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Generative Shape Design Detailed Steps

2021-10-11 21:17| 发布者: 鬼见愁| 查看: 527| 评论: 0

摘要: Table of ContentsWireframe Recapitulation Exercise 4Surface Recapitulation Exercise 8Operation Recapitulation Exercise 17Advanced Tasks Recapitulation Exercise 30B-Pillar 41Step 1: Publishing the Styl ...
Table of Contents
Wireframe Recapitulation Exercise 4
Surface Recapitulation Exercise 8
Operation Recapitulation Exercise 17
Advanced Tasks Recapitulation Exercise 30
B-Pillar 41
Step 1: Publishing the Styling Inputs and Creating the Mating Part 41
Step 2: Creating the Outer Part 50
Step 3: Creating the Inner Part 60
Step 4: Creating the Reinforcement Part 71
Step 5: Replacing the Input Styling Data and Managing the Update Failures 79
Mobile Phone 84
Step 1: Creating the Wireframe Geometry 84
Step 2: Creating the Surfaces 89
Step 3: Performing operations 97
Step 4: Analyzing and Modifying 104
Step 5: Completing the part in Part Design 111
Knob 115
Step 1: Creating the Wireframe Geometry 115
Step 2: Creating the Basic Surfaces 119
Step 3: Performing Operations the Basic Surfaces 121
Step 4: Analyzing and Modifying the draft angle 128
Step 5: Offsetting a solid 130
Bottle Exercise 134
Step 1: Bottle Bottom Creation 134
Step 2: Bottle Body Creation 159
Step 3: Bottleneck 180
Step 4: Assemble the three bodies 207
Step 5: Create the Bottleneck Screw 224
Space Mouse Base 237
Step 1: Create the Filleted pad. 237
Step 2: Create the surfacic elements. 244
Step 3: Sew the surface on the Pad. 251
Step 4: Create the Groove. 253
Step 5: Split the solid with an imported surface. 255
Step 6: Shell the created solid. 257
Step 7: Create the Shaft. 258
Step 8: Create the Holes and Pockets. 261
Step 9: Assemble a new body. 272
Lemon Squeezer 280
Step 1: Completing the wireframe elements 280
Step 2: Creating the basic surfaces 286
Step 3: Creating a blend surface with coupling and adding the handle 289
Step 4: Creating filtering holes 298

Surface Recapitulation Exercise
Load the part called surface_recap_begin.CATPart from the ''Companion'' and save the part in the Students directory.

1. First you are going to Offset 7 surfaces (1 mm.) from the inside of the Solid Clamp.

Double Click on the Offset icon.

In the Offset Surface Definition dialog box enter an Offset value of 1mm.

Select the first surface as shown.

Click on OK to confirm the Offset surface creation.

As you have double clicked on the icon, the Offset function is still active.Select the other six surfaces with the same method.

Once you have created the seven surfaces clcik on the cancel button to deactivate the function.

2. You are going to create a blend surface to close off the Offset Surfaces.

Click on the Blend icon  .
The Extremum Definition Dialog box is opened, select the Maximum option.
Select the edges and the support surfaces as shown below.

Click OK to confirm the blend creation.

3. You are going to Insert a JOIN operation to assemble all the Offset surfaces and the Blend surface into one single surface.

Multi select the seven Offsets and the created blend. 

Click on the Join icon  .

All the pre-selected objects are added to the join list. Click on OK to confirm the Join creation.

4. You are going to Extract a Boundary Curve from this JOIN surface.

Select the Boundary icon  .

Select an edge of the Join as shown below. 

Click on OK to confirm the Boundary curve creation.

5. You are going to Create a Sweep Surface using the circular section curve (Output1) per parameters on the right.

Click on the sweep icon  .

In the Swept Surface Definition dialog box choose a Line Profile type and ’’With reference surface’’ Subtype.

Select the Output1 circle as Guide curve1 and the Output1-Plane as Reference surface.

Key in –88 degrees as Angle value and 100mm as Length 1

Click on OK to confirm the Swept Surface creation.

6. You are going to create a Loft tangent to the Join and the Sweep surfaces
Select the Loft icon  .
Select the Output1 as first Section and the Sweep.1 as tangent surface.

Select the Boundary.1 as second section and the Join.1 as tangent surface. Check that the two profiles are in the same direction.

Click OK to confirm the loft creation.







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