Functional Molded Parts
CATIA V5 Training Exercises
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Functional Molded Parts
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Version 5 Release 19 September 2008 EDU_CAT_EN_FMP_FX_V5R19
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Functional Molded Parts Student Notes:
Table of Contents (1/2) Recap Exercise - Color Pallet Do It Yourself
Recap Exercise - Front Cover Do It Yourself
Recap Exercise - Bottle Do It Yourself
Master Exercise: Locking Cover Locking Cover Presentation Locking Cover Step 1: Create Basic Features Locking Cover Step 2: Create the Functional Features Locking Cover Step 3: Create the Dress Up Features Locking Cover Step 4: Add the Clips Locking cover Step 5: Create a Locating
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Added Exercises Belt Housing Electrical Box Housing Notepad Mold Extraction of Electrical Box Housing
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4 5
8 9
17 18
22 23 27 29 33 35 38
40 41 53 70 83
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Table of Contents (2/2)
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Mold Design of Electrical Box Housing
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108
Functional Molded Parts
Color Pallet Recap Exercise 15 min
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In this exercise you will : Create the ‘Color Pallet’ using ‘Basic Features’
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Student Notes:
Functional Molded Parts
Do It Yourself (1/3) Part used: Color_Pallet_Start.CATPart Create a Shellable Feature using the sketch ‘BasicShape’. Use the parameters as shown in the panel. Create the Shellabe Pad in the downward direction. (negative Z direction) To fillet the floor edge, go to the ‘Fillet’ tab and enter ‘First Radius = 5.0mm’
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Open ‘Shell Properties.1’ and select the ‘face to remove’. Also enter ‘Thickness = 1mm’
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Student Notes:
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Do It Yourself (2/3) Similarly create pockets using the ‘Pallets’ sketch. Use Shellable Feature to create the pockets.
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Enter 3mm as value to fillet the floor edges of the pocket.
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Do It Yourself (3/3) Create the outer flange of 2mm thickness using the ‘External Feature’ and the ‘Added_Boundry’ sketch.
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Create a cutout using ‘Protected Feature’. Use the ‘Hole_Cut’ sketch for the ‘Protected Feature’
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Functional Molded Parts
Front Cover Recap Exercise 20 min
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In this exercise you will create ‘Front Cover’ of a PC Speaker. You will use Basic Features and Functional Features to create the Front Cover.
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Student Notes:
Functional Molded Parts
Do It Yourself (1/8) Part used: Front_Cover_FMP_Start.CATPart
Create a ‘Shellable Feature’ using the pink ‘Main_Shape’ sketch. Keep the direction as that of the arrow and enter ‘First Length = 70 mm’.
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For ‘Shell Properties’, enter the ‘Thickness’ = 1.0 mm and remove the face as shown.
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Functional Molded Parts
Do It Yourself (2/8) Using the Remove Feature, cut the ‘Shellable Feature’ that you have created in the previous step. Unhide ‘Removed_Loft’ body.
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Use the ‘Removed_Loft’ body to cut the ‘Shellable Feature’ as shown below.
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Do It Yourself (3/8)
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Create circular holders for the speakers using the green colored “Speaker_Rest1” and “Speaker_Rest2”. Use the ‘Thick’ option of ‘Internal Feature’.
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Student Notes:
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Do It Yourself (4/8) Create the ‘Grill’ using the ‘Grill_Sketch_1’ Unhide the ‘Grill_Sketch_1’ and select the parameters for ‘Grill Feature’ as shown in the figure.
As all the curves required for various profiles for ‘Grill’ feature are defined in a single sketch, you will have to use contextual menu ‘Go to profile definition’ to select the profile curves for various parameters of the ‘Grill’ feature.
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For the ‘Boundary’ profile, select the outermost circular curve and enter the values for the parameters as shown in the figure.
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For the ‘Ribs’ profile, select all the circular curves except the one selected for ‘Boundary’. Also enter the values for the parameters as shown in the figure.
Functional Molded Parts Student Notes:
Do It Yourself (5/8)
For the ‘Spike’, select the lines and enter the values of parameters as shown.
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Before clicking ‘OK’ to the Grill panel, just check the direction of the ‘Grill’ feature and make sure that the it points downwards towards the face of the part. To change the direction, just click the arrow in the geometry area.
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Do It Yourself (6/8) Similarly create a grill for the smaller speaker using ‘Grill_Sketch_2’
Create added material for the screw holes using ‘Internal Feature’ as shown.
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Use the blue colored sketch – ‘Speaker_Screws’ for Internal Feature.
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Student Notes:
Functional Molded Parts
Do It Yourself (7/8) Similarly create added material for the back plate screws holes using ‘Internal Feature’ as shown. Use the magenta colored sketch – ‘Back_Cover_Screws’ for Internal Feature.
Create slots for volume buttons using the ‘Cutout’ feature.
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Use the brown colored sketch – ‘Volume_Button_Slots’ for the Cutout Feature
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Student Notes:
Functional Molded Parts
Do It Yourself (8/8) Create holes of diameter 5mm for the volume buttons on the floor of the slot as shown.
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To make the hole exactly concentric, select the circular edge first, click the ‘Hole’ tool and then select the floor face.
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Functional Molded Parts
Bottle Recap Exercise 20 min
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In this exercise you will create ‘Bottle’, using Basic Features and Feature Modifiers.
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Student Notes:
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Do It Yourself (1/4) Part used: FM_Bottle_Start.CATPart Open the CATPart and view the features and geometry that is already created for you. You will see a pink surface. This surface will form the bottom of the bottle. Unhide the ‘Solid Functional Set.1’. You will see a ‘Shellable revolve’.
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You can apply transparency to the ‘PartBody’ to visualize the inner surface.
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Do It Yourself (2/4)
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Form the bottom of the bottle by cutting the ‘Shellable Revolve’ using the pink colored surface.
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Student Notes:
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Do It Yourself (3/4) Using the ‘Remove Sketch’ and ‘Remove Feature’, alter the shape of the bottle as shown.
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Select the parameters as shown.
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Student Notes:
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Do It Yourself (4/4) Fillet the marked edges using the ‘Functional Fillet’. (Radius = 7mm)
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To increase the size of the bottle, use the Offset Feature and offset the whole bottle by 4mm.
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Functional Molded Parts
Master Exercise: Locking Cover In this Master Exercise, you will design the 'Locking Cover' using appropriate features of FMP Workbench.
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Locking Cover Presentation Locking Cover Step 1: Create Basic Features Locking Cover Step 2: Create the Functional Features Locking Cover Step 3: Create the Dress Up Features Locking Cover Step 4: Add the Clips Locking cover Step 5: Create a Locating
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Functional Molded Parts
Locking Cover Master Exercise Presentation 45 min
In this exercise you will see how to create a molded part using both Functional Molded Part and Part Design workbenches:
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Creating sketches and reference elements (planes) Creating Basic Features (shellable features, External features) Creating functional features Creating dress up features ( fillet, draft) Creating a Boolean operation ( trim)
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Student Notes:
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Design Intent
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Creation of a wireframe geometry using sketcher and planes Creation of a Shellable Feature and an External Feature Functional Features (Rib, Reinforcement) Dress-Up features (Fillets) Modification of the geometry by changing parameters of the surface definition.
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Student Notes:
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Design Process: Locking cover
1 Create the wireframe geometry (Done in this exercise)
Enter the Functional Molded Part workbench
4
2 Add the dress up features
Create internal feature across removed face of the shell
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5
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6 Add a locating
3
Create the Basic Features Create the functional features
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Part Definition
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Student Notes:
Functional Molded Parts
Locking Cover Step 1: Create Basic Features 5 min.
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In this step you will: Create a ‘Shellable Feature’ Create an ‘External Feature’
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Student Notes:
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Do It Yourself Load: locking_cover_start.CATPart 1
Main shape sketch
Shellable Feature
Height = 18mm Draft angle = 5deg Lateral radius = 8mm First radius = 4mm
2
Shell Properties
Thickness = 1mm Faces to remove = bottom planar face
3
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External Feature
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Extension plane sketch Height = 1,5mm Draft angle = 2deg Lateral radius = 5mm First radius = 1mm
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Locking Cover Step 2: Create the Functional Features. 20 min.
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In this step you will create the necessary functional features like: - Protected Features - Reinforcement - Rib
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Student Notes:
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Do It Yourself (1/3) Load: locking_cover_step_2.CATPart
1
Protected Feature
Rectangle hole sketch
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First Length = 22mm Second length = 5mm Draft angle = 3deg Lateral radius = 3mm
1) Create the Protected Feature 2) Hide the resulting red volume
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Do It Yourself (2/3) 1) Create the Rib.
1 Draft Angle = 1 Deg Height = 20mm
2) Create a second protected area.
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2
Draft Angle = 3 Deg Height = 6mm (cut the ribs)
3) Hide the resulting red volume.
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Functional Molded Parts Student Notes:
Do It Yourself (3/3) 1
Reinforcement
- Why the reinforcement is not trimmed after the parting plan ? - What is the difference between the With and Wall thickness values ?
Reinforcement sketch Reverse Direction Ceiling length = 0mm Opening length = -22mm Width = 1,5mm Wall thickness = 1,5mm Direction = Z axis Draft angle = 1 deg Ceiling radius = 0,5mm
2
Core Feature
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Removed sketch First Length = 52mm Second length = 17mm - What is the impact of a Core Feature on a External Feature ?
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Locking Cover
Student Notes:
Step 3: Create the dress up features. 5 min
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In this simple step you will create the fillets as shown here.
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R = 0.5mm
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Do it Yourself Create the fillets of the specified radius as shown below.
Load: locking_cover_step_3.CATPart
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R = 0.5mm
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Student Notes:
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Locking Cover Step 4: Add the clips. 5 min.
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In this step you will create the “clips”.
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Student Notes:
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Do It Yourself (1/2) Load: locking_cover_step_4.CATPart
1) Create a new part body (menu Insert + Body) and rename it “Clips” 2) Create an Added Feature with the following parameters. 1
Shape definition: Prism Profile: Clip 1 Sketch First Length: 2.5 mm Second Length: 0 mm Mirrored extent
3) Create a Draft with the parameters shown in the dialog box.
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2 faces to Draft + back face + second lateral face
4) Create a Mirror with the following parameters. Features to mirror: Draft.1 and Draft.2 Mirroring element: YZ plane
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Faces to Draft 3
New part body
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Do It Yourself (2/2) 1) Create another Added Feature for the Clips using the following parameters Shape definition: Prism Profile: Clip 2 Sketch First Length: 2.5 mm
2
Second Length: 0 mm Mirrored extent
2 faces to Draft + back face + second lateral face
2) Create a Draft Added Feature
3) Create a Mirror with the following parameters.
Shape definition: External Shape External Shape: Clips Trim to shell
Features to mirror: Draft.2
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Mirroring element: YZ plane
4) Activate the Main PartBody 5) Create an Added Feature
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Locking Cover Step 5: Create a locating (Design change). 5 min.
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In this step you will remove an area from a protected prism to create a locating.
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Student Notes:
Functional Molded Parts
Do It Yourself Load: locking_cover_step_5.CATPart
Use ‘Remove’ feature to cut the Protected Prism.6. (last protected feature in the spec. tree). Use the following parameters for the ‘Remove’ feature.
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Locating sketch First length = 20,5mm Second length = To Plane XY Features to modify = Protected Prism.6 Profile = Locating sketch Draft = -1deg
After modification, hide the modified protected volume (displayed in red).
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Student Notes:
Functional Molded Parts
Added Exercises In these added exercises, you will practice designing some more molded parts using FMP workbench. You will also practice "Extraction of Core and Cavity" of a molded part.
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Belt Housing Electrical Box Housing Notepad Mold Extraction of Electrical Box Housing Mold Design of Electrical Box Housing
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Student Notes:
Functional Molded Parts
Belt Housing You will design the 'Belt Housing' using appropriate features of FMP Workbench.
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Belt Housing Presentation Belt housing Step 1: Create Basic Features Belt Housing Step 2: Create Functional Features Belt housing Step 3: Create Fillets
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Functional Molded Parts
Belt Housing Exercise Presentation.
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30 min.
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Student Notes:
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Design Intent The Electrical Box Housing is a molded part with holes and ribs. It also has holes for external fastening. The intention here is to select proper Functional Features and Feature Modifiers to create the shape.
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Holes
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Holes for External Fastening
Ribs
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Belt Housing Step 1 : Create the Basic Features 5 min.
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In this step you will create several Shellable Features.
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Student Notes:
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Do It Yourself 1 2
3
Locating sketch Height = 5mm Draft angle = 2deg Lateral radius = 2mm First radius = 2mm
Body sketch
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Height = 20mm Draft angle = 2deg Lateral radius = 20mm First radius = 5mm
Side prism sketch Height = 14mm Draft angle = 2deg First radius = 3mm
1) Create the small locating. 2) Create the main body. 3) Create the side prism. 4) Apply the shell properties 1mm with the bottom face removed.
4
Part used: belt_housing_start.CATPart
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Functional Molded Parts
Belt Housing Step 2 : Create the Functional Features 35 min
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In this step you will create features like: Protected features Boss Rib Cutout
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Student Notes:
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Do It Yourself (1/4) 1
First length = 26mm Second length = -8mm Draft angle = 2deg Neutral = Profile Plane Thick option Thickness1= 1mm
2
Boss sketch Internal prism sketch 3
First length = 26mm Second length = -8mm Draft angle = 2deg Neutral = Profile Plane Thick option Thickness1= 1mm
Cavity sketch
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Height = 2mm Draft angle = 2deg First radius = 1mm
1) Create the internal feature. 2) Create the External feature. 3) Create the other internal feature. Load: belt_housing_step2.CATPart
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Do It Yourself (2/4) 1
2 Height = 20mm Draft angle = 1deg Rib sketch 2 sketches for sweep cutout Keep angle mode Lateral radius = 2mm
3
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Boss sketch
1) Create the sweep cutout. 2) Create the boss. 3) Create the rib.
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Ceiling length = 25mm Draft angle = 2 deg Ceiling radius = 2mm
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Do It Yourself (3/4) 1 2
Inside protected area sketch
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Height = 5mm Draft angle = 1deg
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1) Create the protected feature. Hide the resulting volume in red 2) Create the top cutout.
Top cutout sketch Floor length = 18mm Opening length = -45mm Check option With floor Draft angle = 2deg Neutral element = Floor Lateral radius = 7mm Floor radius = 4mm
Functional Molded Parts Student Notes:
Do It Yourself (4/4) 1
2
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4 circles diameter = 4mm Position the circles using the yellow sketch (Cavity sketch) Do not use the solid to position the circle, it is better to keep the features independency (parallel design)
1) Create a new sketch with 4 circles. 2) Create the protected feature using this sketch.
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First length = 5mm. second length = 7mm. Draft angle = 3deg
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Belt Housing Step 3: Create the Fillets 15 min
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In this step you will create the edge fillets.
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Student Notes:
Functional Molded Parts
Do It Yourself
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Add the fillets trying to keep the thickness constant.
Tips: First fillet the edges which will have the smaller radius (concave) edges then fillet the edges which will have the larger radius (convex). Select multiple edges for the fillet to increase the robustness in case of changes. Load: belt_housing_step3.CATPart
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Electrical Box Housing You will design the 'Electrical Box Housing' using appropriate features of FMP Workbench.
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Electrical Box Housing Presentation Electrical Box Housing Step 1: Create Basic Features Electrical box housing Step 2:Create Functional Features Electrical Box Housing Step 3 : Design Changes
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Student Notes:
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Electrical Box Housing Master Exercise Presentation 45 min
In this exercise you will design the Electrical Box Housing In the Exercise you will:
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Create the basic shape using Shellable Feature Use Functional Features to create ‘Cutout’ ‘Pockets’ etc. Do some Design changes to complete the design.
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Student Notes:
Functional Molded Parts Student Notes:
Design Intent The Electrical Box Housing is basically a ‘Y’ shaped housing with some Pockets and Cutouts for special purposes. The intention here is to create the shape and alter the shape using proper Functional Features. Basic Y Shape
Cutout
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Filleted Pocket
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Electrical Box Housing Step 1 – Creating the basic shape 30 min
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In this step you will create the Main Shape of the Box: In the step you will Create Basic Features Assign Draft and Shell Properties for the Part
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Student Notes:
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Do It Yourself (1/5) CATIA Data used: electrical_box_housing_Step_1.CATPart Define the Draft Properties of the Part Click the ‘Draft Properties’ tool and define the following ‘Draft Properties’ for the Part Draft Angle = 3deg Pulling Direction = XY Plane
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Default Draft
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Draft angle = 3deg Pulling Dir = XY Plane Parting = no selection
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Do It Yourself (2/5) Create the main shape of the Part. Use the ‘Shellable Feature’ to create the main Shape of the Part with the parameters as shown near the figure.
Main shape sketch Height = 40mm Draft angle = Default properties
Create the outer ‘Opening Shape’ of the part Use the ‘Shellable Feature’ to create the outer ‘Opening Shape’ of the part with the parameters specified below.
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Height = 43mm Draft angle = Default properties
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Openings sketch
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Do It Yourself (3/5) Define the ‘Shell’ Properties as shown below and remove the lower face as shown in the figure.
Shell Properties Thickness = 1.5mm Remove the lower face Bottom Face Removed
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Create the openings using the ‘Core’ Feature with the following parameters.
Height = 45mm Intrinsic Draft angle = 5deg (reversed direction) Parting for openings sketch
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Functional Molded Parts Student Notes:
Do It Yourself (4/5)
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Change the Functional Behavior of the ‘Core’ feature that you have created in the last step. Use the contextual menu to change the behavior from ‘Core’ to ‘Protected’ Hide the Red Volumes.
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The End Result will not change.
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Do It Yourself (5/5) Create an external Flange using the Flange Sketch as shown.
Flange sketch Height = 3mm Draft angle = Draft Properties.1
Fillet the following edges with the radii as shown in the picture below.
R = 12mm, 6 edges
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R = 2mm, 3 edges
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Functional Molded Parts
Electrical Box Housing Step 2 – Creating Functional Features 30 min
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In this step you will modify the Shape of the housing using Functional Features like Protected Features Cutout Boss Rib
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Student Notes:
Functional Molded Parts Student Notes:
Do It Yourself (1/4) CATIA Data used: electrical_box_housing_step_2.CATPart Create a Cutout Feature. Use the ‘Cutout’ sketch to create the Cutout Feature as shown in the picture below. For the Cutout features use the parameters as shown below.
Cutout sketch
Floor length = 20mm Opening length= -70mm With floor Draft angle = Draft Properties.1 Neutral element = Floor Lateral radius = 10mm Floor radius = 5mm
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Create an additional Shellable Feature and create the new Shellable shape as shown below.
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First length = 49mm Draft angle = Draft Properties.1 First radius =5mm Lateral radius =10mm Boss sketch
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Do It Yourself (2/4) Add a Flange to the shellable shape created in the previous step.
First length = 3.0mm Draft angle = Draft Properties.1 Lateral Radius = 13mm Flange for Boss Sketch
Create the Protected Opening as shown in the picture below. Use ‘Protected Feature’ sketch to create the Protected Opening. Select the pulling direction as shown in the picture below.
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First length = 60mm Second length = -25mm Draft angle = Draft Properties.1 Neutral = Second limit
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Protected feature sketch Draft Direction
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Do It Yourself (3/4) Create the Ribs using the Rib Sketch with the parameters specified below.
Rib sketch First limit = 52mm Second limit = -13mm Draft angle = 1deg Neutral = Second Limit
Create a second ‘Protected Shape’ to cut some of the Ribs as shown.
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Protected feature 2 sketch
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First length = 35mm Second limit = 0mm Draft angle = Draft Properties.1 Neutral = first limit
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Do It Yourself (4/4) Add the fillets keeping the thickness constant.
R = 2.5mm
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R = 1mm
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R = 1mm
R = 2.5mm
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Electrical Box Housing Step 3 – Doing the Design Changes 30 min
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In this step you will do some modifications in the design of the Housing You will: Modify a Sketch of a feature. Fillet an edge formed due to modification of the Sketch.
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Student Notes:
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Do It Yourself (1/2) CATIA Data used: electrical_box_housing_step_3.CATPart
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Unhide the ‘Boss’ Sketch, edit it and change the value of the dimension as shown in the picture below.
Boss Sketch
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Dimension Angle.197 = 30deg
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Do It Yourself (2/2)
Fillet the edges as shown.
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Edge fillet
Change the default Draft angle.
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Draft Properties.1 Draft angle = 4deg
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Notepad You will design the Notepad using the FMP workbench.
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Design Intent Do it Yourself
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Student Notes:
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Design Intent Notepad
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30 min
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Student Notes:
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Do It Yourself (1/11) CATIA Data Used: notepad_start.CATPart
1
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1) Create the default Draft properties.
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Default Draft Draft angle = 1deg Pulling Dir = XY Plane Parting = XY Plane
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Do It Yourself (2/11)
1
Sketch.1
2
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Sketch.1 First Limit: Up to plane XY Second Limit: 0mm Direction = Z axis Draft = Properties.1 Lateral and second limit Fillet = 5mm
1) Create the main shellable prism. 2) Define the Shell properties.
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Shell Properties Thickness = 2mm Faces to remove = bottom face (face coincident to the XY plane)
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Do It Yourself (3/11)
1a 1 Hook fastening sketch
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First Limit = 60mm Second Limit = 0mm Direction = X axis Draft = Properties.1 Neutral = Use Parting element Selected by Pulling direction
1) Create the protected feature. How many faces are actually drafted by the draft properties.1 ? 1a) Optional: Change the behavior to Added, check the faces drafted, then change it back to the protected behavior. 2) Translate the protected feature using a Pattern.
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2
Pattern of Protected Ref Element = YZ plan First direction tab Instances=2 Spacing = 100mm
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Do It Yourself (4/11)
1 Main Holes sketch
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First Limit = 5mm Second Limit = 0mm Reverse Direction With floor Draft =10deg Wall Enter thickness = 1.5mm With Constant Wall thickness
1) Create a cutout. 2) Create a second cutout.
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2
Additional Holes sketch Same parameters than previous cutout
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Do It Yourself (5/11)
1 Pattern Feature = Cutout.1 Ref element = Plane.2 Spacing = 80mm Spacing = 30mm
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2
1) Create a rectangular pattern. 2) Create a translation using a rectangular pattern.
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Rectangular (linear) Pattern Feature = Cutout.2 Ref element = Plane.2 Spacing = 30mm
Functional Molded Parts Student Notes:
Do It Yourself (6/11)
3
1 Ribs sketch
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First length = Up to XY Plane Direction = Z axis Draft = 1deg Thickness = 1.5mm
2 Add Posts Diameter = 5mm Taper Angle = 1deg Reference = First limit
1) Create the Ribs. 2) Edit the Ribs sketch, switch from Construction to Standard mode then add points at each intersection of the lines for post. 3) Activate the posts in the Rib feature.
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Functional Molded Parts Student Notes:
Do It Yourself (7/11)
1
Cylinder body
2
Tool body = Cylinder Clearance distance = 0mm
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Push.1 surfaces Radius = 2mm
1) Use the Push feature with the orange cylinder as Tool body. 2) Create the edge fillet as shown.
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Do It Yourself (8/11)
1 Alternative for Locating Tool body = Alternative Pad for Locating Clearance = 0mm
2
Core extension
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Do it yourself
1) Use the Pull feature with the body “Alternative pad for locating” to extend the shell. 2) Extend the Core to remove the unwanted cavity extension resulting of the Pull (Create a sketch-based feature to open the parting plane).
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Functional Molded Parts Student Notes:
Do It Yourself (9/11)
1 Style surface
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Features to cut = Shellable Prism.1 Cutting element = Style surface (located in Geometrical Set.1) Reverse the direction of the cut
1) 2)
Cut the Main shell using a styling surface. Edit the feature in error and select the missing edge.
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Functional Molded Parts
Do It Yourself (10/11)
Fillet Radius = 1mm
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1) Create a ‘Face-to-face’ fillet.
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Functional Molded Parts
Do It Yourself (11/11)
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Compare your design with the end file below.
Load: notepad_end.CATPart
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Functional Molded Parts
Mold Extraction of Electrical Box Housing You will learn how to Extract the Core and Cavity of a molded part designed using FMP workbench.
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Mold Extraction Presentation Step 1: Extraction of Core and Cavity Bodies of a Mold Step 2: Detailed definition of Core and Cavity Bodies Step 3: Fillets creation and design change Step 4: Shrinkage of the Core and Cavity
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Functional Molded Parts
Functional Mold Extraction - Presentation Master Exercise Presentation 25 min.
In this exercise, you will see how to extract the functional core and cavity parts of a molded part, using Functional Molded Part workbench (P2 only) and more specially the Functional Extraction toolbar
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You will perform the following tasks: Basic extract of the Core and Cavity Bodies Refined definition of Core and Cavity Bodies Update of the Core and Cavity Bodies after a design change
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Student Notes:
Functional Molded Parts Student Notes:
Design Process 1
Enter the Functional Molded Part workbench
Extract basic Core and Cavity Bodies
3
Refine Core and Cavity Bodies definition
4 Create an additional insert
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5
Reroute fillets from the main PartBody to the Cavity Bodies (copy dress-up feature from the Part to the Cavity/Core extraction)
6
7 Perform a design change
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Shrink Core, Cavity Bodies and additional Insert
2
Create Added Features to materialize the Mold Plates
Functional Molded Parts
Functional Mold Extraction Step 1 - Extraction of Core and Cavity Bodies of a mold 30 min
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In this step you will: Extract the Core Body. Extract the Cavity Body. Create 2 Added Features to materialize the Core and Cavity Plates.
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Student Notes:
Functional Molded Parts
Do It Yourself (1/3) 1
Core Extraction
Source Body PartBody Extract behavior = None Excluded features = None
1) 2)
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3)
Core Extraction. Rename the created Body.2 as Core Body. Set the Graphic Properties of the Core Body to a yellow color.
Load: electrical_box_housing_for_mold_extraction_START.CATPart
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Functional Molded Parts
Do It Yourself (2/3) 2
Cavity Extraction
Source Body PartBody Extract behavior = None Excluded features = None
1) 2) 3)
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4)
Hide the Core Body Cavity Extraction Rename the created Body.3 as Cavity Body Set the Graphic Properties of the Cavity Body to a blue color
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Functional Molded Parts Student Notes:
Do It Yourself (3/3) Added Feature
2
1) 2)
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3)
4) 5) 6)
3
Shape definition: Prism Profile: Sketch from step 2 First Length: 60 mm Second Length: 0 mm 4
Insert a Geometrical Set. Rename it as “Insert Plate” Create a rectangular sketch on XY plane that includes the Cavity shape (dimensions as shown on the picture) Activate (define in work object) the Cavity Body and create an Added Feature using the rectangular sketch which you have recently created . Hide the Protected Feature created in Functional Body.3 Hide the main PartBody Hide the Cavity Body Show and activate the Core Body and create the same Added Feature in Reverse Direction using the same rectangular sketch. Some inconsistency after the automatic extraction will be fixed next step.
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Functional Molded Parts
Functional Mold Extraction Step 2 - Detailed definition of Core and Cavity Bodies 10 min
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In this step you will: Use Extract Properties to improve the Core and Cavity Extraction Exclude a feature from the Cavity Extraction (manage the manufacturability of the core) Create an additional Insert Remove the additional Insert shape from the Cavity Body Exclude the rib features from the Core Body
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Functional Molded Parts
Do It Yourself (1/7) 3
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1) 2) 3)
Hide the Core Body Activate and Show the Main PartBody Properties Extraction: Switch Clash Protection.7 from Cavity to Core 4) Hide the Main PartBody What is the purpose of the Extraction Properties feature ?
Load: electrical_box_housing_for_mold_extraction_STEP2.CATPart
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Student Notes:
Functional Molded Parts
Do It Yourself (2/7) 2
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1) 2)
Show the Core Body In Functional Body.2, edit the Added Extracted Core.1 feature and apply Extraction Properties.1 as Extract behavior (select in the combo box)
Result: the Core Body is now a closed volume 3)
Hide the Core Body
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Student Notes:
Functional Molded Parts
Do It Yourself (3/7) 2
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1) 2)
Show the Cavity Body In Functional Body.3, edit the Protected Extracted Cavity.2 feature and apply Extraction Properties.1 as Extract behavior
Result: the Cavity Body is now made of a single volume
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Functional Molded Parts
Do It Yourself (4/7)
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1
1)
In Functional Body.3, edit the Protected Extracted Cavity.2 feature Select, in Functional Body.1, Wire opening.6 as Excluded feature
2)
Hide the Cavity Body
Remark: The Wire opening shape will be obtained from an additional insert Question: How to create this additional insert?
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Student Notes:
Functional Molded Parts Student Notes:
Do It Yourself (5/7) 3
1
4
1)
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2) 3) 4) 5) 6)
Create a Volumes Extraction - Protected volume extraction - Extract from: Features - Selection: Wire opening.6 Rename the new created Body as “Local Insert” Create a rectangular sketch on the lower face of the ‘Added Behavior Extraction’ that includes its geometry Create an Added Feature Show the Cavity Body Hide the Local Insert Body
Question: How to remove this additional insert from the Cavity Body?
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Added Feature Shape definition: Prism Profile: Sketch from step 3 First Length: 10 mm Second Length: 0 mm
Functional Molded Parts
Do It Yourself (6/7) 1
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1) 2)
3) 4)
Activate the Cavity Body Create a Behavior Extraction Feature to extract: Wire opening.6 Change functional behavior: Protected In Functional Body.3, hide the Protected Behavior Extraction.1 that was just created Hide the Cavity Body
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Student Notes:
Functional Molded Parts
Do It Yourself (7/7) 1
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1) 2)
3)
Show the Main PartBody In Functional Body.2, edit Added Extracted Core.1 Click on Excluded features selection icon and select the ribs (Rib.1) from the Main PartBody Hide the Main PartBody and show the Core Body
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Functional Molded Parts
Functional Mold Extraction Step 3 - Fillets Creation and Design Change 5 min
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In this step you will: Copy the fillets from Main PartBody to Cavity Bodies Make a design change on the Part definition
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Functional Molded Parts
Do It Yourself (1/3) Load: electrical_box_housing_for_mold_extraction_STEP3.CATPart
3
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1) 2) 3)
Hide the Core Body Show the main PartBody Menu Insert / Knowledge Templates / Power Copy … Name: Cavity Fillets Select EdgeFillet.1 and EdgeFillet.2 from the main Part Body Click OK on the warning message that appears to create the Power Copy
Note: Powercopy is a way to ensure that all the dress-up features will be transferred from the PartBody to the Cavity Body. Alternatively, you can copy-paste the fillet one by one. (Generally, no reroute is necessary as the extracted solid are associative to the PartBody)
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Student Notes:
Functional Molded Parts
Do It Yourself (2/3)
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3
1) 2) 3) 4)
Hide the Main PartBody Activate and show the Cavity Body Contextual menu on Cavity Fillets object / Instantiate Reroute the 5 Edges Hide the Cavity Body
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Student Notes:
Functional Molded Parts
Do It Yourself (3/3)
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2
1) Activate and show the Main PartBody. 2) Edit the Sketch “Main shape sketch” from Functional Body.1 Modify value of Radius.44 from 60mm to 80 mm. 4) Exit the sketcher and update the part. 5) Delete EdgeFillet.1. 6) Edit the other two EdgeFillets which are in error and click OK to their definition dialog box. 7) Show Core and Cavity Bodies to check the result of the modification.
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Functional Molded Parts
Functional Mold Extraction Step 4 - Shrinkage of the Core and Cavity 5 min
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In this step you will: Apply shrinkage to the Cavity, Core and to Additional Insert Bodies Generate the Molded Part from the Cavity, Core and Additional Insert Bodies in order to check that the Mold process is correct
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Functional Molded Parts
Do It Yourself (1/5) Load: electrical_box_housing_for_mold_extraction_STEP4.CATPart
1
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1)
2) 3)
Create a f(x) parameter Type = Real Name = Shrinkage Value = 1.05 Activate skeleton Geometrical set. Create a point (0mm,0mm,0mm). Rename it Scaling point. Hide PartBody and Cavity Body. Activate and show Core Body
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Student Notes:
Functional Molded Parts
Do It Yourself (2/5) 1
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1)
Create a Transform feature Type = Scaling Reference = Scaling Point Ratio = Shrinkage parameter Features to transform = Added Extracted Core.1 in Functional Body.2
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Functional Molded Parts
Do It Yourself (3/5) 2
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1) 2)
3)
Hide Core Body. Activate and show Cavity Body Create a Transform feature Type = Scaling Reference = Scaling Point Ratio = Shrinkage parameter Features to transform = Protected Extracted Cavity.2 in Functional Body.3 Protected Behavior Extraction.1 in Functional Body.3 Hide the resulting red volume
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Functional Molded Parts
Do It Yourself (4/5) 2
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1) 2)
3)
Hide Cavity Body. Activate and show Local Insert Create a Transform feature Type = Scaling Reference = Scaling Point Ratio = Shrinkage parameter Features to transform = Added Extracted Protected.3 and Added Prism.10 in Functional Body.4 Hide Local Insert
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Student Notes:
Functional Molded Parts Student Notes:
Do It Yourself (5/5) 2
Added Feature
3
Shape definition: Prism Profile: Sketch .16 First Length: 60 mm Mirrored extent
1) 2) 3)
4)
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5)
6)
Insert a new Body and rename it as “Molded Part” Create an Added Feature, based on the sketch used to create the Core and Cavity plates (Sketch.16 used for Added Prism.9 in Functional Body.2) Create a Protected Feature Shape definition = External Shape Select Core Body Create a Protected Feature Shape definition = External Shape Select Cavity Body Create a Protected Feature Shape definition = External Shape Select Local Insert Hide the 3 red volumes
Remark: the obtained Body represents the Molded Part, which can be used to check that the Core, Cavity and Additional Insert were correctly defined.
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Functional Molded Parts
Mold Design of Electrical Box Housing You will design the 'Molding Tool' for the 'Electrical Box Housing'
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Mold design: Electrical Housing Design Process Do it Yourself
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Functional Molded Parts
Mold design: Electrical Housing Added Exercise 20 min
Prerequisite: Functional Mold Extraction Exercise (Electrical box housing) In this exercise you will see how to integrate the Core and Cavity Bodies (which are extracted using Functional Molded Part workbench) in a Mold.
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You will perform the following tasks: Create a Mold in Mold Tooling Design Workbench Insert the Molded Part Create the Core Insert, insert it in the Mold and drill the Core Plate Create the Cavity Insert, insert it in the Mold and drill the Cavity Plate
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+
Student Notes:
Functional Molded Parts Student Notes:
Design Process 1
Create the Mold and Insert the Molded Part
Enter the Mold Tooling Design workbench
2
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3
Create the Core Insert, Insert it in the Mold and Drill the Core Plate
Create the Cavity Insert, Insert it in the Mold and Drill the Cavity Plate
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Enter the Functional Molded Part workbench
Functional Molded Parts Student Notes:
Do It Yourself (1/7) Load: electrical_box_housing_for_mold_integration_START.CATPart
1) 2)
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3)
Create a new Product and enter the Mold Tooling Design workbench Create a new Mold with parameters as shown in the picture Contextual menu on MoldedPart / Components / Replace Component In Session Select electrical_box_housing_for_mold_integration _START.CATPart
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2
Functional Molded Parts
Do It Yourself (2/7) 1)
2)
3)
4)
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5)
Use the contextual menu on the Compass and select ‘Snap Automatically to Selected Object’ Select the “electrical box housing” CATPart and position it as shown on the pictures. Use Top View and Right View Use the contextual menu on the Compass and select Snap Automatically to Selected Object to unselect this option. Enter the Assembly Design workbench. Fix the “electrical box housing” CATPart Use the contextual menu on “electrical box housing” and select MoldedPart.1 object > Open In New Window.
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Student Notes:
Functional Molded Parts Student Notes:
Do It Yourself (3/7) 600 mm
6
5
Added Feature
200 mm
600 mm
Shape definition: Prism Profile: Sketch from step 5 First Length: 100 mm Second Length: 0 mm
250 mm
7 Added Feature
1) 2)
3)
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4) 5) 6) 7) 8)
Create a New Part and rename it Core Insert In electrical_box_housing_for_mold_integration_START.CATPart, copy the Core Body and paste it As Result With Link in the Core Insert CATPart In Core Insert CATPart, contextual menu on Core Body object / Change PartBody Rename the second Body “DrillHole” Activate the DrillHole Body and create a rectangular sketch based on the XY plane Create an Added Feature based on the created sketch Create an Added Feature based on the Core Body Set the Graphical Properties on the DrillHole Body as red and transparent (100)
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Shape definition: External Shape External Shape: Core Body
Functional Molded Parts
Do It Yourself (4/7) 1) 2) 3) 4) 5) 6) 7)
8) 9)
Using drag and drop, insert the Core Insert CATPart in the Ejection Side of the Mold Activate the Ejection Side sub-assembly Show the reference planes of both the Core Insert CATPart and “electrical box housing” CATPart Snap the reference planes of the Core Insert CATPart on the reference planes of the “electrical box housing” CATPart Hide the “electrical box housing” CATPart Enter the Mold Design Tooling Workbench Menu Tools / Drill Component Components to Drill: CorePlate Drilling Components: Core Insert With Drill Hole Hide the DrillHole Body on the Core Insert CATPart Hide the Injection Side sub-assembly
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Result: the Core Plate is ready 10) Show the Injection Side sub-assembly 11) Show the “electrical box housing” CATPart
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Student Notes:
Functional Molded Parts Student Notes:
Do It Yourself (5/7) 5
600 mm 6
200 mm
600 mm
250 mm
1) 2) 3)
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4) 5) 6)
Added Feature Shape definition: Prism Profile: Sketch from step 5 First Length: 100 mm Second Length: 0 mm Reverse Direction
Create a New Part and rename it Cavity Insert In electrical_box_housing_for_mold_integration_START.CATPart, copy the Cavity Body and paste it As Result With Link in the Cavity Insert CATPart In Cavity Insert CATPart, contextual menu on Cavity Body object / Change PartBody Rename the second Body “DrillHole” Activate the DrillHole Body and create a rectangular sketch based on the XY plane Create an Added Feature based on the created sketch
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Functional Molded Parts Student Notes:
Do It Yourself (6/7) 1
2 Added Feature Shape definition: Prism Profile: Sketch from step 2 First Length: 60 mm Second Length: 0 mm
1) 2)
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3)
Create a second rectangular sketch based on the XY plane (Cavity Plate projection) Create an Added Feature based on the created sketch Set the Graphical Properties on the DrillHole Body as red and transparent (100)
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Functional Molded Parts
Do It Yourself (7/7) 1) 2) 3) 4) 5) 6) 7)
8)
Using drag and drop, the Cavity Insert CATPart to insert in the Injection Side of the Mold Activate the Injection Side sub-assembly Hide the EjectionSide and EjectorSystem sub-assemblies Show the reference planes of both the Cavity Insert CATPart and “electrical box housing” CATPart Snap the reference planes of the Cavity Insert CATPart on the reference planes of the “electrical box housing” CATPart Hide the “electrical box housing” CATPart Menu Tools / Drill Component Components to Drill: CavityPlate Drilling Components: Cavity Insert With Drill Hole Hide the DrillHole Body on the Cavity Insert CATPart
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Result: the Cavity Plate is ready 9)
Show the Ejection Side
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Student Notes:
