CATIA V5 Surface Design- Lesson 2: Wireframe Creation Student Notes:
Lesson 2: Wireframe Creation In this lesson you will learn how to create wireframes. Lesson Contents:
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Case Study: Wireframe Creation Design Intent Stages in the Process Reference Geometry Creation 3D Curve Creation Curve Continuity Management
Duration: Approximately 3 Hours
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CATIA V5 Surface Design- Lesson 2: Wireframe Creation
Case Study: Wireframe Creation
Student Notes:
The case study for this lesson is ‘Toy car’. The focus of this case study is to create a wireframe model of a toy car as the first stage of concept designing .You will build the model in Generative Shape Design workbench using the required wireframe tools.
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You will be given the set of reference elements using which you will create 3D wireframe geometry.
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CATIA V5 Surface Design- Lesson 2: Wireframe Creation
Design Intent
Student Notes:
The design intent is to create wireframe model of a toy car at concept stage. While you create wireframe model, you will practice several wireframe creation tools. The model should meet the following design intents:
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Create a quick model of the car considering all the dimensions of the car. This is to understand the overall shape of the model while designing it. • Create reference boxes of the size required, using a curve mesh. Create feature lines on the model to understand the shape and visual characteristics of the car. • Create a spline and connect a curve to form 3D feature lines
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CATIA V5 Surface Design- Lesson 2: Wireframe Creation Student Notes:
Stages in the Process The following steps are used to perform the case study: 1.
Create the wheel features of the car.
2.
Create bonnet feature curves.
3.
Create lower door features.
4.
Create roof features
4
3 2
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CATIA V5 Surface Design- Lesson 2: Wireframe Creation
Step 1: Reference Geometry Creation
Student Notes:
In this step, you will learn about reference geometries and how to create them. Use the following steps: 1. Reference Geometry Creation 3D Curve Creation Curve Continuity Management
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2. 3.
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CATIA V5 Surface Design- Lesson 2: Wireframe Creation
What is a Reference Geometry?
Student Notes:
Reference geometries are the basic elements, which provide a stable support to your geometry. As the design matures, the designer can use these initial reference elements to design more intricate wireframe and surface geometries. A reference geometry can be used to limit and control the overall size of the part. Reference elements can be renamed based on its functionality in the model, thus helping you to identify and reuse it at any stage of the design process.
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It is important to rename the Reference elements, in order to make the model easy to understand during concurrent engineering.
Let us see an example of reference geometry and discover the simple features that can be used to create it (L2_CONCEPTS.CATPart/REFERENCE_GEOMETRY)
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CATIA V5 Surface Design- Lesson 2: Wireframe Creation Student Notes:
Type of Reference Geometries (1/4) Following is the list of Point creation options: Name
Icon
Geometry
Point
You can create a point at any location in the 3D space by specifying references and selecting the type.
Points and Planes Repetition
You can create multiple points along a curve, a line or an edge. In the example shown, four points are created equidistant from each other on a spline.
Extremum Direction
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Description
Polar Extremum
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You can create points, edges or faces that represent the minimum or maximum locations along a curve, a surface or a pad feature. In the example shown, the point represents the maximum location along the curve in the direction shown. You can create an element that represents the minimum or maximum radius, or angle to a reference of a contour. In the example shown, a minimum radius point is created on the arc, using the plane as the support and the sketch origin and H axis for direction.
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CATIA V5 Surface Design- Lesson 2: Wireframe Creation Student Notes:
Type of Reference Geometries (2/4) Following is the list of Line creation options: Name
Icon
Line
Axis
Description You can create a line by specifying the references based on the selected type. In the example shown, a line is created between two existing points.
You can create an axis through the existing circular elements.
You can create a Polyline by joining two or more points, forming a line made up of several connected segments. These linear segments can also be connected by a blending radii.
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Polyline
Geometry
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CATIA V5 Surface Design- Lesson 2: Wireframe Creation Student Notes:
Type of Reference Geometries (3/4) Following is the list of Plane creation options:
Type
Geometry
Description Creates a plane parallel to a reference plane, offset at a distance.
Parallel Plane through a Point
Creates a plane parallel to a reference plane passing through a specified point.
Plane at an Angle or Normal to another Plane
Creates a plane at an angle to a reference plane, based on the rotation axis.
Plane through Three Points
Creates a plane passing through three point.
Plane through Two Lines
Creates a plane passing through two lines.
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Offset Plane
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CATIA V5 Surface Design- Lesson 2: Wireframe Creation Student Notes:
Type of Reference Geometries (4/4) Following is the list of Plane creation options (continued):
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Type
Geometry
Description
Plane through a Point and a Line
Creates a plane passing through a point and a line.
Plane through a Planar Curve
Creates a plane passing through a planar curve.
Plane normal to a Curve
Creates a plane normal to a curve at a specified point.
Plane Tangent to a Surface
Creates a plane tangent to a surface passing through a point.
Plane by an Equation
Creates a plane by defining the components of the plane equation.
Mean Plane through a Point
Creates a plane defined as a mean through three or more points.
Let us see an example of reference geometry and discover the simple features that can be used to create it (L2_CONCEPTS.CATPart/ REFERENCE_GEOMETRY)
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CATIA V5 Surface Design- Lesson 2: Wireframe Creation Student Notes:
What is a Local Axis? A local axis is a user-defined axis system that can be used to define local coordinates. For example, it is often easier to build a point by coordinates with respect to a local axis rather than creating it in the absolute coordinates system. An axis system can automatically be generated when a new part is created. This axis system is defined at the origin of the model and uses the default reference planes for direction.
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Local Axis System
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CATIA V5 Surface Design- Lesson 2: Wireframe Creation Student Notes:
Types of Local Axis Systems The following types of local axis systems can be defined:
A
A. The Standard axis system is defined by an origin and three orthogonal directions. B. The Rotation axis system is defined by an origin, three orthogonal directions, and an angle based on the selected reference. C. An Euler axis system uses Euler angles to define its orientation.
B
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C
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CATIA V5 Surface Design- Lesson 2: Wireframe Creation Student Notes:
Creating a Local Standard Axis Use the following steps to create a local standard axis system: 1.
Select the Axis System icon.
2.
Select the local axis origin point.
3.
To set an axis direction, select the X axis field and define X direction of the Axis System.
4.
Select in the Y axis field and define Y direction of Axis System (The direction of the third axis will automatically be defined based on the previous selections).
5.
Select the Reverse option to reverse the axis direction, if necessary.
6.
Click OK to create the axis.
3 2
1
4
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CATIA V5 Surface Design- Lesson 2: Wireframe Creation
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Setting a Local Axis as Current 1.
By default, the last created axis system becomes the active system. The axis system that is current, is highlighted in the specification tree, and is displayed with solid lines on the model. All other axis systems are displayed as dashed lines on the model.
2.
To change the active axis system, right-click on the system that needs to be made current and select Axis System.x object > Set as Current.
Student Notes:
Let us see an example of axis system use (L2_CONCEPTS.CATPart/AXIS_SYSTEM)
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CATIA V5 Surface Design- Lesson 2: Wireframe Creation Student Notes:
Step 2: 3D Curve Creation In this section, you will learn what are Curves and Wireframes, and how to create them.
Use the following steps : Reference Geometry Creation
2.
3D Curve Creation
3.
Curve Continuity Management
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1.
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CATIA V5 Surface Design- Lesson 2: Wireframe Creation Student Notes:
Concept of Curve Continuity A curve is said to be Continuous when the vertices of two curves join to form a single curve. The Continuities are of three types: A.
B.
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C.
Point Continuity: If the distance between two vertices of the connecting curve is within (Less than) specified CATIA V5 tolerance, then the curves are said to be Point Continues. If the angle between two normal curves at the connecting points is equal to zero or 180deg then the curves are said to be Tangent Continues.
A
Point Discontinuity
Point Continuity
Tangent Discontinuity
Tangent Continuity
B
C
Curvature Continuity: It is the ratio of the change in the angle of a tangent that moves over a given arc to the length of the arc.
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Curvature Discontinuity
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CATIA V5 Surface Design- Lesson 2: Wireframe Creation Student Notes:
The Tension Concept Changing Tension
In Generative Shape Design (GSD), you can apply different tension values to curves to achieve the required shape of the curve.
Curve 1
A
Let us understand the impact of tension on a curve with an example of Connect curve. A. B.
The tension value at curve 2 is kept constant at default value (T=1) and the tension value at curve 1 is varied.
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•
T2
T3
T4
T1 Constant Curve 2
The tension value at curve 1 is kept constant at default value (T=1) and the tension value at curve 2 is varied
Observations: •
T1
You will observe that when the tension value increases from T1 to T4 the connect curve (constrained with tangent continuity) changes its curvature. You can apply different tension values at both the ends to attain desired shape of the curve. The curve still maintains the continuity constraints with its parent curve at different tension values.
T1 Constant Curve 1
B
T4
T3
T2 T1
Changing Tension Curve 2
See the influence of the tension (L2_CONCEPTS.CATPart/TENSION)
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CATIA V5 Surface Design- Lesson 2: Wireframe Creation Student Notes:
Curves Created from Scratch In GSD you can create primary curves, independent of the existing curves in the part. These curves are created from scratch using the reference elements as inputs. You can create a curve from scratch using the following tools.
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Tools
Geometry
Description
Spline
Creates a curve passing through points on which you can impose tangency conditions.
Circle
Creates a complete or partial circle by defining parameters such as center, radius and tangency.
Helix
Creates a helical curve oriented by an axis.
Spiral
Creates a spiral curve defined on a support
Spine
Creates a curve normal to a list of ordered planes or planar curves
Polyline
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Creates a single element consisting of multiple line segments.
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CATIA V5 Surface Design- Lesson 2: Wireframe Creation Student Notes:
Creating a Spline 1
Let us see how to create a Spline.
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In this example we have a set of points as reference elements to create the Spline. Use the following steps to create a Spline: 1.
Select the Spline icon.
2.
Select the first point of the Spline.
3.
Successively, select the points through which the spline should pass. In this case, the spline defines the shape of the bottle.
4.
Select a. The tangency direction at the start and end points of the spline. b. By default, the tension value of the spline at each point is 1. Modify the tension values at the start and end points to get the desired shape of the bottle.
5.
Click OK to generate the Spline.
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4a
4b
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CATIA V5 Surface Design- Lesson 2: Wireframe Creation Student Notes:
Curves for Connecting Existing Curves In many design cases, you come across situations where you may have to: A. Create a connecting curve between two existing curves and at the same time maintain the continuity constraints. B. Create a round corner between two 3D curves. C. Use the spline to connect existing curves. These curves can be created using GSD tools like Connect Curve and Corner respectively. You will now study (in detail) about these curves.
A
Connect Curve
B
3D Corner
C
Spline
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A Corner created between two 3D curves
3D Curve Curve connecting the existing curves Let us see these tools (L2.CATPart/CONNECTING)
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CATIA V5 Surface Design- Lesson 2: Wireframe Creation Student Notes:
Creating a Connect Curve (1/2) Connect Curve is a tool used to create an intermediate curve between two existing curves.
1
The designer can define the type of connection, such as Point, Tangency or Curvature, at each end of the connecting curve to achieve the desired continuity. You can also apply the tensions at both the ends of the connecting curve to control the stiffness of the curve. Hence, the shape of the connect curve is driven by the tension applied on it.
2 3
Use the following steps to create a Connect Curve: 1. 2. 3.
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4. 5.
Select the Connect curve icon. Select the first point. If required, select the curve for the first point. Select the second point. If required, select the curve for the second point.
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CATIA V5 Surface Design- Lesson 2: Wireframe Creation Student Notes:
Creating a Connect Curve (2/2) Use the following steps to create a Connect Curve (continued..) 6.
7. 8.
Define the type of continuity for each point. Continuity can be defined as: a. Point b. Tangency c. Curvature If required, change the default tension values. Click OK to generate the Connect Curve.
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Curve 1 : Tangency Curve 2 : Tangency
Curve 1 : Point Curve 2 : Point
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Curve 1 : Tangency Curve 2 : Point
Curve 1 : Point Curve 2 : Curvature
Curve 1 : Tangency Curve 2 : Curvature
7 7
6 Observe the change in continuity by changing the continuities.
Curve 1 : Curvature Curve 2 : Curvature
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CATIA V5 Surface Design- Lesson 2: Wireframe Creation Student Notes:
Creating a 3D Corner Use the following steps to create the Corner curve: 1. 2. 3. 4. 5. 6. 7.
1
Select the Corner icon. Select the first curve. Select the second curve. Select the support plane or surface (if you have opted for Corner on support option). Select the direction (if you have opted for 3D Corner option). Specify the radius of the corner. Click OK to generate the Corner Curve.
2 3 4
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CATIA computes the direction automatically.
5
If you have opted for Corner type as ‘Corner on support’. You will be specifying the support.
Let us see these tools (L2.CATPart/CURVES_ON_SUPPORT)
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CATIA V5 Surface Design- Lesson 2: Wireframe Creation Student Notes:
Curves Based on Supporting Surfaces In certain design situations you may need curves that use a surface as a support. These curves are either derived from the surface or they use it as a supporting element to create other elements of the model.
Boundary curve Spline Circle
Let us learn more about these curves using the following categorization: A. Curves such as Boundary, Intersect and Isoparametric can be derived using the existing surfaces. B. Curves such as Parallel, Project, Corner, Reflect Line, Spiral and Conic lie on the surface.
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C. While curves such as Line, Spline, and Circle can be created using surface as the supporting element (optional).
Parallel Curve
Let us see these tools (L2.CATPart/CURVES_ON_SUPPORT)
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CATIA V5 Surface Design- Lesson 2: Wireframe Creation Student Notes:
Creating a Boundary (1/2) Boundary tool creates boundary curves on the internal or external surface edges.
A
While defining the boundary, only one element needs to be selected. Using the correct propagation type, the remaining boundary is automatically determined. The propagation of a selected edge can be defined by: A.
Complete Boundary
B.
Point continuity
C.
Tangent continuity
D.
No propagation
B
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C
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CATIA V5 Surface Design- Lesson 2: Wireframe Creation Student Notes:
Creating a Boundary (2/2) Use the following steps to create a boundary: 1. Select the Boundary icon.
1
2. Specify the propagation type. 3. Select the surface edge.
2
4. If necessary, limit the boundary curve using points or vertices. a. Click on the Limit1 field. b. Select the first limiting element in the geometry. c. Click on the Limit2 field.
4a
4c
5
d. Select the second limiting element.
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5. Click OK to generate the boundary curve.
4b
3
4d Let us see these tools (L2.CATPart/CURVES_ON_SUPPORT)
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CATIA V5 Surface Design- Lesson 2: Wireframe Creation Student Notes:
Creating a Parallel Curve (1/2) Parallel Curve tool is used to create curves parallel to a reference curve on a specified support. You can specify the offset value for a parallel curve. When specifying the offset value in constant field, CATIA calculates the distance using two modes. They are:
Original Curve
Geodesic result
A. Geodesic Mode B. Euclidean Mode
A Equal offset Geodesic result
B
Support
Euclidean result
Euclidean result
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Original Curve
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CATIA V5 Surface Design- Lesson 2: Wireframe Creation Student Notes:
Creating a Parallel Curve (2/2) Use the following steps to create a Parallel Curve : 1. Select the Parallel Curve icon.
1
2. Specify the reference curve. 3. Select the support plane or surface on which the reference curve lies.
2
4. Specify the offset of the parallel curve either by
3 4a
a. Specifying a value or using the graphic manipulator in the Constant field.
4b
b. Selecting a point in the Point field (in both Geodesic and Euclidean mode) In which case, the Constant field is disabled.
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5. Click OK to generate the Parallel Curve.
5
Let us see these tools (L2.CATPart/CURVES_ON_SUPPORT)
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CATIA V5 Surface Design- Lesson 2: Wireframe Creation
Exercise 2A Start
Student Notes:
Recap Exercise 10 min
In this exercise you will practice how to create reference elements. You will create reference elements for the wireframe model of a Table Lamp. Detailed instructions for this exercise are provided. By the end of this exercise you will be able to: Create reference elements such as Plane and Axis systems
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Create 2D wireframe elements such as Line and Point
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CATIA V5 Surface Design- Lesson 2: Wireframe Creation Student Notes:
Exercise 2A Start (1/7) 1. Create a new part and access the Generative Shape Design workbench To create a new part file, select Part from the New dialog box. a. Click File > New. b. Choose Part from the New dialog box. c. Click OK. d. Enter the new part name as – Table Lamp e. Click OK.
1b 1d 1c 1e
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To access workbench from start menu. a. Click Start > Shape >Generative Shape Design.
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CATIA V5 Surface Design- Lesson 2: Wireframe Creation Student Notes:
Exercise 2A Start (2/7) 2.
Create an Axis System Create an axis system at the co-ordinate -
X = 200, Y= 0, Z= 0.
2b
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a. Select Insert > Axis System. b. Right-click on Origin selection box to create point for Axis origin as shown. c. In the Point creation dialog box specify the the following coordinate X = 200, Y= 0, Z= 0. d. Click OK to create the Point. e. Click OK in the Axis system dialog box to create an Axis system at a specified Point. f. Rename the Point created as Reference Point.
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2e
2c
2d
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CATIA V5 Surface Design- Lesson 2: Wireframe Creation
Exercise 2A Start (3/7) 3.
Student Notes:
Create a set of Points Create a set of points on YZ plane of Axis System.1 a. Point A , H = 42, V = 28 b. Point B , H = -21, V = 117 c. Point C , H = -28, V = 155 d. Point D , H = 46, V = 213 e. Point E , H = -50, V = 0 Point C Point D
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Point B
Point A
Point E
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CATIA V5 Surface Design- Lesson 2: Wireframe Creation Student Notes:
Exercise 2A Start (4/7) 4a
4. Create a Line Create Line using Point-Direction option. a. Select Line Icon. b. Select Point A as a point input. c. Select Z axis for direction. Use Reverse Direction to change the direction of the line if needed. d. Specify [30mm]. e. Click OK to generate a Line.
4b 4c 4d
5. Create an Axis System
5b
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Create an Axis system.2 at Point D. a. Select Insert > Axis System. b. Select Point D as Origin. c. Rotate the Axis System along X axis by [-15 deg]. d. Click OK.
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5c
5d
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CATIA V5 Surface Design- Lesson 2: Wireframe Creation Student Notes:
Exercise 2A Start (5/7) 6.
Create a set of Points Create a set of points on XY plane of new Axis system. a. Point F , H = -35, V = 50 b. Point G, H = 35, V = 50 c. Reference Point : Point D
6a
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6b
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CATIA V5 Surface Design- Lesson 2: Wireframe Creation Student Notes:
Exercise 2A Start (6/7) 7.
Create a Plane Create a Plane, using Plane Type Parallel through point Option. a. Select a Plane Icon. b. Select Plane type Parallel through point option c. Select XY plane of Axis system.1 as parallel plane d. Select Point G as input point for Plane location. e. Click OK.
7a
7c 7d 7e
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7d
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CATIA V5 Surface Design- Lesson 2: Wireframe Creation Student Notes:
Exercise 2A Start (7/7) 8.
Create a Point Create a Point, using Point type On plane option. a. Click on Point Icon. b. Choose Point type On Plane Option. c. Select Plane Created in the previous step as support. d. Specify the coordinate- H = 0, V = 5 e. Select Point A as the Reference point. f. Click OK. Rename the point as Point H.
8a
8b 8c 8d 8e
8f
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8d
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CATIA V5 Surface Design- Lesson 2: Wireframe Creation
Exercise 2A Start : Recap
Student Notes:
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Create reference elements such as Planes, Axis systems, Points and Lines.
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CATIA V5 Surface Design- Lesson 2: Wireframe Creation
Exercise 2A End
Student Notes:
Recap Exercise 20 min
In this exercise you will practice how to create 3D wireframe elements. You will complete the wireframe model of a Table Lamp. Detailed instructions for this exercise are provided.
By the end of this exercise you will be able to: Create 2D wireframe elements such as Circle and Line
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Create 3D wireframe elements such as Spline and Connect curve
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CATIA V5 Surface Design- Lesson 2: Wireframe Creation Student Notes:
Exercise 2A End (1/9) 1.
Create a Circle
Browse and open the part Exercise_2A_End_Initial.CATPart Create a Circle with radius 70mm and the Reference point as centre. a. b. c. d. e.
Specify [70mm] radius. Create a semi-circle from [0deg to 180 deg] Click OK to create Circle.
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f.
Click on Circle Icon. Choose Reference point as Circle center. Select XY plane of Axis System.1 as support plane.
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1a
1b
1e
1c 1d
1f
R 70
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CATIA V5 Surface Design- Lesson 2: Wireframe Creation Student Notes:
Exercise 2A End (2/9) 2.
Create a Line Create a Line using the Point-Direction option. 2a a. Select Line Icon. b. Select Point.E as a point input. c. Select X axis for direction. d. Specify [30mm] length and select Mirrored extent option. e. Click OK to generate a Line.
2b 2c
2d 30
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2e
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CATIA V5 Surface Design- Lesson 2: Wireframe Creation Student Notes:
Exercise 2A End (3/9) 3.
3a Create a Connect Curve Create a Connect Curve between Circle and Line (as shown). a. Click on Connect curve Icon. b. Select one end point of the semi-circle. By default the circle is selected as the first connecting curve. c. Select the corresponding end point of the Line. By default line is selected as the second connecting curve. d. Change the direction of the connect curve, if required. e. Change the tension value of the Connect curve to adjust the shape, if required. f. Click OK to create Connect Curve
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Repeat the operation to connect two other ends of the Circle and Line.
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3b
3c
3f
Connect Curve
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CATIA V5 Surface Design- Lesson 2: Wireframe Creation Student Notes:
Exercise 2A End (4/9) 4.
Create a Spline
4a
Create a Spline using Point.A to Point.D. a.
Click on Spline Icon.
b.
Select Point A as the first input point (as shown). Use previously created line to specify tangent direction.
c.
Select Point.B and consecutively Point.C and D.
d.
Reverse the tangent direction, if required.
e.
Click OK to create the Spline.
4b
Rename the feature as Spline.A
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4e
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CATIA V5 Surface Design- Lesson 2: Wireframe Creation Student Notes:
Exercise 2A End (5/9) 5.
Create a 2D Circle 5a Create a Circle with Two points and radius Option. a. Click on Circle Icon. b. Select Point.D and then Point.G through which the circle passes. c. Specify [50mm] radius and XY plane of Axis System.2 as support d. Click OK to create a Circle. e. Rename the circle as Circle.A. Repeat the operation for creating circle between Point. F and Point.D ( Rename the circle as Circle.B )
5b 5c
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5d
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Circle B
Circle A
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CATIA V5 Surface Design- Lesson 2: Wireframe Creation Student Notes:
Exercise 2A End (6/9) 6.
Create a Line 6a Create a Line using Point- Direction option. a. Select Line Icon b. Select Point.F as a point input. c. Select X axis for direction. d. Specify 5mm towards the direction shown. e. Click OK to generate a Line Repeat the operation to create the line from Point. G. Rename both lines as Line.A and Line.B
6b 6c
6d
Line A
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m 5m
Line B
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m 5m
6e
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CATIA V5 Surface Design- Lesson 2: Wireframe Creation Student Notes:
Exercise 2A End (7/9) 7.
Create a 2D Circle 7a Create a Circle with Two points and radius Option. a. Click on Circle Icon. b. Select end points of the lines created in the previous operation. c. Specify [33mm] radius. d. Select plane.1 previously created as a support. e. Click OK to create a 2D Circle.
7b 7d 7c
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7e
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CATIA V5 Surface Design- Lesson 2: Wireframe Creation Student Notes:
Exercise 2A End (8/9) 8.
Create a Spline Create a Spline passing through the three points
8a
a.
Click on Spline Icon.
b.
Select end Point of Line.A as the first input point (as shown).
c.
Select Point.H
d.
Select end point of Line.B.
e.
Reverse the tangent direction, if required.
f.
Click OK to create the Spline.
8f 8c 8b
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8d
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CATIA V5 Surface Design- Lesson 2: Wireframe Creation Student Notes:
Exercise 2A End (9/9) 9.
Create a Corner
9a
Create a 3D Corner between Spline and Circle as shown. a.
Click on Corner Icon.
b.
Select Circle.A as the first input element (as shown).
c.
Select Spline.A as the second input element.
d.
Specify [50mm] radius.
e.
Specify Axis System.2 X axis as direction.
f.
Click OK to create a Corner.
9c 9e 9d 9f
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Repeat the Operation to create a 3D corner between Spline.A and Circle.B. 3D Corner
9b
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CATIA V5 Surface Design- Lesson 2: Wireframe Creation
Exercise 2A End: Recap
Student Notes:
Create 2D wireframe elements such as Circle and Line.
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Create 3D wireframe elements such as Spline and Connect curve.
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CATIA V5 Surface Design- Lesson 2: Wireframe Creation
Exercise 2B
Student Notes:
Recap Exercise 20 min
In this exercise, you will practice on some of the tools in 3D curves creation of GSD workbench.You will be provided with a set of points of a mirror shell model. You will be creating a basic curve using the points data. High-Level instructions for this exercise are provided. By the end of this exercise you will be able to: Create a 2D Spline and an Arc. Create a 3D Spline and a Connect curve
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Create a Combine curve and a Curve project.
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CATIA V5 Surface Design- Lesson 2: Wireframe Creation Student Notes:
Exercise 2B (1/5) 1. Open the part. Open an existing part file 1 Exercise_2B_Start.CATPart The file consists of Scanned points and construction planes.
2. Inspect the Point data with ‘Quick view’ Icons. Select the FRONT, LEFT and TOP icons. You should be able to determine that the green and red set of points are three dimensional, and the yellow and blue set of points are linear.
2
3
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3.
Project the points on the given planes. Project the Green points on the Green and Pink Construction planes.
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CATIA V5 Surface Design- Lesson 2: Wireframe Creation Student Notes:
Exercise 2B (2/5) 4.
Create a partial curve on the Pink plane in a Sketcher using the points projected.
4
5.
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6.
Create a sketch with a Spline using the projected points.
5
Repeat steps 3 ,4 and 5 for Red set of points. Project the Red points on the Pink and Red plane Using these projected points create partial circles on the Pink plane, and Spline on the Red plane using a sketcher.
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CATIA V5 Surface Design- Lesson 2: Wireframe Creation Student Notes:
Exercise 2B (3/5) 7.
Combine 2D curve into 3D shapes. Use the Combine tool to create 3D curve from the first and second sketched curve.
7
Similarly, combine the curves third and fourth to create a 3D curve.
8.
Create Line over Yellow and Blue set of points. Create a Line using the point to point option.
9.
8
Create a point on 3D Curve. Create a point on both the combine curves at a distance ratio of 0.1 from both the ends of the curve.
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9
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CATIA V5 Surface Design- Lesson 2: Wireframe Creation
Exercise 2B (4/5)
Student Notes:
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At this stage the part should look like this.
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CATIA V5 Surface Design- Lesson 2: Wireframe Creation Student Notes:
Exercise 2B (5/5) 10. Create a 3D Spline. Create a Spline at the corner where the Red and Blue points meet. Similarly, create a Spline at the corner where the Green and Blue points meet.
Tangent Direction for Point1 Tangent Direction for Point2
11. Create a Curve Connect. Create a Connect Curve at the corner where the Red and Yellow points meet.
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Similarly, create a Connect Curve at the corner where the Green and Yellow points meet.
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CATIA V5 Surface Design- Lesson 2: Wireframe Creation Student Notes:
Exercise 2B: Recap Create a 2D Spline and an Arc. Create a 3D Spline and a Connect curve. Create a Combine curve and a Curve project.
3D Spline
Combine Curve Line
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Connect Curve
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Point on Curve
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CATIA V5 Surface Design- Lesson 2: Wireframe Creation
Exercise 2C
Student Notes:
Recap Exercise 15 min
In this exercise, you will practice how to create 3D wireframes with surface support. You will be given a datum surface of sunglasses. You will be creating the feature profiles of sunglasses using the surface support. High-level instructions for this exercise are provided. By the end of this exercise you will be able to: Extract Boundary of an existing surface. Create a parallel curve using the surface support. Create a Corner using the surface support. Copyright DASSAULT SYSTEMES
Create points on the surface. Create 3DSpline on a surface.
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CATIA V5 Surface Design- Lesson 2: Wireframe Creation Student Notes:
Exercise 2C (1/3) 1.
2.
Open the part. Open an existing part file. The file consists of datum surface of sunglasses. a. Browse and open part Exercise_2C_Start.CATPart
Create a Geometrical Set. Insert a Geometrical set and rename it as Wireframes.
1
2
Boundary
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3 3.
Create a boundary Create a boundary at the top and bottom edge of the sunglass surface (as shown) using the boundary tool.
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Boundary
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CATIA V5 Surface Design- Lesson 2: Wireframe Creation Student Notes:
Exercise 2C (2/3) 4.
5.
Create a Parallel curve Create a parallel curve on the sunglass surface from boundary curves using the Parallel curve tool (4mm offset).
Create a Corner on the surface Create a corner between the two parallel curves at their intersection point using the Corner tool (5mm radius)
4
5
Parallel Curves
Corner
Points on surface
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6.
Create Points on the surface Create nine points on the surface (use more points if required) using the Point tool.
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6
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CATIA V5 Surface Design- Lesson 2: Wireframe Creation Student Notes:
Exercise 2C (3/3) 7.
Create Spline on the surface Create a Spline by joining all the previously created points on the sunglass surface.
7
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Spline
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CATIA V5 Surface Design- Lesson 2: Wireframe Creation
Exercise 2C: Recap
Student Notes:
Extract Boundary of an existing surface. Create a parallel curve using the surface support. Create a Corner using the surface support. Create points on a surface.
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Create 3DSpline on a surface.
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CATIA V5 Surface Design- Lesson 2: Wireframe Creation
Step 3: Curve Continuity Management
Student Notes:
In this section, you will learn the importance of curve continuity and how to achieve it.
Use the following steps : 1. 2.
Curve continuity Management
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3.
Reference Geometry creation 3D Curve Creation
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CATIA V5 Surface Design- Lesson 2: Wireframe Creation Student Notes:
Importance of a Continuous Curve Whenever you create a surface, it derives many of its characteristics from the wireframe used to generate it. When a house is built, the foundation is an important element in determining the quality of the resulting structure. In surface design, the wireframe should be considered as the foundation of the design. Hence great care should be taken while constructing the wireframe, both inside and outside the sketcher.
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Surfaces inherit the flaws of the parent curve. In a product development cycle, this surface would be further used in downstream operations such as prototyping, machining, tooling, etc thus affecting the final product.
Curve with small flaw, used to make a surface
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Curve will always transmit flaw to the surface
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CATIA V5 Surface Design- Lesson 2: Wireframe Creation
Geometrical Continuity versus Topological Continuity
Student Notes:
Topology is the representation of the geometry as seen by the CAD system. The accuracy of this representation depends on the merging distance of the modeler. The merging distance is the minimum distance between two distinct geometrical points below which the modeler sees only one point. One topological D < merging point (vertex) Topological point distance: continuity between the two curves D
Two distinct geometrical points (curves extremities)
Topological point discontinuity between the two curves
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D > merging distance:
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Two distinct topological points
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CATIA V5 Surface Design- Lesson 2: Wireframe Creation
When to Check the Continuity of Curves?
Student Notes:
Curves generated in CATIA V5 are most likely to be continuous curves. CATIA provides Tolerant modeling features which can overcome some of the problems that may occur at the time of curve creation. Continuity check on curves is mostly used for curves imported into CATIA V5. Many times when a curve is imported into CATIA V5, you may find problems such as: the curve is selfintersecting or disjoint, it has discontinuities in its tangency or curvature, leading to geometrical flaws in the model.
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Hence, you should always check the curve for the above mentioned defects and repair the curve before proceeding with surface creation.
Discontinuous Curves
Many times the defect on the curve cannot be seen with the naked eyes. In GSD you have the tools to check the continuity of curves and measure the severity of the defects.
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CATIA V5 Surface Design- Lesson 2: Wireframe Creation
Tools to Detect Geometric Connection in Curves
Student Notes:
If you have imported a curve from another application, and you want to know whether it is good before creating surfaces from it, you can use the Connect Checker Tool and Porcupine Analysis tool to detect the discontinuities. Connect Checker allows you to detect Point, Tangency, or Curvature discontinuities between two or more curves. The Connect Checker can detect :
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A. B. C. D.
A
B
The Distance between two or more curves The Tangency discontinuities The Curvature discontinuities An Overlap by highlighting the affected area
C D Let us see these tools (L2.CATPart/CURVE_CORRECTION)
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CATIA V5 Surface Design- Lesson 2: Wireframe Creation Student Notes:
Analyzing Curve Connections in Boundary Mode Use the following steps to check the connection between the curves: 1. 2. 3.
4. 5.
Select both the curves that have to be analyzed. Select the Connect Checker Tool icon. The Connect Checker Tool dialog box is displayed. You can choose the type of analysis to be performed. Click the Quick button. Select the desired check box to know the results. a. Distance: In this case, distances more than 0.1mm are highlighted. b. Tangency: Tangent discontinuities which are more than 0.5 deg are highlighted. c. Curvature: Curvature discontinuities which are more than 5% are highlighted. d. Overlapping option displays the status of overlap between two curves.
6.
2 3 4
5a 5b
Click OK to finish the Curve Analysis.
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5c
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5d
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CATIA V5 Surface Design- Lesson 2: Wireframe Creation
Curve Connection Analysis in Projection Mode
Student Notes:
The Projection mode for Curve-Curve analysis allows you to directly project the curve extremity of the first selected curve onto the second curve. The analysis is then performed between the curve extremity and its projection on the second curve. The curve selected first is the ‘Source’ curve. The curve extremities of this curve will be projected on the second curve. Similarly, the second curve selected is the ‘Target’ curve. The display of the results will be similar to Curve-Curve connection analysis in Boundary mode.
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Source Curve
Target Curve
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CATIA V5 Surface Design- Lesson 2: Wireframe Creation Student Notes:
Analyzing Curve Connections in Projection Mode Source
Use the following steps to check the connection between curves: 1. 2. 3. 4. 5.
6. 7.
Select the Connect Checker icon. Select Curve-Curve Connection analysis type and check the Projection check box. Select the Source curve and the Target curve. Click the Quick button. You can choose the type of analysis to be performed: Distance (G0), Tangency (G1), Curvature (G2) or Curvature-Tangency (G3). Define the tolerance range between 0 mm to 7 mm Select the desired continuity type to know the results. a. b.
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c. d.
8.
Distance (G0): In this case, distances more than 0.1mm are highlighted. Tangency (G1): Tangent discontinuities which are more than 0.5 deg are highlighted. Curvature (G2): Curvature discontinuities which are more than 5% are highlighted. Curvature-Tangency (G3): Discontinuities which are more than 5% are highlighted
Click OK to finish the Curve Analysis.
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1 Target
3 2 4 5
7
6
8
G0 continuity
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CATIA V5 Surface Design- Lesson 2: Wireframe Creation
The Curve Smooth Tool
Student Notes:
The Curve Smooth tool allows you to correct the discontinuities in a curve. It repairs flaws such as Point, Tangent and Curvature discontinuity of the curve. When you select the curve to be smoothened, the tool indicates the discontinuities of the curve by displaying text labels on the curve. You can obtain the desired smoothness of the curve by specifying the smoothness parameters in the Curve Smooth dialog box.
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Let us learn about the smoothening parameters in detail in the subsequent pages.
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CATIA V5 Surface Design- Lesson 2: Wireframe Creation Student Notes:
Using the Curve Smooth Tool (1/3) When you select a curve to be smoothened, the command indicates the discontinuities on the curve. You can smoothen the curve to a desired extent by specifying the Threshold value. This value sets the upper limit of the discontinuity acceptance. Discontinuities of the curve below this value are considered for correction. During the smoothening process, the curve gets deformed to achieve the specified continuity type. You can have a control on the deviation of the curve after deformation with respect to the input curve.
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The threshold values for correcting Tangency and Curvature discontinuities in a curve can be specified in the dialog box. You can decide the threshold value based on the quality acceptance criteria of your design or by the smoothness required on the curve.
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Smoothed
Not Smoothed Tangency Threshold
Tangency Threshold Not Smoothed
Smoothed
Curvature Threshold value Curvature Threshold
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CATIA V5 Surface Design- Lesson 2: Wireframe Creation Student Notes:
Using the Curve Smooth Tool (2/3) When you select a curve to be smoothened, 1. 2.
1
The discontinuities are indicated on the curve. When the required threshold values are specified in the dialog box, a smooth curve is obtained depending on the specified values.
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2
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CATIA V5 Surface Design- Lesson 2: Wireframe Creation Student Notes:
Using the Curve Smooth Tool (3/3) Use the following steps to create a smooth curve: 1. 2. 3.
Select the Curve Smooth icon. Select the curve to be smoothened. Check the value of discontinuity on the curve a. Point Continuity b. Tangent Continuity c. Curvature Continuity
4.
5.
4
Specify the Threshold value to attain the required smoothness of the curve (the threshold value also depends 5 on the quality acceptance criteria for the curve in design 6 context). Specify the Maximum deviation value. This is the deviation you want to allow between input curve and the smoothened curve. Specify the Continuity value. Click OK to get the smooth curve.
7
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6. 7.
1
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CATIA V5 Surface Design- Lesson 2: Wireframe Creation
Removing Unhealed Defects of a Curve The erroneous area of the curve such as self intersecting or overlapping cannot be healed using curve smoothen tool. Such areas of the curve have to be cropped and reconnected to achieve a smooth curve.
Student Notes:
A
In Generative Shape Design workbench (GSD), you can crop the erroneous area of the curve using the Split-Trim tools. And you can bridge the gap between the curves using curve connect tools.
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For Example: A.
The curve in the illustration is self intersecting. This can be cropped using the Split-Trim tools available in GSD workbench.
B.
The curve in the illustration is intersecting with an another curve. In order to achieve a smooth connection between the two curves, you can split them and reconnect using connect curves.
B
Let us see these tools (L2.CATPart/CURVE_CORRECTION)
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CATIA V5 Surface Design- Lesson 2: Wireframe Creation
To Sum Up
Student Notes:
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In the following slides you will find a summary of the topics covered in this lesson.
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CATIA V5 Surface Design- Lesson 2: Wireframe Creation Student Notes:
Reference Geometry Creation Reference geometries are the basic elements (planes, points, lines, axis), which provide a stable support to geometry. They can be used to design more intricate wireframe and surface geometries. A reference geometry can be used to limit and control the overall size of the part. They can also be renamed, based on its functionality in the model.
Side limiting plane
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CATIA uses a fixed coordinate system called the Absolute Axis System. Any point in the model always has coordinates specific to this axis system. You can also define an arbitrary coordinate system located anywhere in three dimensional space and oriented in any direction. This user-defined axis system is called as Local Axis System. There can be multiple axis systems in a single part.
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CATIA V5 Surface Design- Lesson 2: Wireframe Creation Student Notes:
3D Curve Creation A curve is said to be Continuous when the vertices of two curves join to form a single curve. These are of following type: A. Point Continuity: When the distance between two vertices of the connecting curve is within (less than) the specified CATIA V5 tolerance. B. Tangent Continuity: When angle between two normal curves at the connecting points is equal to zero or 180deg. C. Curvature Continuity: This is the rate of change of the angle of a tangent.
A
Point Discontinuity
Point Continuity
B
Tangent Discontinuity
Tangent Continuity
C
Curvature Continuity
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Curvature Discontinuity
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CATIA V5 Surface Design- Lesson 2: Wireframe Creation Student Notes:
Curve Continuity Management A surface derives many of its characteristics from the wireframe used to generate it. A defective surface will propagate the defect in downstream operations such as prototyping, machining, tooling, etc thus affecting the final product. Hence care must be taken while constructing a wireframe. Tools used to detect geometrical discontinuities of curves are:
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Connect Checker Analysis Porcupine Curvature Analysis
Curve with small flaw, used to make a surface
Curve will always transmit flaw to the surface
The Curve Smooth tool allows you to correct the discontinuities in a curve up to a required extent by specifying the Threshold value. This value sets the upper limit of the discontinuity acceptance. The Maximum deviation value allows to set acceptable deviation between input curve and the smoothened curve. This tool repairs flaws such as Point, Tangent and Curvature discontinuity of the curve.
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CATIA V5 Surface Design- Lesson 2: Wireframe Creation Student Notes:
Removing Unhealed Defects of the Curve The erroneous area of the curve such as self intersecting or overlapping cannot be healed using curve smoothen tool. In such situations you must remove the problem area and reconnect the curve to achieve a smooth result.
You can crop the erroneous area of the curve using the Split-Trim tools.
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Two intersecting curves can be split and reconnect using connect curves.
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CATIA V5 Surface Design- Lesson 2: Wireframe Creation Student Notes:
Main Tools Wireframe Toolbar 1
2
Points: Creates a point or multiple points.
1
Line-Axis: Creates lines, axis or polyline. 3
2 3
Plane: Creates planes using different options. 4
4
5
Circle Conic: Creates 3D curves. Curves: Creates 3D curves like Spline, Helix and Spiral.
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Analysis Toolbar 6
5
6
Connect Checker Analysis: Performs connection analysis of curves and surfaces.
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CATIA V5 Surface Design- Lesson 2: Wireframe Creation
Exercise 2D
Student Notes:
Recap Exercise 15 min
In this exercise you will perform the curve connect analysis on a set of imported curves. You will also repair the defective areas of the curve and make it smooth. Detailed instructions for this exercise are provided. By the end of this exercise you will be able to: Perform Connect Checker Analysis Create a Smooth curve. Remove the defective areas of the curve
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Fill the gap between the two curves using Connect curve.
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CATIA V5 Surface Design- Lesson 2: Wireframe Creation Student Notes:
Exercise 2D (1/7) 1. 2.
Open the part. Exercise_2D_Start.CATPart Perform Connect Checker Analysis. Analyze each imported curve for its connections and continuity.
2a
a. Click on Connect Checker Analysis Icon and 2b select Curve-Curve Connection type. b. Select the Boundary check box. c. Specify the value for Distance (G0), Tangency (G1) and Curvature (G2) above which the defects are highlighted. d. Select each curve to check its connection. e. Click OK to keep the result in the specification tree.
2C
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You will observe that the Blue curves in a set are having defects.
Tangent Discontinuity
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Curvature Discontinuity
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CATIA V5 Surface Design- Lesson 2: Wireframe Creation Student Notes:
Exercise 2D (2/7) Results of Connect Checker Analysis. Defects
Severity
Curve 1
Curvature Discontinuity
87.78%
Curve 2
Tangent Discontinuity
29.873 deg
Curve 3
Curvature Discontinuity
57.84%
Curve 4
Curvature Discontinuity Tangent Discontinuity
25.16% 11.016 deg
Curve 5
Curvature Discontinuity Tangent Discontinuity
73.44% 8.036 deg
Curve5
Curve4 Curve3 Curve1
Curve2
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Curve
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CATIA V5 Surface Design- Lesson 2: Wireframe Creation Student Notes:
Exercise 2D (3/7) 3.
Smoothen the defective curves Correct the defects of Curve.1 using Curve Smooth tool keeping the continuity type as Curvature. 3a a. b. c. d.
Click on Curve Smooth Icon. Select the Curve.1. Select Continuity type as Curvature. Click OK to get a continuous smooth curve.
Curve5
CATIA computes the threshold value for correcting Curvature defects, when the continuity type selected in the panel is Curvature. Curve4
3b
Curve3
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Curve1
Curve2
3c
3d
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CATIA V5 Surface Design- Lesson 2: Wireframe Creation Student Notes:
Exercise 2D (4/7) 4.
Smoothen the curves 4 and Curve 5 using Continuity Threshold. Curve. 4 has Tangency and Curvature defects. Smoothen the defects using Threshold option. Click on Curve Smooth Icon. Select the Curve 4. Select Continuity type as Threshold. Specify the threshold value for tangency and curvature. (For tangency, defects lying below threshold value are healed. For curvature, defects lying above threshold value are healed) e. Click OK to get a continuous smooth curve.
4a 4b
a. b. c. d.
4c
4e
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Repeat the operation on Curve.3 and Curve.5 to get a smooth curve.
4d
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CATIA V5 Surface Design- Lesson 2: Wireframe Creation Student Notes:
Exercise 2D (5/7) 5.
Remove the self intersecting areas of curves which cannot be smoothened by the Smooth tool. Extract the two intersecting parts of the Curve.2. a. b. c.
Click on the Extract icon. Select both sides of the defective curve as shown. (Two curves are extracted.) Click OK.
5a
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Curves to be Extracted
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CATIA V5 Surface Design- Lesson 2: Wireframe Creation Student Notes:
Exercise 2D (6/7) Create two Points on either sides of the defect area. d. e. f. g.
Click on Point Icon. Select Point On Curve option. Position the Point as shown. Click OK .
5d
Split the curve at both the points. The defective area is removed from the curve. Hide the Parent curve (Curve .2).
5f Point 1
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Curve Split at Points
Point 2
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CATIA V5 Surface Design- Lesson 2: Wireframe Creation Student Notes:
Exercise 2D (7/7) 6.
Fill the gap created between the curves. Connect the two curves using Connect Curve. a. b. c. d. e. f.
6a
Click on Connect Curve Icon. Select end Point of the first curve. Select end Point of the second curve. Reverse direction, if required. Select Trim Elements option. Click OK .
6e
6b
6f
End Point 1
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End Point 2
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CATIA V5 Surface Design- Lesson 2: Wireframe Creation
Exercise 2D: Recap
Student Notes:
Perform Connect Checker Analysis. Create a Smooth curve. Remove the defective area of the curve.
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Fill the gap between the two curves using Connect curve.
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CATIA V5 Surface Design- Lesson 2: Wireframe Creation
Exercise 2E
Student Notes:
Recap Exercise 15 min
In this exercise, you will be provided with a curve which has to be analyzed for its continuity and connections. No instructions will be provided for this exercise. By the end of this exercise you will be able to: Check continuity of a curve using Connecter checker.
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Perform the Porcupine analysis on a curve to check its Curvature Continuity.
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CATIA V5 Surface Design- Lesson 2: Wireframe Creation
Exercise 2E 1. 2.
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3.
Student Notes:
Load the start data. Exercise_2E_Start.CATPart Analyze the Section Curve of a car’s bumper for its geometrical discontinuities. Perform Connect Checker analysis to understand the discontinuities on the curve. Perform the Porcupine analysis to check the inflection points and curvature continuities. Smoothen the curve using the Curve Smooth tool.
Analyze the Airfoil curve for its connections and continuities using Curve Connect Checker. Perform connect checker analysis to understand the discontinuities. Smoothen the curve using the Curve Smooth tool.
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CATIA V5 Surface Design- Lesson 2: Wireframe Creation
Exercise 2E: Recap
Student Notes:
Check continuity of the curve using Connect checker.
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Perform the Porcupine analysis on a curve to check its curvature continuity.
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CATIA V5 Surface Design- Lesson 2: Wireframe Creation
Case Study: Wireframe Creation
Student Notes:
Recap Exercise 30 min
In this exercise you will practice with the Wireframe creation tools. Create a quick model of the car considering the overall dimensions of the car. Create feature lines on the model to understand the shape and visual characteristics of the car.
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Using the techniques you have learnt in this lesson and previous exercises, create the model without detailed instruction.
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CATIA V5 Surface Design- Lesson 2: Wireframe Creation Student Notes:
Do It Yourself: Wireframe Creation (1/7) 1.
Open the given part consisting of reference elements to build a wireframe of the model of a Toy Car. a) Browse through the files and open the model Case_Study_Start.CATPart
1
Reference Points
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Reference Planes
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Reference lines (Boxes)
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CATIA V5 Surface Design- Lesson 2: Wireframe Creation Student Notes:
Do It Yourself: Wireframe Creation (2/7) 2.
Create a front and back wheel curve. a. Create a Circle at the point shown with a plane support of radius 60mm b. Create a part Circle with the same inputs from 0 deg to 155 deg. and Radius = 70mm. a. Create a Line from the center of the circle, length 375mm along Y axis. b. Create a Circle at the end point of the line as a center of radius 60mm (with initial plane support) c. Create a part Circle with the end point of Line as center with start angle 75 deg and End angle 180 deg. Radius = 70 mm (with initial plane support)
2a
2b
2c
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2d
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CATIA V5 Surface Design- Lesson 2: Wireframe Creation Student Notes:
Do It Yourself: Wireframe Creation (3/7) 3.
4.
Create a Corner between elements. a. Create a corner between the first part circle and line as shown. Specify the radius 20mm b. Create a corner between the second part circle and line as shown. Specify the radius 20mm Create a Connect Curve between first part circle and point on reference curve. a. Specify the tension at both the ends (if required) to achieve desired shape. b. Specify curvature continuity option.
3a
3b
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4a
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CATIA V5 Surface Design- Lesson 2: Wireframe Creation Student Notes:
Do It Yourself: Wireframe Creation (4/7) 5.
Create a Connect Curve between Second part circle and point on reference curve. a. Specify the tension at both the ends (if required) to achieve the desired shape. b. Specify the curvature continuity option.
6.
Create a Point on the line as shown. a. Create a point at a distance ratio of 0.3.
7.
Create a Spline to form a Bonnet feature line. a. Create a Spline passing through the points shown in the image. b. Specify the tangent direction and modify the tension values to attain the desired shape.
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7
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5
6
Point
Point 2
Point 3
Point 1
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CATIA V5 Surface Design- Lesson 2: Wireframe Creation Student Notes:
Do It Yourself: Wireframe Creation (5/7) 8.
Create a body shell. 8a a. Create a Point on Spline created in previous operation at a distance ratio of 0.4. b. Create a Plane passing through three points as shown. c. Create a sketch of a three-point arc passing through these three points.
8c
8b
Point 2
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Point 1
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Point 3
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CATIA V5 Surface Design- Lesson 2: Wireframe Creation Student Notes:
Do It Yourself: Wireframe Creation (6/7)
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9. Create a window and wind shield features. a. Create a Point on the Spline created in the previous step at a distance ratio of 0.3. b. Create a Point on the Spline created in the previous point at a distance ratio of 0.7. c. Create a Point on the Spline created in the previous point at a distance ratio of 0.9. d. Create a line between two points as shown. e. Create a Plane parallel to XY plane at the end point of the line previously created. f. Create a sketch on the plane created in the previous step as shown. g. Create a part circle joining the end point of the sketched curve and mid-point of the reference curve. Specify radius 100mm.
9b
9a
9c 9d
9f
9g
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9e
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CATIA V5 Surface Design- Lesson 2: Wireframe Creation Student Notes:
Do It Yourself: Wireframe Creation (7/7) 9. Create a window and wind shield features (continued…). h. Create the lines up to YZ planes from a specified point. i. Create a 3D Corner at left corner of front wind shield. Specify radius of 20mm. j. Similarly, create a 3D corner at top-left corner of the front wind shield. Specify radius 20mm. k. Similarly, create a 3D corner at both the corners of the back wind shield. Specify radius 20mm.
9h
9j 9i
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9k
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CATIA V5 Surface Design- Lesson 2: Wireframe Creation
Case Study: Wireframe Creation Recap
Student Notes:
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Create a quick model of the car considering the overall dimensions of the car. Create feature lines on the model to understand the shape and visual characteristics of the car.
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