SolidWorks Tip - Create an extrusion on a non-planar surface - Step by Step w/ pix

SolidWorks Tip - Basic Extrusion on a Non-Planar Surface - SolidWorks Tutorial by Video-Tutorials.Net

Last week someone sent in a request about how to create an extrusion on a non-planar surface. The surface in question was a cone-shaped extrusion. This SolidWorks user was having trouble creating the extrusion from the blue curve shown on the left.  The fact that the extrusion is based on a non-planar surface does add some complexity to the operation, but SolidWorks will definitely let you create the extrusion.  In this short SolidWorks lesson, I'll show you one way to create it.

I'll begin by creating a cone-shaped extrusion. This can be a simple extrusion with a draft applied.   Let's try it as outlined below:

1. Create a sketch on the top plane

2. Draw a circle in the graphic area. You don't need to dimension it at this time.  Exit the sketch.

3. Go to the Features tab.  Activate the Extruded Boss/Base Command.  We'll make the extrusion depth 100mm.  Press the tab key on your keyboard to register the data so you can see the preview.   While you're still on the direction 1 control area, click the Draft option on.   Enter a value of, for example, 30 degrees.  Tab to register, and you'll see the preview. Accept and you will have your cone-shaped extrusion.

4. Next we'll create a new sketch on the right plane. With the sketch selected, take a Normal-To view.

5. Draw a circle and exit the sketch.

6. Take an isometric view.

7. Go to the Features tab, then Curves > Project Curve. You can also get to this tool via Insert > Curves > Projected Curve.

8. The Projected Curve command manager opens. Select the Sketch on Face option. Select Sketch 2 if it isn't preselected. It should be.  Now select the face to which you'll project sketch 2. The name of the face appears in the selection box, as you see below.   You can click the arrow that appears in the graphic area if you need to change the direction of the projection.   Click the green checkmark to accept your changes.

9. Now I need to convert this curve to a 3d sketch.  Let's go to the Sketch tab.  Click on the menu flyout arrow of the Sketch command button.  Select 3D Sketch.    

10.  Click the  Convert Entities tool.   The circular edge, Edge 1, is preselected, as shown below.  Click the green checkmark to accept.   Then exit the sketch.

11.  We need to create 1 more sketch. This time it'll be on the front plane.Take a normal to view. Activate the line command. Draw a line as shown below.  The reason?  We'll use this line as a direction vector for the extrusion.   Accept and exit the sketch.

12. Time to create the extrusion.  Take an isometric view.  Click in the graphic area to deselect everything.  Activate the Extruded boss/base command on the Features tab.  Select the 3D sketch (the curve shown below).   Next we specify the direction to extrude.  I'll select the line I just created.  The preview of the extrusion displays as shown below.  We'll leave the extrusion depth at 100mm.   Be sure to uncheck Merge Result (in the Direction 1 control area).  Click the green checkmark to accept the extrusion.

13. To hide the cone, expand the Solid Bodies folder. Right-Click on Boss-Extrude 1 and click Hide (the glasses icon).

14. Now you should see your extrusion! Have fun.

 

Thanks! Rosanna D, Video-Tutorials.Net