Having trouble getting a surface loft that was turned in to a solid to combine

Rich,

I tried opening the file, since your profile says you are running SW 2010, but I got the old future version error, so I guess you have moved on to 2011 or 2012 while I'm still stuck at 2010. Could you post some pictures?

Failure to combine often means that you've got areas that are just touching, rather than overlapping, or you've got an area that will result in a zero thickness, like a cylinder tangent to a plane.

Jerry Steiger

I was able to get it to work, but I'm on 2012, so I can't just upload it back here for you.  I'll try to explain how I did it. 

OK, so you have Surface-Offset36 on your base part that you used to create the profile you're lofting to.  After you create surface-loft14 and you're happy with the result, hide it and the surface offset so you can see the base part you're trying to attach that loft to.  Then, start a delete face command, select the option to just delete, not delete and patch or delete and fill.  Select the faces within Split Line18 and hit OK.  You'll now be left with a surface body instead of a solid.

Then, turn the surface-loft and the planar circle you lofted to back on.  Start a surface knit command, and knit it to the rest of the base part.  Select Gap Control and you'll see you have two small gaps, this could be the problem in getting your part to combine maybe?  When in the surface knit command, tell it to try to form a solid, and you'll be in business.  Worked on my machine no problem.

I've noticed on occasion if I try to do a combine feature when fillets or funky surfaces are present and your surfaces directly coincide with eachother,  (meaning the bodies do not extend into eachother,) you tend to get some disagreement from SW, because it sees small gaps or zero-thickness conditions.

Hope that helps!