Anyone seen a case where placing a hole feature in a existing boss with a pilot hole deletes the entire part?
First image shows the first two holes placed with the third pilot hole and all of the surrounding part geometry.
Second image shows third hole placed deleting the entire part except the hole itself.
Yes. We are required to model at Absolute .0005. However, I tried A.001, A.002, A.003, A.005, and R.001. All yield the same results. Oddly it isnt just that location. This part has hundreds of these bosses. The hole feature will go into most of the bosses I have tried without deleting the entire part. It only occurs in certain bosses. However, they are in random locations throughout the part.
May have to call PTC!!!
What I have noticed is if I place the hole all the way through the part it doesnt have the same affect. Additionally, if I place a extruded cut in those same locations to a specified depth it still deletes the part. However, if I place the cut through all it does not delete the part.
I have seen this on occasion. It shouldn't happen, but it usually has to do with the dimensions of the new feature and proximity to edges or vertexes in the part. Nothing jumps out in your screen shots, but I'd try tweaking the dims of the feature to see when it causes the trouble, that can lead you to a solution.
I'd also look for other geom checks in the part. My experience is that a geom check that seems to regen how you want still means that Creo is guessing about what should happen and happens to be guessing right. It can lead to odd results like this later down the tree sometimes. Resolve those and you may clear this up.
This is the exact reason very clients maintain their support contracts. This needs to be reported if for no other reason to have PTC acknowledge that these types of things are still happening; just in case someone snuck in there and ticked off the "done" box on something that is far from resolved.
Patrick, what version are you using?
I still have a nasty bug on patterned features that would disappear instances on random locations of the pattern. I drove that one through support team to resolve. They said it was resolved in M050 and sure enough, it popped back up in M090 IIRC. Sometimes it is easier to live with a bug than to find new ones that stop you dead in your tracks.
The only other option is a revolve. Again, none of this should be necessary. As Doug said, you may have to backtrack to the place the hole surface was created. Most likely, this is the culprit. You can also try moving the pilot holes to after these hole features or removing them all together. I have seen instances in some functions that did not like origins floating in space. Something like the Auto Remove switch setting can get confused.
Anyway, I hope you get a chance to report it and let PTC fix their issues. When I have a feature I need, I don't like having to tweak it just so the software will accept it.
What does the model look like shaded?
I'm guessing from the pictures that there is solid geometry that is the inverse of the hole and pilot, but that doesn't make entire sense. Still, that's what it looks like.
One way to tweak this sort of situation is to use an orientation plane that is not at 90 degrees to existing geometry for linear protrusions or sketch planes not perpendicular to the sides for revolves. This avoids having some geometry almost aligned, but not close enough to be actually aligned, causing the software to fail.
I don't know how an orientation change can be applied to holes, but if it works for cuts then that's a start.
The other try is to insert the failing hole ahead of all the other holes to see what happens.
No other geom checks in model.
Turns out it is related to (or at least it goes away) the formed state of the part (Flatten-Quilt). The hole can be placed in the flat state with no problem. However, it seems it would be a problem with all of the holes in the rolled state rather than a select few locations if it is truly related to the Flatten Quilt feature. The pilot holes are drilled on the flat part. The part is then rolled. Then the tapped holes are modeled. So basically how the part is actually built.
2 comments: 1) you can place datum points on the flat state and have them move with your quilt deformation. and 2) is the surface you are placing the holes on not truly flat?
1) Tried that, the points or curves placed in the flat do not move with the quilt deformation. They stay in the flat.
2) The surface in the flat state where the pilot holes a modeled is flat. The formed shape is conical...which completely screws up every pilot hole for reference.
So what I am doing in the formed state is creating a datum curve through the two pilot hole curve vertices, creating a datum point at the center of that curve, creating a datum axis throguth that point normal to the conical surface, creating a datum plane normal to that datum axis through the point at the center of teh datum curve. The datum plane is the placement place for the tapped hole in the formed state. The datum axis is the locating axis for the tapped hole.