Placing features inside a shelled loft

jan_rychter

I'm having trouble figuring out how to place features inside a part that is created by a) a loft between two cross-sections, b) a shell feature that removes the inside of the part.

I'm trying to extrude features from the internal floor plane (inside the shelled part), but the extrudes are not limited by the loft, so they protrude on the "wrong" side, too. I have no idea how to avoid this. I tried boolean operations, extruding from a face to another face, but nothing seems to work. The best I could do for ribs was extrude from one (internal) loft face to another, but that limits the rib height to the height of my curvature, because you can only use a single face to limit an extrude on each side, not two conjoined faces.

This is a problem when creating internal features such as ribs, screw mounts, etc.

Hopefully the attached pictures illustrate the problem. Any tips appreciated.

NeilCooke

Two options:
1. Extrude in the opposite direction and use up to next or up to part.
2. Create it as you have then use delete face to remove the bits sticking out. 

jan_rychter

Well, that will indeed work for those supports, but won't work for a grid of ribs (#-pattern). Both "Up to next" and "Up to part" will encounter a face or part, which won't be the desired end, but another rib at a right angle.

Removing the bits sticking out sounds good, unless I have to do it for 24 or so ribs and worry about things breaking whenever my parameters change…

premysl_janecek

Hello there Jan.

Did something like this in the past, while working on a model of charge air cooler plastic end tank.

Here goes the tip:

Do an extrude of the bosses or ribs to be too long on purpose (use blind option and be bold with the distance), so it will positively stick out of the part on the other side. Then, prepare an offset surface (or surfaces) that have to lie inside the volume they are not supposed to go out of. In the end just use Split command to cut the problem parts of the ribs or bosses off.

It is very similar to Neil's number 2, but it wil (if the offset surface(s) is(are) done wisely) survive parameter changes, as the delete face command does (in its nature) involve some gueswork.

The difficulty here would be to get the skin surface of a solid part, but that is something yet to be implemented as I believe.

jan_rychter

Hey, thanks, that is an interesting suggestion — I will try that. It sounds a bit complex in cases where there are multiple surfaces (like in my case, a curved part and a straight part), but should be doable!

BTW, I hope OnShape will implement features for ribs and gussets like SolidWorks does. Things are much easier there.