Single Curve with Stop at Intersection worked. Thanks!
Can I ask for more - I have to click on the two vertical lines and the two arcs. Can I click in the center open area and it picks that area with one click?
Depends on what version of NX you're running. Starting with NX 7.5 we added an additional option to the selection 'Curve Rule' titled 'Region Boundary Curves'. In this case all that you need to do is place your cursor in the 'region' and you will see it highlight and when you press MB1 that region will be used as the selected profile. Note that there are some limitations, such as the fact that this only works with sketches or the faces of a body, that in the case of a sketch, the boundary must be defined by a single sketch, that is you can't use overlapping sketches and use this new selection option (the manual selection tools including stop at intersection and single select will work with multiple overlapping sketches).
John R. Baker, P.E.
Product 'Evangelist'
Product Design Solutions
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
Thanks John, the Region Boundary Curves helped a lot. I selected one region and then manual selected other sketch lines and I get an error "The input selection is invalid". Is the attached screenshot possible as one extrude?
You can't create that solid as a single feature since the model is non-manifold (specifically you have edges which are attempting to be shared by more than 2 faces, a classic non-manifold condition). The best that you can do is to create it as two separate features, the single 'circular' central body as one extrude feature and the two 'C-shaped' sections as the second feature.
John R. Baker, P.E.
Product 'Evangelist'
Product Design Solutions
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
