My part is missing one of its internal faces. The face was created by cutting a hollow out of a larger solid, so I can't select the face itself in the tree or anything.
I've seen elsewhere that there is probably an error caused by my use of fillets, and probably freeform. However, the face is symmetrical to the opposite side, which shows fine.
I read about it here: Missing face on solid body
I'm having trouble finding my error though. Any ideas?
Maybe it's just a display error. If one face is missing, the object would be a surface. But the edges are displayed in black color, which indicates "solid body". Surfaces have a blue outside edge color by default. What do you have in the project tree? Solid or Surface?
I'm not sure, I usually only work with solid bodies, but I used freeform here as well, if that's considered a surface.
I attached the model above if that's easier.
I have also tried adjusting Options > Document Properties > Image Quality, that didn't work.
Unfortunately I have older version SW.
There seems to be something wrong with your sketch (sketch 2 of cut extrude 7 - the error exists after your second feature). If you replace the line that's making that face in the cut with a new line, it works. (turn the line into construction geometry, and then draw a new line over it). Of course making equation driven nested contours, but using the region anyway is a freakishly complex way of asking for problems. Is there a reason why you did it that way?
I have no idea why I did it that way... I have learned a lot since I drew that sketch.
Thanks for your help, I drew a simple rectangle in the sketch and it fixed the issue.
Also, if you delete the second feature and recreate it, the problem doesn't return.
Do you run into issues like this a lot?
Not really. I have run into some relating to sketches, but I can pretty much chalk all of it up to still learning.
That's weird... Did you roll back and add that cut later? Because it's the second feature in the tree... Or did that face disappear sometime later and just never come back? I'm surprised that turning on Verification On Rebuild doesn't find it.
Or did that face disappear sometime later and just never come back?
Yes. I must have referenced something in the sketch that I later changed/removed.
I used Rebuild, but not sure what you mean about Verification On Rebuild. If that's the dialog if something is wrong, then no, nothing was found and I expected something too.
Matt Helm wrote:
Or did that face disappear sometime later and just never come back?Yes. I must have referenced something in the sketch that I later changed/removed.
I used Rebuild, but not sure what you mean about Verification On Rebuild. If that's the dialog if something is wrong, then no, nothing was found and I expected something too.
"Verification on rebuild" is a system setting in the "Performance" category under Tools->Options. It does some advanced body checking that's not necessary 99% of the time for normal users, so it's usually turned off by default. More info:
VOR Improvements (Verification on Rebuild - Extra Body Checking)
Or another option is copy the whole part by using Move/Copy Bodies it will be OK. But in this case you must not combine the bodies.
There seems to be something wrong with your sketch (sketch 2 of cut extrude 7 - the error exists after your second feature). If you replace the line that's making that face in the cut with a new line, it works. (turn the line into construction geometry, and then draw a new line over it). Of course making equation driven nested contours, but using the region anyway is a freakishly complex way of asking for problems. Is there a reason why you did it that way?