Hello,
I have got two solid bodies I want to combine. However, for some reason, they don't perfectly match with each other. Interescting or combining them does not fix this.
How can I merge the bodies and have solidworks fill the gaps where the matches aren't perfect ? I will eventually add a filet so that the match looks nice.
Thanks for your help.
All the best,
A.
Hi John,
Yes, this is an age-old problem with SolidWorks and has to do with the Tolerance that SW sets for the use of Parasolids. I tried to get a enhancement going when I worked for the company but never got it thru. The work around, and I do have to do this regularly since my design approach is to usually model just half (or quarter) and I use Multibody extensively - I design consumer products:
If you try to mirror the body and it does not merge, then just before the mirror create a planar surface (anything rectangle, circle etc.) on the mirror plane and then use that surface to do a Replace face on the mirror face of the body you are trying to mirror. This usually takes care of the issue. In some cases If the mirror face of your body is more than one face (indicative of the problem I describe following- then use delete face in combination with Replace face to get it to a single face lying on the mirror plane)
What's happening is that sometimes extrudes (and especially thicken) when offsetting or extruding are not doing so theoretically/perfectly - i.e. the face being offset in is slightly not normal but at a minute angle. If this is the case it will generate a zero-thickness error when mirroring and merging.
I consider this a bug, but it is questionable because all modeling systems have to contend with tolerance.
Mark
Hi Mark,
Thank you for this great explanation. I am not surprised to think this is an age-old problem. As a software engineer I understand that this would be one of the first issues when dealing with 3d modeling.
I am not sure I understand your workaround though. A pictured example would help. However, I found two workarounds eventuall: either try "insert->faces->move" then "offset" and make the extend the faces that don't match so that they extend beyond the surface of the main body, which obviously removes all ambiguities for SW when intersecting. However that only worked for the tail of my model so I had to move the sketches of the wing to ensure it was designed a bit larger than necessary so it would no have ambiguities. This was a bit of work as I had to fix some other sketches afterward but I ended up getting it to work.
The solution proposed by Dennis Bacon works as well, so thanks to him also
All the best,
J.
Hey John,,, Combine the bodies then do a "DeleteFace" (with Delete and Patch) on the faces then things should match up like you would like to see.
I have included a file that I have done this with the surfaces I think you want patched.
Edit:... I think I found another face to patch so I attached another file. This is easier than you may think.
Hello Dennis and thank you for your answer. I verified your file and that is indeed the result I want. I didn't know of that feature. Sometimes it's a bit difficult to search on google for specific features. Obviously, searches for "combine", "fill", "intersect" give good results, but when you are trying to find a specific feature you don't get much out of the search. In fact, I discovered the "move face" feature which also helped for another - much more time consuming - working I found (see answer above).
All the best,
J.
Hi J... I'm not sure where I ran across that solution. I think it was Solid Professor many years ago. Probably most of my tips and tricks have come from reviewing issues people are having on the Forum. Sometimes you can pick something up which comes in real handy in future projects.
Hey John,,, Combine the bodies then do a "DeleteFace" (with Delete and Patch) on the faces then things should match up like you would like to see.
I have included a file that I have done this with the surfaces I think you want patched.
Edit:... I think I found another face to patch so I attached another file. This is easier than you may think.