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Solidworks Demo For Industrial Design


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#31 parel

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Posted 06 November 2004 - 04:07 PM

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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#32 parel

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Posted 06 November 2004 - 04:08 PM

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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#33 parel

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Posted 06 November 2004 - 04:10 PM

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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#34 parel

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Posted 06 November 2004 - 04:11 PM

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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#35 parel

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Posted 06 November 2004 - 04:12 PM

Use the bottom edges of the lofts to define the bottom planar surface

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#36 parel

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Posted 06 November 2004 - 04:14 PM

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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#37 parel

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Posted 06 November 2004 - 04:15 PM

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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#38 parel

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Posted 06 November 2004 - 04:16 PM

Fillet the bottom edge 2mm

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#39 parel

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Posted 06 November 2004 - 04:18 PM

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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#40 parel

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Posted 06 November 2004 - 04:19 PM

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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#41 parel

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Posted 06 November 2004 - 04:21 PM

Go to the Solid Bodies folder and pick the top part of the mouse and hide it

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#42 parel

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Posted 06 November 2004 - 05:23 PM

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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#43 parel

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Posted 06 November 2004 - 05:24 PM

Hide the bottom and fillet the edge of the top component

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#44 parel

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Posted 06 November 2004 - 05:26 PM

Create an extruded surface to split the top component again.

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#45 parel

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Posted 06 November 2004 - 05:28 PM

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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