Until you find the source for the issues you can try a workaround assuming you know where the original position was.
The new SW18 3Dinterconnect has cause a fair bit of issues. Maybe toggling this setting on or off might affect something.
Run evaluate & check stringent...maybe you have import body issues that went unnoticed.
Next I would try to use move copy body and align displace body back into original position. The move body doesn't affect face ID so it should work well with downstream dependencies.
Other things I would try. Add a delete body feature and suppress it. Sometimes those toggle-tricks can fix random errors.
Alternatively if that fails try this.
- Open the import part (P1) and select import1 body.
- Save as step. It will ask you if you want to export the selected body only. Confirm with yes.
- Import the step file into SW and run import diagnostic.
- Export the body again to step (S2).
- In P1 Select the import1 body/RMB and choose <Edit Feature> & browse to the S2 to replace the body.
That can cause some issues with dependent features.
Maybe you find something that works....
See what sticks kinda idea...
Thanks for your answer.
I was suspecting the 3D interconnect. However, we always release the "connection" after import so we get a standard "imported body" geometry. But still perhaps that can be one of the reasons so I should try and disable it. If it is so, it's a pity, because importing complex geometry got a lot better with interconnect.
There is no errors in the imported body or surfaces. That is checked.
Move/Copy body could perhaps work. Have not tried it, but as you mention, it doesn't affect the edge/face ID.
I noticed one thing. If I add some feature on the imported geometry I can use that when I reopen the part to get it in correct position again. So when the file is reopened and in incorrect position, editing the feature and click ok directly puts it back in the correct positition. I guess that is similar to your idea to delete body and then suppress it.
Anyway, everything mentioned is just a work around, and the original problem lies within SW2018. We have used this method in several previous versions without any problem at all. So hopfully it will be fixed in SP2 when it is released.
I hear ya. Using workarounds in SW is a means to get the job done. If I had to wait on SW to fix the many quirks that come with this software then I would have thrown it out long time ago. No bull. You have to work with what you can control. That more I read about the 3Dinterconnect the more I get the impression it is beta-status at best. I don't know how often I have used an enhancement-feature only to be shut down half way through because it wouldn't deliver in the real world or broke down easily. It's in its 1st release. Given SW reputation to make 1st release features work, I would recommend against using it for production. As you see for yourself....it comes in faster but obviously you have to deal with a bug now....That doesn't spell enhancement, does it.
As a rule of thumb. I have never started to use a new release before SP2 or 3 and only if I had measureable prove that the new version could deliver more productivity.
I a few instances I would upgrade because of new functionality, but very rarely. Sometimes customers dictate the SW version to be used.
I still do most of my work in 2016. It's not bug free but I know most of the quirks that I need to look out for. And that is the performance advantage that I use to my benefit. Most often I would like to check with test projects to see if SW has come up with new ideas of breaking things. But time is precious.
We pay pre(sub)scription every year but try to upgrade no earlier than every two years. That has reduced the head ache of upgrading at least by about half.
You mentioned a "feature edit trick".
"I noticed one thing. If I add some feature on the imported geometry I can use that when I reopen the part to get it in correct position again. So when the file is reopened and in incorrect position, editing the feature and click ok directly puts it back in the correct position."
Just recently someone had issues with SW2018 files where the material change wouldn't stick unless you used the same feature-edit-toggle trick. It was assigned SPR 1058446. Maybe there is something bigger at work here with SW 2018 file updates.
Some similarity is evident.
Finally found the bug.
As mentioned in the beginning.
- Import customer part with 3D interconnect
- Relase link so it becomes a standard imported body
- Save as SW part file.
- Insert part in assembly so the origin and CSYS are the same on the assy as the part.
- Create new part/parts in the same CSYS in the assy and start modeling with reference to customer part.
Now comes the trick.
We add, in the top level assembly, a coordinate system (ref. geometry) to be able to export the part as stl or stp for our external simulation software in the correct direction.
After this export, SW decides that the parts with imported bodys should be moved to fit the custom coordinate system for some reason. It is like an invisible move/copy body feature. If you just open the customer part, not the assy, you can see that the origin is now moved to where my custom coordinate system was added.
So as you mentioned, I can save my work by doing a move/copy body to reposition the customer part to its original location/direction.
Another solution is to save the assembly and parts first, then add the coordinate system and export to stl/stp and after this close without saving.
But the bug is that if adding a custom coordinate system in the assembly level, and using this to export to stl/stp or iges, it will move parts to so their origin aligns with the customer CS.
What if you had an export assembly template with the coordinate system in it. Then insert the asm 150-2144 and export out from there using the custom coordinate system. That way the CCS is one level up from the imported parts.
Maybe that prevents SW from moving the imported bodies.