I am wondering if there is a simple way to get rid of unwanted cavities in a part that I want to be solid. I have attached the part and an image that shows the problem. Any help is greatly appreciated!
Samuel,.. the easiest way I can think of is to select (tangency and a few more)...offset all the outer surfaces (zero).. and thicken/solid. (file attached)
Try the attached file.
Thanks J. Mather this is what I was hoping for - how did you do it?
Samuel Murley wrote: Thanks J. Mather this is what I was hoping for - how did you do it?
Samuel Murley wrote:
Given that I am lazy - I used a different CAD program that has a Delete Void tool.
Here is an image from 3rd CAD program, but unfortunately it missed the two tiny cavities.
Thanks for letting me know!
Paul,,, If you are still available for a consultation... I did the same thing (tangency and a few more) offset 0. Then you end up with one surface. Couldn't figure a way to convert to solid so I tried the thicken.. How do you get the thicken to make a solid filling the inside cavity of the surface. I know I have seen other do this but for some reason I can't figure it out.
What I ended up doing was doing the zero offset thing then exporting to .x_t... Then Importing. had a couple of faces to heal (automatic) which made it solid.
Hey Dennis... hmm there were some small slivers..I'll try to post later.
Hmmm,,,, Here is another method. I used the delete face cus I was going to try an intersect on it. When the intersect failed I realized there were some openings so I filled those suppressed the DeleteFace knitted to a solid. Apparently on the one I exported and imported it took care of that for me.
I get it now Paul.. The thicken to solid didn't work for me because I had some open areas. Your method works great if I select all the surfaces to offset. I had missed a few...
..yeah, there are some very small slivers.. I've attached what I had..
Thanks a lot Paul - this is really useful to know!
A really good tool for finding those open areas is Check Entity. After it runs, double click on the listed item to see where it is on the part.
The other method that can be useful is "intersect" tool.
Extrude a rectangle to cover whole part, and use intersection tool to fill unwanted cavities.
ps. For those who can open SW2018 file attached.
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