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Solidworks Demo For Industrial Design

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Start a Loft between the Edge of the Trimmed Surface and the 2D sketch "Plan View" All required sketches should be in the folder "Sketches for the Main Surfaces" which is nested in the history tree.

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Start editing the loft so that it is curvature continuous at the top. This is done by editing the Start Constraint to "Curvature Continuous" in the drop down menu.

 

Define the loft a little more with guide curves. This can get a little squirrelly along the center line because the guide curves at the rear and front (Rear Section of Side Profile and Front Part of Side Profile ) along the center-line are cut (convert entities) from the Profile Sketch. Use the secondary history tree in the modeling window to pick the right sketch

 

To create a smooth connection along the center line click the guide curves and choose Normal to Profile to make the loft smooth along the center line.

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Mirror the surface bodies along the Right Plane. Generally mirroring the bodies (as opposed to Faces or features) is the most straight forward because the computer does not have to calculate too much information

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If at any point the sketches become annoying or too busy CLick View>Sketches to toggle visibility of Sketches. You can do the same thing with planes, curves, origins etc:

 

I have toggled sketch visibilty so that I can choose the edges of the surfaces to define a planar surface

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Knit all the surfaces together to create a Solid. Check the box that says "Try to form a Solid" (the process is similar to creating a closed polysurface in Rhino)

This will give the model mass properties and gives you the ability to use solid modelling tools on the model

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Shell the solid to give wall thickness of 2mm. If you click on any faces that will create an opening in the shell because those selected faces will not be included in the final shell. So in this case Dont click on any faces because we are interested in keeping all the surfaces

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Created an extruded surface with the 2D sketch that defines the material break between the two colored plastics.

 

This will be used to split the solid body into two bodies along the character line that we defined earlier

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Split the body using the extruded surfaces.

 

Pick the surface

Cut the part

Pick the Bodies that you want to keep from the resulting bodies

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You can see the wall thickness now that you can see inside. Fillet the top edge. Fillets are cool from an engineering perspective they eliminate stress risers at sharp edges, and allow for easier ejection from tooling. Fillets also make your final renders look good because they catch light well.

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Split the model with the extrude. In hindsight it would have been better to combine all the splits in to one command

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