It had been few weeks since I’ve put up any trick or tutorial. Joseph Huntley from Scale Model Design And Fabrication Services, L.L.C recently asked one question “SolidWorks Google group (SWCad)“ where he need to have an intermediate sketch on an intermediate plane between two parallel sketches.
Usually one may use Projecting Sketched Curves with Sketch on Sketch option. But what he needs was as below so this option failed.
So basically how to get this intermediate sketch. Here is the way:
1. The trick is to use loft (either surface or solid). I’ve used a surface loft because eof open geometry.
2. Select the first sketch as the profile.
3. Select the second sketch as profile.
4. Hit OK.
5. Here is the result of surface loft.
6. Now right click on the loft and select “Add Loft Section” option.
7. Select the option “Use selected plane” in feature property manager and select the intermediate plane.
8. Hit OK
9. An extra sketch (a spline) will be added at the selected plane.
10. You can delete surface loft feature if required.
11. Here is final result after deleting surface loft feature.