed profiles. These profiles must not intersect Slot
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Rib
Instructor Notes:
Non-Intersecting multiple Profiles can also be used under the Complex definition…
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Part Design
Sketch Based Features: Recap Exercises You will Practice the concepts learnt in this lesson to build a exercise following a recommended process.
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Jewel Case Core
Instructor Notes:
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Part Design
Jewel Case Core Sketch Based Features: Recap Exercise 20 min
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In this exercise you will : Design the part to create the core geometry for the Jewel Case. Create combine from two profiles perpendicular to each other Design the strengthening and mating part rib on the back perimeter of the core geometry Design the relief Rib
Instructor Notes:
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Part Design
To Sum Up This concludes the lesson on the Sketch based features You have learnt to create advanced sketch based features like Rib,Slot,Stiffener,Multi-Section solids Rib :Rib is feature that is created by sweeping a profile along a given part. Slot:Slot is a feature that removes material and is used in a similar way as Rib. Stiffener:A stiffener is a brace that is added to a wall to strengthen it and prevent breakage. it is mostly used in casting components. Multi-Sections solid: Multi-Sections solid is used to sweep several sections along a guided path. Removed Multi-sections solid is a feature similar to loft but the difference is that it removes material Multi-section solid can be created using guides,spines,couplings
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Multi-section solids can be relimited using Relimitation.
Instructor Notes:
Summarize what has been covered in the Sketch-Based Features section of the training.
Solicit questions from the students.
Next Section: Using Wireframe and Surface elements to create Solid Features…
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Part Design
Part Manipulations You will learn how to manipulate part elements
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Introduction to Part Manipulations Scanning a Part Design Using Boolean Operations Cut, Paste, Isolate, Break Sharing Geometries Sketch Selection with Multi-Document Links Part Manipulations Recommendations Part Manipulations: Recap Exercises Sum Up
Instructor Notes:
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Part Design
Introduction
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You will see in this lesson different tools used to manage features (cut, paste…), bodies (inserting, boolean operations), and how to create multi-model links
Instructor Notes:
Now you will learn different methods of Manipulating Part Features and Bodies and how to Create and Manage Multi-Model Links…
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Part Design
Scanning the Part
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You will see how to replay the construction history of a part.
Instructor Notes:
You will now see how to Replay the Construction History of a part in order to Visualize Dependencies…
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Part Design
What is Scanning a Part ?
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Scanning a part means to replay the construction history of a part and isolate temporarily any feature to work locally. By scanning a Part we can understand the complete steps that were followed to complete the design.
Instructor Notes:
Explain the purpose of Scanning a Part. Point out that while Replaying the History, you are actually Defining in Work Object each feature in the Current Part Body. Note that Using the Scan toolbar allows you to move Forward, Backward, to the Beginning, to the End or to Stop the Scanning. When you Stop the Scan, whichever feature was currently Defined in Work Object remains in that state.
Let’s see how to Scan a Part…
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Part Design
Scanning the Design Process
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Here is a powerful tool to show the Part History step by step in order to visualize how the model is designed. Scanning the design is done through Edit > Scan or Define in work Object.
You can select ‘forward’ at each step to scan all steps
Instructor Notes:
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Part Design
Scanning a Part (1/2) 1
Select Edit > Scan ... Menu option
Initial part 2
Use the Scan tools to navigate through the part structure
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Structure: all feature are scan in the order of the specification tree Update: all features are scan in the order of the update
Starting feature: feature active when starting scanning Backward: goes to the previous feature in the tree First to Update: goes to the first element to update and update it Forward: goes to the next feature in the tree Exit: when you exit the active feature becomes in work (it is underlined in the tree)
Display Graph: Make a dialog box appear displaying all the features belonging to the part
Last feature: last feature in the tree Play Update: replay the update of the geometry
Instructor Notes:
Explain how to access the Scan or Define in Work Object toolbar via the Edit menu. Note that selecting a feature in the tree references it as the starting point for the Scan. Explain the various functions available on the toolbar (Forward, Backward, etc.) Point out the purpose of Stopping the Scan in order to keep the current feature Defined in Work Object.
Solicit questions from the students about using the Scan or Define in Work Object tools.
When questions have been answered, continue on to Part Analysis Summary…
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Part Design
Scanning a Part (2/2)
3
4 To work again on the whole part, click the last feature in the tree and select the Define in work option in the contextual menu (MB3)
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The Mirror.1 feature is in work: you can make local changes
Instructor Notes:
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Part Design
What is Define in work Object ? Define in Work Object :To create a intermediate feature especially during design modification stage, define in work object is used.This is done through contextual menu. Define in work objects is useful when working with several bodies (in Boolean operations) By using Define in work object you can create features in a body by working in that body.
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Here the entire part is created in the same part body
Instructor Notes:
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But after creation of Pad.1 Body.2 is defined in work object then top part will be created in the second Body.
Part Design
Defining in Work Objects (1/2)
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1
Select a feature in the Tree with MB1
2
Select the Define in Work Object option in the contextual menu
Note that in the same Body, CATIA no longer displays features coming after the ‘active’ feature defined as in Work Object
Instructor Notes:
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Part Design
Defining in Work Object (2/2)
3
If you insert a new Sketch, it is positioned after the active feature(Feature that is underlined) defined as in Work.
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Here Pad.1 is Defined in work Object.
Instructor Notes:
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Here Shell.1 is Defined in work Object.
Part Design
Design Using Boolean Operations You will learn to design parts using Boolean Operations and by managing bodies.
ADD
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REMOVE
INTERSECT
Instructor Notes:
Now you will learn how to Insert Bodies into a Part and to Manage them using Boolean Operations…
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Part Design
What are Boolean Operations? The Three Basic types of Boolean operations are: 1.Add (Union):Adding two solids, combines the two solids such that they become one solid. The exterior surface looks the same, however the two objects now act as one unit and can moved, copied and manipulated as a single entity. 2.Remove (Subtraction): Using Boolean remove on two objects, the second objects is removed from the first object. The first object remains as it is, except the “volume” where the second object intersects the first object gets removed. 3.Intersect: Using Boolean intersection, the common volume or material to the two objects is kept. Object 2 in brown Object 1 in Green
REMOVE
INTERSECT
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ADD
Instructor Notes:
Explain that Add, remove and intersect are basics of boolean operation and catia provides with more advenced boolean operations such as union trim, assemble, remove lumps.
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Part Design
Why do we need Boolean Operations ?(1/3) We need Boolean operations for following Reasons: 1.Boolean approach facilitates design of complex parts. 2.To Optimize the design and Update of the part. 1. Design of Complex Parts Boolean ADD: For example, you want to create the following complex part.
It can be designed easily by using Boolean operations Then, create Material 2
Add them together so that a single object is formed.
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Create Material 1 first
Instructor Notes:
Boolean operations are used o design complex parts which are not easy to design by conventional parts as it would increase the design time.Explain using the illustration above.
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Part Design
Why do we need Boolean Operations ?(2/3) Boolean operations are used to design the complex Parts Boolean REMOVE: For example, you want to create the following complex part.
It is required to get the precise fillet value here.
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It can be designed easily by using Boolean operations
Create Part 1 first
Then, create Part 2
Remove Part 2 from Part 1 to get the final single part.
Instructor Notes:
Boolean operations are used o design complex parts which are not easy to design by conventional parts as it would increase the design time.Explain using the illustration above.
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Part Design
Why do we need Boolean Operations ?(3/3) Boolean operations are used to design the complex Parts Boolean INTERSECT: For example, you want to create the following complex part.
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It can be designed easily by using Boolean operations
Create Part 1 first
Then, create Part 2
Intersect part 1 and part 2 . Here Common part is kept
Instructor Notes:
Boolean operations are used o design complex parts which are not easy to design by conventional parts as it would increase the design time.Explain using the illustration above.
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Part Design
How to Create Boolean Operations ? (1/2) To create Boolean operations we need parts designed in different bodies and not in in a single Part Body. At a given time Boolean Operations can be performed on two different bodies only. To perform Boolean operations between the bodies ,you need to insert bodies through Insert > Body.
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You can create different Design steps in these bodies separately. Now You will be able to perform operations (add, assemble,remove,intersect,union trim) to define relation between these bodies. For example, to create a molded part. You can create Main part of the Mold in one body and the core in another body, then you can remove the core from the main part. Later it will be easy for you to separate the part and its core.
Instructor Notes:
Reinforce Boolean opertation can be created between two different bodies at a given time.Reinforce the use of define in work object.
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Part Design
How to create Boolean Operations? (2/2) Assembling/Adding :When Body2 is Assembled or Added with Body1, the operation between the bodies is a Union.The only difference between them is that Assemble will respect the “nature” of features. If Body2 contains Pocket feature (permissible) as its first node , Assemble will remove material from Body1. If Add is used, the Pocket will be seen by Body1 as a Pad. Intersecting : The resulting solid is the material common the two bodies. Removing : If Body2 is Removed from Body1, the operation is Body1 minus Body2
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Union Trim : The Union Trim is basically a Union with an option to remove or keep one side or the other. In the picture, the purple face is selected to be removed. For the Union Trim to work, the geometry must have sides that are clearly defined Remove Lump : All the above options work between two bodies. The Remove Lump works on geometry within a specific Body. “Lump” is the material that is completely disconnected from other parts in a single Body . The user can delete any Lump as a single entity even if the Lump is a combination of numerous features
Instructor Notes:
Explain the different Boolean Operations that can be performed on Bodies. Pay special note to the difference between Assemble and Add in a Boolean Operation. Also note how a Lump might be formed in a Body and how to Remove it.
Let’s look at some examples of these Boolean Operations…
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Part Design
Assemble 1
2
With the cursor on Body.2, select Assemble from the contextual menu (MB3)
We want to assemble Body.2 with PartBody
3
Select OK in the Dialog box
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Body.2 contains a groove In a complex part, when features are numerous it is useful to group together some of them in a body which becomes a subassembly of the first body using Insert in new body tool.
You get:
Because Body.2 contains a groove which is a feature that removes material, the result of the assemble operation is also removing material
Instructor Notes:
Explain the steps of creating an Assemble. Point out that Body.2 contains a single Solid Feature which removes material. Since there are no other Solid Features in Body.2 in which the Groove can operate, it is represented as a Positive Solid Volume. Note how it reverts to a Negative Solid Volume after the Assemble is created.
Let’s see what happens when we use these same two Bodies in an Add Operation…
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Part Design
Add 1
2
With the cursor on Body.2, select Add from the contextual menu (MB3)
We want to add Body.2 in PartBody
3
Select OK in the Dialog box
You get: Body.2 contains a groove
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Body.2 contains a single groove, so it appears as a solid (even if it normally removes material). When you Add a Body, CATIA keeps the feature like it appears before the addition.
Instructor Notes:
Explain how to create an Add from the two Bodies previously shown. Point out how this Boolean Operator does not respect the Negative Solid Volume represented by the Groove.
Let’s now look at the Remove operation…
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Part Design
Remove 1
2
With the cursor on Body.2, select Remove from the contextual menu (MB3)
3
Select OK in the Dialog box
We want to remove Body.2 from PartBody
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You get:
Instructor Notes:
Explain the process of performing a Remove Operation between two Bodies. Review the structure of the Specification Tree before and after the Boolean Operation is performed. Note that the Operation is simply another Feature in the Tree. If you delete this Feature, it will not delete the Bodies but only delete the Operation between them.
Let’s see how the Intersect Operation works…
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Part Design
Intersect 1
2
With the pointer on Body.2, select Intersect from the contextual menu (MB3)
3
Click OK in the Dialog box
We want to intersect Body.2 with PartBody
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You get:
Instructor Notes:
Explain the process of creating an Intersect between two Bodies. Note the results in Geometry View and in the Specification Tree.
Let’s look at creating a Union Trim between two Bodies…
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Part Design
Union Trimming Bodies 1
2
We want to do a Union Trim of Body.2 with PartBody
3
With the pointer on Body.2, select Union Trim in the contextual menu (MB3)
Select the Face to remove then the face to keep
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You get:
4
Click OK
Instructor Notes:
Explain the process of creating a Union Trim between Bodies. Note that this will have no effect on the geometry unless Faces to Remove or Keep are selected. Several different results can be derived from the two Bodies shown here.
Let’s now see what Lumps are and how to Remove them…
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Part Design
Removing Lumps (1/3) After certain operations, it may happen that some Lumps or Cavities appear in the part. We need to remove them. The Remove Lump capability allows you to remove Lumps and Cavities Cavity
Pockets
Shell
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Lumps
Instructor Notes:
Explain that there are times when unwanted artifacts are created in the Solid Body as a result of Boolean Operations or a Shell creation. These artifacts may manifest themselves as Lumps, Cavities or both. It is desirable to remove these artifacts to complete the Part Design…
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Part Design
Removing Lumps (2/3) 1
With the pointer on PartBody, select Remove Lump in the contextual menu (MB3) 2
Select the ‘Faces to remove’ field in the dialog box
Select the two following faces belonging to the lumps to be removed
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3
Instructor Notes:
Explain how to perform a Remove Lump Operation. Note that Face Selection identifies the Lumps being Removed…
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Part Design
Removing Lumps (3/3) 4
In order to select a face of the cavity, place the pointer on the cavity to be removed then press the Up arrow key of the keyboard
6
7
5
Using the small arrows, highlight one of the cavity face
To confirm the face selection click inside the circle
Click OK
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You get:
Instructor Notes:
Explain how to use the Preselection Navigator to select hidden Faces such as found with Cavities. Point out the differences between the final Part and the original Part.
Solicit questions from the students about any of the Boolean Operators covered thus far.
When questions have been answered, continue on to Assembling a Set of Bodies…
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Part Design
Assembling a Set of Bodies (1/3) Assembling a set of bodies (Multi selected using the Ctrl key) is possible
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1
Using the Ctrl key, select the three following bodies to be assembled
Instructor Notes:
You will now see how to Assemble a Set of Bodies. Note that you can Multi-Select two or more Bodies with the Ctrl Key in order to Assemble them in one Operation…
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Part Design
Assembling a Set of Bodies (2/3) With the cursor placed on the last body, select the Assemble option in the contextual menu
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Instructor Notes:
Right-Clicking on any one of the Selected Bodies will provide you with the Selected Objects Contextual Menu where you can click the Assemble menu…
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Part Design
Assembling a Set of Bodies (3/3)
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Select OK in the dialog box
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You get:
Instructor Notes:
Explain that this procedure will result in a single Assemble feature for each Body that was in the Selection. Each Body is assembled to the same Body selected in the Dialogue Box.
Let’s see how we can use Replacing Bodies to modify an existing Boolean Operation…
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Part Design
What is Replacing a Body?
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You can replace a body used in an operation by another one
Instructor Notes:
Explain that when you need to change one of the Bodies involved in a Boolean Operation and use another Body in its place, it is not necessary to delete the Boolean feature and recreate it. You can use Replacing a Body to do this.
Let’s see how this is done...
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Part Design
Replacing a Body (1/3) Body to be replaced
1
Select the Replace command from Body.3 contextual menu
2
Select Body.4
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Replacing body
Instructor Notes:
Explain the process of accessing the Contextual Menu on a selected Body in order to perform a Replace. Note that this is performed on the Body being Replaced…
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Part Design
Replacing a Body (2/3) 3
4
Select the following line in the dialog box
Select the following face in the Replace Viewer. This face is the face that will be removed during the Union Trim operation
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Select OK
Select OK
Instructor Notes:
Explain the use of the Replace Command Dialogue box. Note that the Body being Replaced requires input of the Replacing Body and any Faces involved in the Boolean Operation. Clicking OK will launch a Replace Viewer that provides an easy means of redirecting Faces between the Bodies involved in the Replace Operation. Point out the option to Delete Replaced Elements and Exclusive Parents, if this is desired.
Let’s see the final result of this Operation…
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Part Design
Replacing a Body (3/3)
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If necessary, update the part by selecting the Update All icon
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You get:
Instructor Notes:
Note the differences in the Geometry View and in the Specification Tree.
Now let’s look at how to change the Boolean Operation Type once it has been created…
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Part Design
Changing the Boolean Operation Type (1/4) The initial part is composed of three bodies. Assemble Body.1 to Part Body.
2
Remove Body.2 from Assemble.1.You obtain Remove.1.
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Instructor Notes:
Explain the structure of this example. Note the Assemble Operation performed on the first two Bodies (rectangular Pads). Point out the Remove Operation performed with the third Body (cylindrical Pad) and the final result in the left-side illustration…
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Part Design
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Changing the Boolean Operation Type (2/4)
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Click with the right button mouse on Remove.1. In the contextual menu, select Remove.1 object
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Choose now the new operation. For example, click on Change To Assemble.
Instructor Notes:
In this example, point out that you are going to change the Remove Operation to an Assemble Operation. Explain that this is done by accessing the Contextual Menu from the Operation being changed. Note that the Remove could also be changed to an Add Operation through this menu…
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Part Design
Changing the Boolean Operation Type (3/4) 5
You obtain :
Change now Assemble.2 to Union Trim. You obtain :
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Instructor Notes:
Point out the changes in the Geometry View and in the Specification Tree. Note that you can change the Boolean Operation Type yet again and experiment with different results. In this example, you can change the Assemble to a Union Trim…
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Part Design
Changing the Boolean Operation Type (4/4) You can edit Trim.1. For instance, select the cylinder's top face as the face to keep. You obtain :
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Instructor Notes:
Here is the final result of these Operation Type changes.
Solicit questions from the students about Inserting and Managing Bodies.
When questions have been answered, continue on to Multi-Model Links…
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Part Design
Cut, Paste, Isolate, Break
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You will see how to cut or copy a feature and paste it into a body and you will also see how to isolate or break 3D geometry from its parents
Instructor Notes:
You will now learn how to Cut, Paste, Isolate and Break Part Features…
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Part Design
What is Cut/Copy and Paste (Drag and Drop)?
The operation Cut/Copy and then Paste captures the node specified into the clipboard and either replaces (Cut) or copies (Copy) the content into a different selected point in the part structure. The action is interpreted by the system in a context-sensitive manner. For example, if a pad is copied onto a different sketch, the new sketch is used for the profile and information on extrusion limits will be those of the pad. However, if pad1 is copied onto pad2, since this action has no real meaning, it is interpreted as generically copying the clipboard’s content into the part. The effect is to create another copy of pad1 (with its original sketch) in the part structure. This copy will be placed after whatever node is currently the “In Work” node.
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Cut/Copy then Paste can be achieved by using the drag and drop capability. If the CTRL key is pressed during the drag and drop, the action is interpreted as a copy otherwise as cut.
Instructor Notes:
Explain how CATIA handles Cut/Copy/Paste (CCP) in Part Design. Point out some of the uses for this capability and note that this process works in a single Part Document or between two different Part Documents (Multi-Model, discussed later). Note the use of the CTRL + Drag and Drop to produce a Copy and Paste operation. Point out that the Paste of the features being Copied or Cut will appear in the Specification Tree after whichever feature is currently Defined in Work Object.
Let’s see how to use CCP…
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Part Design
Cut/Copy and Paste (Drag and Drop) (1/3) 1
2
paste the Pad feature on sketch.3.Select Sketch.3,click MB3,and select paste.
Pad.3 is created on sketch.3 with the same limits as those in Pad.2
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Select the feature that you want to copy on another feature from the tree.Copy Pad.2
Instructor Notes:
Explain the process of Copying one Sketch-Based Feature onto another Sketch Profile to save time and when you want the definition of the new feature to match the prior feature. Point out that this process does not create a Link and each feature can be modified independently (note the new features in the Specification Tree).
Solicit questions from the students about the use of CCP.
When questions have been answered, continue on to Isolate and Break…
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Part Design
Cut/Copy and Paste (Drag and Drop) (2/3) 4
Copy Draft.1 from the tree.Select the vertical face of the Pad.3 and Paste it using MB3.
Draft.2 is applied to Pad.3.
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Instructor Notes:
Explain the process of Copying one Sketch-Based Feature onto another Sketch Profile to save time and when you want the definition of the new feature to match the prior feature. Point out that this process does not create a Link and each feature can be modified independently (note the new features in the Specification Tree).
Solicit questions from the students about the use of CCP.
When questions have been answered, continue on to Isolate and Break…
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Part Design
Cut/Copy and Paste (Drag and Drop) (3/3) 6
Keeping the Ctrl Key pressed, select Edgefillet.1.
Drag the selection and drop it on one of the edges of Draft.2.
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Instructor Notes:
Explain the process of Copying one Sketch-Based Feature onto another Sketch Profile to save time and when you want the definition of the new feature to match the prior feature. Point out that this process does not create a Link and each feature can be modified independently (note the new features in the Specification Tree).
Solicit questions from the students about the use of CCP.
When questions have been answered, continue on to Isolate and Break…
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Part Design
When to Use Isolate and Break?
• Isolate is used when 3D geometry is projected into a sketch in order to be modified and used as part of the sketch’s profile. Isolate duplicates the element since the original element cannot be changed because other geometry depends on it.
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• Break is used to divide an isolated element into two parts at a specified point (usually to use one side of this element in the sketch).
Instructor Notes:
Explain the use of Isolate 3D Geometry when it has been projected into a Sketch for use in developing another Profile. In Sketcher, Projected Elements result as Marks. Isolate converts the Mark to normal Sketcher geometry with no link to the original 3D Geometry it was projected from. Point out that Break can be used to divide a Mark into multiple segments without affecting its associativity to the 3D Geometry it is projected from.
Let’s see some examples of this…
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Part Design
Isolate, Break (1/3) Starting with the geometry as shown below, we want to add a pad.
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2
Pad
Using the Trim and Break icon in the sketcher, modify the sketch as follows, then exit the sketcher.
Lines
Diameter 100
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Intersection between the pad and the sketch plane
Create a pad with an length of 20.
Added pad
Diameter 50
Instructor Notes:
Explain the process of creating a Break in the Mark (projected element in Yellow color) and then Trimming it the normal 2D Lines drawn in Sketcher. Discuss the Associativity now established between these two Pads as a result of using this methodology.
Now let’s see how we can affect this with the Isolate command…
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Part Design
Isolate, Break (2/3) Edit the Sketch of the first pad and change the circle diameter to 50.
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6
5
Exit the sketcher (Sketch.1), if necessary, Update the part. You will get:
Select the Undo icon (may be several times) in order to come back to diameter 100 Edit Sketch.2, place the cursor on the yellow line. Select Isolate from the contextual menu.
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Instructor Notes:
Explain that sometimes you will get Update Diagnosis errors if you change the feature you have linked to via the Mark. When this happens, you can Isolate the Mark from its Parent 3D Feature and prevent the error.
Even if you don’t use a Projection or Intersection in the Sketch to produce the Mark, you can create the same type of associativity with Constraints…
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Part Design
Isolate, Break (3/3) 8
Create two Coincidence between the isolated arcs and the cylinder and exit the sketcher
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Edit the Sketch (Sketch.1) of the first pad and change the circle diameter to 50
Exit the sketcher, if necessary, Update the part. You will get:
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Instructor Notes:
Explain the use of the Coincidence Constraints used here to tie Sketcher geometry to outside 3D Geometry.
Solicit questions from the students on the use of Isolate and Break.
When questions have been answered, continue on to Inserting and Managing Bodies…
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Part Design
Sharing Geometries
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You will learn ways to Share Geometries using Multi-model links to help propagate design changes.
Instructor Notes:
Now you will learn how link design information from one Part Document into another Part Document in order to establish Links between the Models. In the example shown, a Part Body from another Document has been copied into the current Document using the Paste Special -> As Result With Link. Point out the representation of the Resultant Solid, including the “Green Dot” within the Solid’s icon. This means that the Solid is Linked and Synchronized with its Link…
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Part Design
Introduction Here you will learn to Share geometries between several parts by keeping the link. The link will be maintained between the Source part and the part in which copy is done.
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To do so, you will learn what are Multi Model Links
Instructor Notes:
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Part Design
What are Multi-Model Links ? The concept of working within an independent “Body” and then having the ability to Add, Remove, or Intersect this Body with your “Master” PartBody gives you added modeling flexibility
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There are different ways that an independently modeled Body can be assimilated into a PartBody
Instructor Notes:
If changes are made to the source Document, the icon for the Linked Solid changes so that a “Red X” appears on it. This means that the Solid is Linked, but not Synchronized. Also note that the Part is waiting for an Update to be performed. If the option to Synchronize External Links is activated, then the Part Update will also Synchronize the Linked Body.
Let’s look at these Links in more detail…
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Part Design
Why do we need Multi-Model Links ?(1/2) In the context of the concurrent engineering, Multi-Model Links enable to keep the link between a copied element and its master. This allows to share geometries coming from different designers into your own part and it enables to update your part whenever different designers modify their design. Part Created By Designer A.
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By using MML Part B is Imported in Part A
Instructor Notes:
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Part Created By Designer B.
Part Design
Why do we need Multi-Model Links ?(2/2) Part B is Removed from Part Using Boolean Operations
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Part B is modified by Designer B
Instructor Notes:
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The changes are reflected in the Master design A on update.
Part Design
Establishing Multi-Model Links (1/3) 1
In a CATIA session you have two separate parts 2
Using the Contextual Menu, copy the PartBody of Part2
Place the cursor on the PartBody of Part1 then Select Paste Special from the contextual menu
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Instructor Notes:
Explain that Establishing a Multi-Model Link begins with a Copy operation performed on a Feature or Body in a Part Document. Point out that the Link is established when you perform the Paste Special operation into a second Part Document.
Let’s see which option provides the Link…
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Part Design
Establishing Multi-Model Links (2/3) 3
In the dialog box, select As Result With Link and the Paste button, then select OK
4
Part1 becomes:
In Sketch.1 of part1, create a distance (10mm) between the circle and the copied cylinder then exit the sketcher
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Instructor Notes:
Explain that the Paste -> Result With Link option will Paste the object into the Part Document as a Resultant Solid and Link it Back to the Source Feature. Point out that other options under Paste Special are also available, but do not establish Multi-Model Links. Paste -> As Specified In Part Document will Paste the object into the Part Document with no Link and all original features available for editing. Paste -> As Result will Paste the object into the Part Document as a Resultant Solid but with no Link back to the Source Feature. In this case the Solid cannot be modified, but additional features can be added to it.
Let’s see the behavior of using the Result With Link option…
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Part Design
Establishing Multi-Model Links (3/3) 6
8
Now, in Sketch.1 of part2, create a diameter constraint of 50 then exit the sketcher
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Part1 becomes:
With Part1 active, select the Update All icon
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You get:
Instructor Notes:
Point out how changes to the Source Feauture are passed on to the Linked Feature via Synchronization.
Solicit questions from the students about building Multi-Model Links with Paste Special.
When questions are answered, continue on to learn how to work with Sketches in a Linked Multi-Document environment…
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Part Design
Sketch Selection with Multi-Document Links
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It is possible to copy and paste with link a sketch from a document to another one
Instructor Notes:
You will now see what is possible when Copy and Pasting With Link a Sketch from one Document to another…
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Part Design
Sketch Selection with Multi-Document Links (1/5) You can copy a sketch in a document then paste it into another document keeping the link with the first one. You can use this copied sketch and in case the original sketch is modified, the document in which the copy is used will be also be modified
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2
After loading a part containing a sketch, start a new part using the File + New command
You get:
Display the two parts using the Window + Tile Horizontally command
Instructor Notes:
Explain that a Sketch feature (just like any other feature) is available for use in Copy and Paste operations.
In this example, you see two Documents being displayed through Tiled Windows in preparation for Editing Operations in a Multi-Document environment…
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Part Design
Sketch Selection with Multi-Document Links (2/5) You can copy a sketch in a document then paste it into another document keeping the link with the first one. You can use this copied sketch and in case the original sketch is modified, the document in which the copy is used will be also be modified With the cursor on Sketch.1 in the tree, select the Copy command from the contextual menu (MB3)
4
In the second part, place the cursor on PartBody, then select Paste Special from the contextual menu (MB3)
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Instructor Notes:
As with any feature, you can right-click for the Contextual Menu and Copy / Paste Special from one Document into the other…
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Part Design
Sketch Selection with Multi-Document Links (3/5) You can copy a sketch in a document then paste it into another document keeping the link with the first one. You can use this copied sketch and in case the original sketch is modified, the document in which the copy is used will be also be modified Select AsResultWithLink in the dialog box
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Expand Sketch.1 in order to see what has been copied (by selecting +)
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Instructor Notes:
Using the As Result With Link option establishes the Link with the Resultant Sketch in the destination Document. Note that the Geometry is not accessbile in this Result– it is treated as a Datum. Any changes to Sketch Geometry can only be done in the source Document…
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Part Design
Sketch Selection with Multi-Document Links (4/5) You can copy a sketch in a document then paste it into another document keeping the link with the first one. You can use this copied sketch and in case the original sketch is modified, the document in which the copy is used will be also be modified
7
Create a 20mm-high pad using the copied sketch
In the first part, modify the sketch as shown below
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Instructor Notes:
Explain the process of rolling changes from the Source Document Sketch into the Destination Document Sketch via the Link. Note that the Sketch in the Source Document could be used to generate a Pad while the Sketch in the Destination Document could be used to generate a Pocket. There is no restriction in how the Linked Sketches are used.
Let’s see the final result of this example…
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Part Design
Sketch Selection with Multi-Document Links (5/5) You can copy a sketch in a document then paste it into another document keeping the link with the first one. You can use this copied sketch and in case the original sketch is modified, the document in which the copy is used will be also be modified 9
To take the modification into account in the second part (the one which contains the copied sketch), place the cursor on Part2 then select the Part2object + Update All Links command
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You get:
Instructor Notes:
Explain the example shown here of using Synchronize All from the Part Contextual Menu to synchronize all External Links in the Part. Point out that you can also Synchronize each feature selectively via their respective Contextual Menus. Note that Synchronization can be forced each time a Part Update is performed if that option is set in Tools -> Options.
Solicit questions from the students about using Sketches with Links in a Multi-Document Environment.
When questions are answered, continue to Part Manipulation Recommendations…
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Part Design
Part Manipulations Recommendations
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You will see some hints, tips and advices about tools seen in the lesson
Instructor Notes:
You will now see some Recommendations for Advanced Part Manipulations…
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Part Design
The Different Paste Special Options (1/3)
As specified in Part document: The copied element can be modified and has no link with the original one. The original element is duplicated As Result With Link: The copied element cannot be modified, but in case of modification of the original element, the copied one is updated
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As Result: The copied element cannot be modified (it is a datum) and in case of modification of the original element, the copied one is not updated
Instructor Notes:
Explain the different options for Paste that are shown here.
Let’s see some tips related to copying and pasting sketches…
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Part Design
The Different Paste Special Options (2/3) As Result With Link You can edit the link of the solid which has been pasted in the same part using the option ‘As Result With Link’.
Consider the following scenario: Two different configurations of Cavity Pockets are stored in the two bodies namely: Cavity Pockets V1 and Cavity Pockets V2 Solid.9 is linked to one of the Cavity Pockets bodies and is used in Boolean operation with the part body. By changing the parent link of Solid.9 you can obtain the required design configuration.
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Cavity Pockets
User can only select Bodies within the Part in which the Solid is defined.
Instructor Notes:
Explain the different options for Paste that are shown here.
Let’s see some tips related to copying and pasting sketches…
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Part Design
The Different Paste Special Options (3/3) To change the parent of the pasted solid double-click its representation in the specification tree.
2
Select the another input for the solid as ‘Cavity Pocket V2’.
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Solid.9 has been created by copying the ‘Cavity Pockets V1’ body and pasting it in the same part using the paste special option ‘As Result With Link’.
The design has been changed to accommodate new Cavity Pockets
Instructor Notes:
Explain the different options for Paste that are shown here.
Let’s see some tips related to copying and pasting sketches…
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Part Design
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Copying and Pasting Sketches
To paste a sketch from one document to another, right click the destination plane / face and select paste from the contextual menu. This method can avoid task of changing the sketch support which may be required later.
Instructor Notes:
Explain how you can right-click a plane or planar face and use the contextual menu to paste a sketch directly to the clicked support. This saves time by not requiring you to Change Sketch Support after pasting a sketch.
Let’s see a tip on creating Isolate geometry in a sketch…
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Part Design
Isolating Sketch Links
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You can create an Implicit Projection by making dimensional or geometrical constraints between your sketch geometry and 3D elements outside the sketch.
If you display the Implicit Projection in Sketch Analysis, you can Isolate the projection even though no explicit geometry exists. This process creates the appropriate construction geometry in the sketch which is isolated from the original 3D elements.
Instructor Notes:
Explain how it is not necessary for you to create an Explicit Geometry Projection on to a sketch when you can also create an Implicit Projection. Point out that an Implicit Projection does not create geometry in the sketch. Note that you can use Sketch Analysis to Isolate an Implicit Projection and that the result will be the creation of Isolated construction geometry in the sketch.
Continue on to the Summary for Part Manipulations…
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Part Design
Part Manipulations Recap Exercises 35 min
In this step you will create:
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Adding and Assembling Bodies Creating Union/Trim bodies Copy/Paste Special bodies Modifying Linked Geometry Copying and Pasting Geometry within a Part Copying and Pasting Geometry from one Part to Another Part Creating 3D Constraints between Bodies Connect Curves
Instructor Notes:
45 Min
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Part Design
To Sum Up This concludes the lesson on the Part Manipulation tools. Boolean operations are used to design complex parts. Boolean operations are performed between two bodies at a time. Body is inserted through Insert > Body. Different Boolean operations are Add Remove Intersect Assemble Union Trim
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Remove Lump:Used on the body on which Boolean operations are already performed. Multi-Model links are used to propagate the design changes for one part to another. Features can be dragged from one location to another ,also they can be copied. This is covered under Cut,Copy,Isolate, Break.
Instructor Notes:
Summarize the topics covered in this section.
Solicit questions from the students about these topics.
When questions have been answered, continue on to Annotations…
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Part Design
Dress-Up Features You will learn how to create advanced dress-up features
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Introduction to Dress-Up Features Advanced Drafts Thickness Removing Faces Replacing a Face with a Surface Dress Up Features Recommendations Dress-Up Features: Recap Exercises Sum Up
Instructor Notes:
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Part Design
Introduction The following advanced tools allow you to dress-up existing solids Advanced Drafts: This tool allows you to create complex drafts with a parting element or a reflect line:
Thickness: This tool is useful when you want to add a thickness to a face:
Remove Faces:
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This tool is useful when you want to simplify the geometry of a part for down stream processes:
Replace a Face with a Surface: This tool is useful when you want to have a portion of the solid be extruded to a surface:
Instructor Notes:
In this section, you will learn about a number of tools used to Dress-Up existing Solid geometry…
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Part Design
Advanced Drafts
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In this lesson you will see the Advanced Draft feature
Instructor Notes:
You will now learn how to create an Advanced Draft feature…
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Part Design
What is the Advanced Draft? (1/5) The Advanced Draft tool lets you draft basic parts or parts with reflect lines. It also lets you specify two different angle values for drafting complex parts. This task shows you how to draft two faces with reflect lines by specifying two different angle values and using the two available modes.
By default, the Advanced Draft toolbar is not accessible from CATIA, so in order to get it, you will have to select
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Views -> Toolbars -> Advanced Dress-Up Features
You will see the following toolbar:
Instructor Notes:
Explain the purpose of the Advanced Draft Feature in providing capability to impose multiple Draft characteristics in a single Draft feature. This is especially useful in complex parts that cannot be easily set up for Mold or Tool and Die processes using standard Draft features. Show the students how to activate the Advanced Draft tool on the Part Design workbench.
Let’s see an example of where Advanced Draft is useful for complex Part Design…
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Part Design
What is the Advanced Draft? (2/5) The Advanced Draft tool gives you the option to define standard draft as well as draft with reflect line on one or two sides. To do so, you will have to activate one or two buttons as described hereafter.
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Standard Draft (1st side)
Standard Draft (1st and 2nd Side)
Draft reflect line (1st side)
Draft reflect line (1st and 2nd side)
Instructor Notes:
Point out the set of four buttons in the upper-left corner of the Dialogue Box. Explain how these buttons are used to specify the Draft Side or Reflect Line options for the Advanced Draft feature. For the left buttons, one or two can be activated to specify First Side and/or Second Side Drafts. For the right buttons, one or two can be activated to specify First Side and/or Second Side Reflect Lines. The illustrations give an example of possible results from these combinations. Note that depending on which buttons are selected, certain fields and tabs in the rest of the Dialogue Box will be active or inactive.
Let’s look at some of these fields and tabs to see what they provide in defining an Advanced Draft…
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Part Design
What is the Advanced Draft? (3/5) The 1st side tab is used to define the characteristics of the draft angle for the selected faces. If you decide to draft both sides, you have to define the draft angle characteristics for the second side using the 2nd side tab. When drafting both sides with reflect lines, you define whether the draft angles are independent or not.
To define if the angles are the same or not when using draft with reflect line. To define the draft angle value. To define the Faces to be drafted.
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To define the neutral element.
To define the pulling direction.
Instructor Notes:
Explain that in this example, only the 1st Side is being drafted, so the 2nd Side Tab is inactive. There are section to define Faces to Draft, define Neutral Element and Pulling Direction. In this example, you could define all of this using the regular Draft tool. Point out that if you were to select the 2nd Side option, then the 2nd Side Tab activates. You would also then be able to specify Independent Driving Angles for each Side or optionally specify one side or the other to be the Driving Side. Note that these options give you capability to define a complex Draft in a single resultant feature.
Let’s look at the Parting Element tab in this Dialogue Box…
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Part Design
What is the Advanced Draft? (4/5) To define the Parting Element, you have to use the parting tab. The parting element can be a plane, a surface or a face
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To define the parting element
Instructor Notes:
Explain the options available under the Parting Element tab. Note that the Neutral Elements for 1st Side or 2nd Side can also be defined as Parting Elements. On the tab shown here, Limiting Elements for the Draft can also be specified.
Let’s look at the options available on the 2nd Side tab when it is specified in the Advanced Draft…
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Part Design
What is the Advanced Draft? (5/5) When you decide to draft both sides with independent angles, you have to define the second side characteristics
To define the draft angle value
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Neutral element
To define the pulling direction
Instructor Notes:
Explain that on the 2nd Side tab you can define Draft Angle (unless it is Driven by 1st Side), Neutral Element for the 2nd Side and Pulling Direction.
Let’s explore Drafting Both Sides in a little more detail…
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Part Design
Advanced Draft Angle: Draft Both Sides (1/9) You are going to see how to draft both sides using the Advanced Draft icon
1
Select the Advanced Draft icon
Activate these two buttons
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2
Instructor Notes:
In this scenario you will show how to use the Draft Both Sides option of Advanced Draft. Note that the 1st Side and 2nd Side buttons must be clicked to perform this operation…
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Part Design
Advanced Draft Angle: Draft Both Sides (2/9) Select this face as the object to be drafted
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Instructor Notes:
In this example, you are applying an Advanced Draft to one face of the solid. Note the Faces to Draft selection and the default Pulling Direction in the Dialogue Box…
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Part Design
Advanced Draft Angle: Draft Both Sides (3/9) Select the indicated plane
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4
Instructor Notes:
In this case, the middle Plane of 3 planes is selected as the Neutral Element. The intersection of this Plane with the Solid Body will retain the original part dimensions and profile. Explain that the 1st Side Draft Angle will be calculated from this intersection. Note the option to set the Neutral Element = Parting Element, if desired. In this case, you will use a different Parting Element in a later step…
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Part Design
Advanced Draft Angle: Draft Both Sides (4/9) Enter 21 in the angle field
6
Select the Parting Element tab
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5
Instructor Notes:
In this example, a 21-degree Draft Angle is being applied to the 1st Side of the Neutral Element. Now you will see how the Parting Element is defined…
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Part Design
Advanced Draft Angle: Draft Both Sides (5/9) Select the Parting Element button
8
Select the Parting Element field
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7
Instructor Notes:
Activating the Use Parting Element check box allows you select a Parting Element. Note also that you can specify Limiting Elements from this tab in the Dialogue Box. Now you are ready to select the Parting Element…
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Part Design
Advanced Draft Angle: Draft Both Sides (6/9) 10 9
Select the 2nd Side tab
Select the indicated plane
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Select the required plane from tree or user can create plane by right clicking in selection menu as shown below
Instructor Notes:
In this case, the upper Plane is selected as the Parting Element. This means that the 1st Side Draft will propogate until it reaches the Parting Element. Now you are ready to specify the 2nd Side Draft…
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Part Design
Advanced Draft Angle: Draft Both Sides (7/9) Select the indicated plane
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Instructor Notes:
The lower Plane is selected as the Neutral Element for the 2nd Side. This means that the intersection of this plane with the Solid Body will retain its original design size and profile and that the 2nd Side Draft angle will be propogated from this intersection until it reaches the Parting Element…
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Part Design
Advanced Draft Angle: Draft Both Sides (8/9) Enter 45 in the angle field
13
Select Preview
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12
Instructor Notes:
In this case, a 45-degree Draft Angle is being applied on the 2nd Side. Clicking Preview will give you an indication of how the Advanced Draft is going to be created. If there are any errors in your definition, clicking Preview will present them to you…
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Part Design
Advanced Draft Angle: Draft Both Sides (9/9) You will see
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14
Select OK in the dialog box
You get:
Instructor Notes:
Clicking OK in the previous Dialogue Box will complete the generation of the Advanced Draft. Note the 21-degree Draft imposed on the 1st Side down to the Neutral Element. Also Note the 45-degree Draft imposed on the 2nd Side up to the Neutral Element.
Solicit questions from the students on the Draft Both Sides option in Advanced Draft.
When questions have been answered, continue on to practice creating an Advance Draft feature…
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Part Design
Thickness
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You will see how to add material on a face by defining a thickness
Instructor Notes:
Now you will learn how to add Thickness to any face in order to add more material…
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Part Design
Why Applying Thickness?(1/2)
Applying thickness is basically used to enhance the productivity during solid model creation. A standard use of thickness is to add or remove material before machining a part. Thickness enhances the design intent and allows rapid modifications. Thickness is useful when you need to add material to various faces on a Part to accommodate machining or other manufacturing operations. For instance, you might add Thickness to account for additional material necessary to cast the part.
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Thickness is also applied to select walls of a Part that has been Shelled.
Instructor Notes:
Now you will learn how to add Thickness to any face in order to add more material…
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Part Design
Why Applying Thickness?(2/2) Now suppose we want to add thickness to one of the faces of the following part.
One of the methods is to create a pad,by selecting the face and specifying the length value.
Here you can observe that the filleted portion cannot be thickened in the Pad.To Pad that portion the number of steps would increase.
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By using the thickness tool we can solve this problem quickly and efficiently.
Instructor Notes:
Now you will learn how to add Thickness to any face in order to add more material…
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Part Design
Creating a Thickness (1/2) Select Thickness icon from Dress-Up features toolbar.
2
Select the faces to thicken.
3
Insert 10 as the Default thickness value.
4
Thickness is applied to the selected faces.
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1
Instructor Notes:
Explain that Thickness is useful when you need to add material to various faces on a Part to accommodate machining or other manufacturing operations. For instance, you might add Thickness to account for additional material necessary to cast the part. Note that Thickness is also applied to select walls of a Part that has been Shelled. Review the various options in the dialogue box with the students.
Let’s now look at Removing Faces in order to simplify a Part design…
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Part Design
Creating a Thickness (2/2) 5
Now we want add different thickness value to other faces.To edit the feature,double click on the specification tree to open the thickness definition dialog box.
6
Select the indicated faces and enter the thickness value as 5mm.
Enter 5 mm.
The thickness applied to the other faces ,maintains the same relation with the other features.Here the thickness is created along the the two cylinders.
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7
Instructor Notes:
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Part Design
Removing Faces
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You will see how to simplify a part by removing some of its faces or features.
Instructor Notes:
Now you will learn how to Remove Faces from a solid Part in order to simplify it…
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Part Design
Why would you use this tool ? When a part is to complex for of a finite element analysis you can remove some of its faces or features to simplify the geometry. Remove Faces ICON
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The feature in the Specification Tree contains the part without the removed features
Instructor Notes:
Explain why you might want to use the Remove Faces feature instead of simply deleting the unwanted features. Point out that Remove Faces provides a rapid method of simplifying a part and changing that simplification later, instead of deleting and recreating the unecessary features.
Let’s see how Remove Faces works…
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Part Design
Removing Faces 2 Select internal faces
which have to be removed
3
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1
Select Remove Face tool
Contextual menu of Faces to remove field allows to select tangency propagation option which automatically removes all faces tangent to the selected ones. Faces are removed and a new feature is created in the specification tree
Instructor Notes:
Explain how the Removing Faces dialogue box options. Point out the Contextual Menu option for Tangency Propogation and Clear Selection. Note that Tangency Propogation may pick up faces that you do not want removed! Explain that the Faces to Keep field allows you to select faces that you do not want removed. Point out the Remove Faces feature in the Specification Tree. Note that the original design features remain intact.
Let’s practice using the Remove Faces tool…
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Part Design
Replacing a Solid Face with a Surface
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You will see how to replace a Face of a Solid by extruding it up to an external surface.
Instructor Notes:
Now you will learn how to create a Replacing Face on a Solid part…
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Part Design
Extruding a Solid Face Up To a Surface 2 Select the replacing surface and 1
Select the Replace Face tool
click the arrow to make it pointing in the kept material direction
3
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4
Select the face to extrude
You get the selected face extruded up to the replacing surface. Replace Face feature is added in the specification tree
Instructor Notes:
Explain the purpose of using the Replace Face tool. Note that rather than changing the specifications for the Pad and two Pockets on this part so that their Limits are Up to Surface, you can instead very quickly grab the desired Face on the part and extrude it to the External Surface. Point out that a Contextual Menu is available to create the Replacing Surface if it does not already exist. Note the Replace Face feature in the Specification Tree.
Let’s see how to create a Replacing Face…
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Part Design
Dress Up Features Recommendations
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You will see some hints, tips and advices about tools seen in the lesson
Instructor Notes:
Now we will review Recommendations for Dress-Up Features…
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Part Design
Ignoring Faces When Creating a Thickness In some cases, when you want to create an Offset, an error message appears informing you that the Body can’t built properly. After closing the window, another message appears proposing you to Ignore the Faces causing trouble. If you accept, the Thickness is created and the Face causing trouble is removed. For example, here we want to offset the selected Face but it is not possible. The Face causing trouble is the Radius Fillet.
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We accept to ignore the Fillet, thus the Thickened Body becomes :
Instructor Notes:
Explain how when Creating a Thickness, you may encounter errors with other features during the process. Point out in this example how applying Thickness to the two faces of this part cause an error with the inside corner Fillet. Note that the Fillet cannot accommodate the added thickness. In this case, you can ignore the Face that cannot be thickened…
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Part Design
Reset Ignored Faces Option for Thickness Tool If we edit the Thickness from the specification tree, the Ignored Faces are previewed :
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The option “Reset Ignored Faces” appears in the Thickness Definition Dialog box. After selecting this option, the Ignored Faces are reinitialized and the indication “Ignored Face” in the geometry is removed.
Instructor Notes:
Point out that later on you can Reset the Ignored Faces when you make changes to either the Part Geometry or to the Thickness feature that would allow the Fillet to be included in the Thickness…
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Part Design
Extracting Geometry to Add Thickness
In some cases, you have to use the “Extract” command in order to add thickness. With this command, you can generate separate Elements from initial geometry, without deleting geometry. This command is available after clicking a Dialog box prompting you to deactivate the Thickness feature and Extract the geometry. Once this operation has been done, a node “Extracted Geometry” is displayed in the tree.
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If the Generative Shape Design Workbench is installed, the geometry resulting from the Extract operation is associative.
Instructor Notes:
Note that the Thickness feature (and other Advanced Dress-Up Features) will sometimes give you the option to Extract geometry when an Definition Error for a the feature is encountered. Point out that a new Open Body will be created in the Specification Tree and the Extracted Geometry will be stored under it. This gives you the option to analyze the problem and find other solutions.
Solicit questions from the students on Dress-Up Features.
When questions have been answered, continue on to the Summary of this section…
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Part Design
Dress-Up Features: Recap Exercises You will Practice the concepts learnt in this lesson to build a exercise following a recommended process.
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Plastic Molded Bracket Crank Handle Bracket
Instructor Notes:
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Part Design
Plastic Molded Bracket Dress-Up Features Recap Exercise 15 min
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In this exercise you will : Design the part to use it in an assembly and prepare it for manufacturing. Design the Rough Part and make it thicker in order to meet the manufacturing requirements. Apply a Draft to enable its withdrawal by Molding manufacturing process. Apply Fillets. Create threaded Holes.
Instructor Notes:
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Part Design
Crank Handle Bracket Dress- Up Features Recap Exercise 20 min
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In this exercise you will : Design the part to use it in an assembly and prepare it for manufacturing. Create a Pad apply fillet on it. Add advanced draft to add material to part with non symmetrical parting surface. Apply advanced draft with different angle values above and below the parting surface.
Instructor Notes:
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Part Design
To Sum Up This concludes the lesson on the Dress up features
You have seen the Possibilities of Advanced drafts. Using apply thickness tool enables to apply thickness to a solid and helps to improve the productivity during Modification stage.
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By removing faces you can remove the faces of a complex solid so as to easily perform Finite element analysis.
Instructor Notes:
Summarize what has been learned in the Dress-Up Features section.
When ready, continue on to review Part Analysis…
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Part Design
Part Analysis You will learn how to use different kinds of analyzing tools
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Introduction to Part Analysis Analyzing Threads and Taps Draft Analysis Surfacic Curvature Analysis Part Analysis: Recap Exercises Sum Up
Instructor Notes:
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Part Design
Introduction Different kinds of analysis tools are available:
Threads and Taps Analysis: Useful when you want to visualize threads and taps contained in a part and to have all information about them:
Draft Analysis:
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This tool is used to analyze the ability of a part to be extracted for mold design:
Surfacic Curvature Analysis: Used to detect defaults on high quality surfaces:
Instructor Notes:
Now we will review several tools used to perform Design Analysis functions on Parts: Threads and Taps Analysis, Draft Analysis and Surfacic Curvature Analysis…
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Part Design
Analyzing Threads and Taps
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You will learn how to display and filter out information about threads and taps contained in a part
Instructor Notes:
You will now learn about Analyzing Thread and Taps in a Part Design…
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Part Design
What is Thread and Tap Analysis ? When a part has been created with threads and taps, CATIA does not physically display these features. There is a way to quickly know all the information about threads and taps by using the Thread and Tap Analysis icon • You can display threads or taps or both
• You can display the threads and taps numerical values
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• You can display threads or/and taps of a given diameter value
Instructor Notes:
Explain the purpose of Thread and Tap Analysis in visualizing instances of Thread or Taps defined in a Part. Point out that this Geometric Visualization can consist of Symbolic Geometry for the feature or a Numerical Value call-out or both. These visualizations are only displayed when you are in the Thread and Tap Analysis dialogue box. Note that Filters can also be applied to narrow your choices for visualization. You can show only Threads or only Taps or both. You can also limit the visualization to a specific Diameter by keying-in the value. Emphasize that this is a highly convenient way to identify all thread information in your Part Design.
Let’s look at this capability in more depth…
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Part Design
Analyzing Threads and Taps (1/2) You can display and filter out information about threads and taps contained in a Part
1
Select the Tap – Thread Analysis icon
3 To show the threads or taps geometry
2
Select the criteria that will define the types of thread / tap that will be displayed To show threads
Expand the dialog box using the More button
To show taps
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To show the threads or taps values
To show diameters with a given value
Instructor Notes:
Show the students where they can access the Analyzing Threads and Taps tool. Explain the various Geometric Visualization and Filter options. Point out the use of the More button to access the Filters options…
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Part Design
Analyzing Threads and Taps (2/2) Select Apply in the dialog box
You get:
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4
Instructor Notes:
Point out that clicking the Apply button causes the Analysis to be performed based on the currently selected options. Note that if the Visualization or Filters options are changed, you will need to click the Apply button again in order to perform the new Analysis.
Solicit questions from the students on Analyzing Threads and Taps.
When questions have been answered, continue on to Draft Analysis…
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Part Design
Draft Analysis
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You will learn how to use the Draft Analysis tool to analyze the Draft values.
Instructor Notes:
Now you will learn how to use the Draft Analysis tool to help evaluate producability of a part…
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Part Design
Why Analyze Draft? For mold design, Drafts need to be analyzed to determine the ability of the part to be extracted.
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This type of analysis is based on color ranges identifying zones on the analyzed element where the deviation from the Draft direction at any point, corresponds to specified values.
Instructor Notes:
Explain the purpose of Analyze Draft and its importance in determining the producability of a part manufactured through a molding or casting process. Note that Analyze Draft does this through Color Visualization on the part which is done by assigning various Draft Ranges to specific colors.
Let’s see how this works…
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Part Design
Draft Analysis (1/3) 1
Select the Material option in the View -> Render Style -> Customized View command to see the analysis results on the selected element.
2
Select the Draft Analysis icon
3
In the Draft Analysis dialog box, choose the quick analysis mode (default mode) or the full analysis mode.
and the element you want to analyze.
4 Double-click a color to modify the values
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in the color range or a value to modify the edition values.
Quick
Instructor Notes:
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Full
Part Design
Draft Analysis (2/3) 4 You can activate the fly analysis check box and move
the pointer over the surface. This option allows you to perform a local analysis.
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The displayed value indicates the angle between the draft direction and the tangent to the surface at the current point.
Instructor Notes:
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Arrows are displayed under the pointer: Green arrow is the normal to the surface at the pointer location, red represent draft direction and blue arrow is the tangent.
Part Design
Draft Analysis (3/3) 5 Select
to define the new current draft direction.
A compass giving the current draft direction is displayed (the draft direction is the w axis of the compass).
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6
You can edit the compass proprieties to precisely define the draft direction.
The red areas represents all that cannot be extracted with the current draft direction.
Instructor Notes:
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Part Design
Surfacic Curvature Analysis
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You will learn how to use the Mapping Analysis tool to analyze surface curvature.
Instructor Notes:
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Part Design
Why Curvature Analysis? Curvature analysis of surfaces in generally used to help model high quality surfaces ie to detect the defaults on high quality surfaces. The Mapping analysis tool allows you to measure minimum and maximum curvature values of a point, the mean value (Gaussian analysis) and to see the inflection areas.
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Gaussian
Minimum (Maximum) : to display the minimum (maximum) curvature value.
Instructor Notes:
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Inflection area : to define the curvature orientation. In green : areas where the minimum and maximum curvatures have a same orientation, In blue : they have opposite orientation.
Limited : to check if tool with an end radius can mill the part.
Part Design
Performing a Surfacic Curvature Analysis 1
Select the Material option in the View -> Render Style -> Customized View command to see the analysis results on the selected element.
2
Select the Curvature Mapping icon examine the curvature.
3
The Surfacic Curvature dialog box appears. Select Gaussian as Analysis Type.
and the surface where you want to
4 Adjust the color range fields right clicking on the thresholds values.
… you obtain :
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On the fly enables to perform a local analysis
Instructor Notes:
Explain that the same Rendering Style and Performances Options set up for Draft Analysis also apply to Surfacic Curvature Analysis displays. Point out how to access the tool and switch to the various Analysis Modes. Note that Threshold Value Ranges and Colors can be modified by double-clicking. Also point out that an On The Fly option is available to get information at a specific point on the Surface.
Solicit questions from the students regarding Surfacic Curvature Analysis.
When questions have been answered, continue on to Checking Dependencies Between Features…
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Part Design
Part Analysis Exercises Recap Exercises 25 min
In this step you will create :
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Performing a Curvature Analysis Performing a Structure Scan Object Performing an Update Scan Object Performing a Tap and Thread Analysis Performing a Draft Analysis
Instructor Notes:
25 Min
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Part Design
To Sum Up This concludes the lesson on the Part Analysis tools. You have learned how to:
Analyze Threads and Taps:Used when you want to visualize threads and taps in a part and to have all information about them>you can apply filters on the selection. Analyze Drafts:This tool is used to analyze whether a part can be extracted for mold design.A Color range is displayed identifying different zones of the analyzed part.
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Analyze Surfacic Curvature:Used to detect faults on high quality surfaces.
Instructor Notes:
Summarize what the students have learned in the Part Analysis Tools section.
Solicit questions from the students on the topics covered.
When questions have been answered, continue on to Part Manipulations…
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Part Design
Annotations You will learn how to add annotations in the 3D area
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Introduction to Annotations Text with Leader Flag Note with Leader Annotations Recommendations Annotations: Recap Exercises Sum Up
Instructor Notes:
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Part Design
Introduction You will see how to add text information attached to a part in the 3D geometry
Text with Leader: This tool allows you to add text attached to a part:
Flag Note with Leader:
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This tool allows you to add flag note attached to a part :
Instructor Notes:
Now you will learn how to attach Annotations to 3D Geometry. You will find out how to use Text with Leader and Flag Note with Leader Annotation Sets…
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Part Design
Text with Leader
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You will learn how to attach a text to a part
Instructor Notes:
Now you will learn how to attach Text with Leader to a Part…
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Part Design
What are Texts with Leader ? A text with leader can be attached to a part in order to give information for example on surface treatment. This text can appear on the drawing
Text
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Leader
Instructor Notes:
Explain what Text with Leader is used for. Point out that the Text is stored on a Planar “View” in the 3D Part Document in Geometry View. Note that it appears in the Specification Tree under an Annotation Set branch and a Planar “View” name. Explain that these types of Annotations are useful for creating Design Notes in the Part Document. Point out that these Annotations can also be brought over to a Drawing using the Generative Drafting workbench.
Let’s see more about these Features…
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Part Design
Texts with Leader Select the position of the leader on the part
1
Select the Text with Leader icon
4
Place the text and the leader by dragging the arrow or the square points
2
3
Enter the text in the dialog box then select OK
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You get:
Instructor Notes:
Show how to access the Text with Leader tool and explain the process of creating this type of Annotation. Point out the Handles used to control positioning of the Text and the Leader. Explain how CATIA determines the Planar View Orientation perpendicular to the selected feature.
Let’s practice creating a Text with Leader…
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Part Design
Flag Note with Leader
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You will learn how to add hyperlinks to your document and then use them to jump to a variety of locations
Instructor Notes:
Explain that Flag Note with Leader is very similar to Text with Leader except that you can associate Links to other documents within them. Let’s see how this works…
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Part Design
What are Flag Notes with Leader?
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A flag note with leader can be attached to a part in order to give information for example on surface treatment. This flag is an hyperlink that can start any documents such as a presentation, a Microsoft Excel spreadsheet or a HTML page on the intranet
Instructor Notes:
Explain the purpose of a Flag Note with Leader. Point out that any type of document can be linked to via the Flag Note. This not only includes standard document types such as documents, spreadsheets and presentations– but can also be scanned image files, pdf’s and even other CATIA documents.
Let’s see more about this type of Annotation…
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Part Design
Flag Notes with Leader (1/2)
1
Select the Flag Note with Leader icon
2
Select the position of the leader on the part
Enter Part Process in the Name field
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3
Instructor Notes:
Explain how to access the Flag Note with Leader tool and establish the Annotation View along with the base Flag Note text.
Let’s see how the Links are established…
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Part Design
Flag Notes with Leader (2/2) 4
Select the Browse button then select the file you want to link then select OK
5
You get:
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Place the text and the leader by dragging the arrow or the square points
Instructor Notes:
Explain how to establish a Link to the Flag Note by using the Browse button to locate the desired File. Note that a Name can be given to the Link to make it more descriptive. Point out that a single Flag Note can have Multiple Links associated with it. Explain the purpose of the Remove and Edit buttons to manage a Flag Note’s Links. Point out the use of the Go To button to follow a Link that has been previously established.
Let’s see how this Link is used…
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Part Design
Using Flag Notes with Leader 1
Double click on the flag
2
Select the Link in the dialog box
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3
Select the Go to button in the dialog box
The linked file is now started
Instructor Notes:
Explain how to access a Flag Note’s dialogue box and the use of the Go To button to activate a Link.
Solicit questions from the students about the use of Flag Notes.
When questions have been answered, continue on to Annotations Recommendations…
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Part Design
Annotations Recommendations
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You will see some hints, tips and advices about tools seen in the lesson
Instructor Notes:
Let’s review a few recommendations about Text with Leader and Flag Note with Leader…
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Part Design
Modifying a Text With Leader
To Modify the text of a text with leader, double click on the text, you will recover the dialog box where you can change the text
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Double click
Using the Properties command in the contextual menu will give you access to text, font and graphic modifications
Instructor Notes:
Explain that Double-Clicking a Text with Leader will activate the Text Editor and allow you to change the Text.
Let’s see some recommendations about Flag Note with Leader…
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Part Design
Modifying The Text of a Flag Note With Leader
To Modify the text of a flag note with leader, double click on the text, you will recover the dialog box where you can change the text
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Double click
Using the Properties option in the contextual menu will give you access to text, font and graphic modifications You can have several files linked to a flag note
Instructor Notes:
Explain the options for Modifying the content of a Flag Note. These are basically the same options as described for Text with Leader with the exception that you can also Modify Link information.
Let’s see some recommendations for Repositioning Annotation…
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Part Design
Repositioning 3D Annotation
You can use the Handles to reposition and resize the Annotation feature.
Use this handle to reposition the Annotation along its leader line
Use this handle to reposition the end of the arrow
Use top or bottom handles to move the Annotation up and down Use this handle to reposition the arrowhead
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Use middle handles to adjust the width of the Annotation box
Instructor Notes:
Explain how 3D Annotation can be repositioned and its bounds manipulated. Point out that it is not necessary to double-click to reposition the text or leader– you can drag and drop the Control Handles directly. Note that Annotation can be Hidden or Shown by selection in Geometry View or the Specification Tree.
Let’s see some other recommendations for 3D Annotations…
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Part Design
Changing 3D Annotation Properties You can modify the graphic, feature and other Properties of an Annotation through contextual menus.
Use the Properties menu to modify font color, size, feature name and other properties of the Annotation
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Use these contextual menus to modify other aspects of the Annotation
Instructor Notes:
Explain the use of the Contextual Menu to modify the Properties of an Annotation. Note the additional Contextual Menus that provide capability to further modify an Annotation. Note that Annotation is stored in a View. Additional Views can be created and Annotation can be moved between Views.
Solicit questions from students about 3D Annotations.
When questions have been answered, continue on to Summary…
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Part Design
Annotations Exercises Recap Exercises 25 min
In this step you will create:
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Creating text with a leader Creating a flag note with a leader Creating a projection view Viewing hyperlinks
Instructor Notes:
25 Min
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Part Design
To Sum Up This concludes the lesson on the annotation tools. You have learned how to:
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Create Text with Leader Create Flag Note with Leader
Instructor Notes:
Summarize what has been learned in this section.
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Part Design
Congratulations
In this course you have learned how to design parts using advanced tools and to analyse and manipulate parts …
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In addition, you have built a mobile ‘Phone Bottom Case’ following a recommended design process ...
Instructor Notes:
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