CAD Forum

I'm cleaning things up... in my Design Library. This is a pleasant mystery for once.

I have a bunch of parts badly imported from STEP files from the manufacturer. They come through as broken surface bodies, some with errors unresolvable by Import Diagnostics. I very well may have imported these in a previous version, and now somehow 2018 SP5 handles it better.

I have an Imported Bodies folder, and below that a Patch Bodies folder with manual edits. In various examples, I had between one and 8 erroneous imported surface bodies in that folder. In every example, all I really did was threaten it with repairing it. I created a plane. I converted an entity into a sketch on that plane. I extruded a solid from that sketch. I moved the new features into the Patch Bodies subfolder - and that is exactly when all of my erroneous surface bodies lost their errors. I was delighted. I moved on to the next one and the same procedure applied equally.

I really do not mind errors disappearing. I love it. However, I'd like to understand it. What am I missing? Is it a version thing? Was I merely holding my tongue in the correct position this time?

can you do a GIF ? to show us that magic effect

Obviously SW understands they're fixed when they are placed in the "patched" folder. Just rename the folder "broken" and the errors will come back.


I remember there was a bug they issued a fix for where SW was too aggressively enforcing checks on imported geometry. It was actually causing data loss. Just a shot in the dark, that it may have to do with this...probably not, though.

Can you post a couple parts for people to try to replicate this behavior?

This is pretty specific behavior. You may get your VAR involved?

Turn on VOR and do a CTRL Q and see if the errors come back.

dpihlaja wrote: ↑Fri Apr 23, 2021 7:55 am Turn on VOR and do a CTRL Q and see if the errors come back.
image.png

Nailed it, Dan. Thanks! The same errors returned right away. I'm turning that back off. Happier w/o it.

It's not often that I get to say, "What did I do right?"

mattpeneguy wrote: ↑Fri Apr 23, 2021 6:54 am Can you post a couple parts for people to try to replicate this behavior?

Unfortunately the worst ones (all the ones I was pretending to repair) are all bound by a NDA w the MFR. I will try to find another use case with less restrictive source, like an online download.

Edit: I did find one. I imported STEP w/o VOR and it came in w no errored bodies, although it had plenty of import diagnostics issues available to heal. All I did was turn on VOR, rebuild, and then errors (Warning: Error(s) found.) all popped up. Toggle back, rebuild, and they disappear. There's not much to share there, as it was not the moving of features into a folder - itself - which caused the errors to disappear.

I am very willing to bet that I had VOR on for years before disabling it. That's most likely why I had these bad parts then, and not now.

Merovingien wrote: ↑Fri Apr 23, 2021 4:24 am can you do a GIF ? to show us that magic effect

I initially described it as magically but changed it to unexpectedly because linguistically "magic" merely applies to that which I do not adequately understand.

Tom G wrote: ↑Fri Apr 23, 2021 9:40 am Nailed it, Dan. Thanks! The same errors returned right away. I'm turning that back off. Happier w/o it.

It's not often that I get to say, "What did I do right?"

Just because the error warnings disappear doesn't mean the model is magically fixed, especially if VOR is the "cause" of the errors.

Most error checking in SolidWorks checks each face against all of it's adjacent faces to make sure the faces only touch at edges, and have no gaps.

VOR checking checks each face against ALL THE OTHER FACES IN THE MODEL. This is a much more thorough check. If it fails with VOR and is ok without it, the model definitely has an error, it just takes longer to find it.

Here's a model that has no errors, but you can see with your own eyes that its wrong. This was made with VOR off. The outer fillet is so large that it goes through the shell. It follows the rules - no adjacent faces penetrate each other.
With VOR on, it fails because some face on the model penetrates another face.
This kind of thing happens on more complex models where it's harder to see.

matt wrote: ↑Fri Apr 23, 2021 9:59 am Just because the error warnings disappear doesn't mean the model is magically fixed, especially if VOR is the "cause" of the errors.

That don't confront me.

It's not magical. It's relevant and useful. I'm not making the thing. I'm making a bigger thing with this purchased thing in it. I could care less how internally messed up it is. I DO care about a few things: where does it mount by bolt down holes, where do its connections go, how much space does this take up to obstruct movement of other things.

Turning off irrelevant errors helps reduce delays in (large) assemblies and drawings which contain this product.

This is an example. The brackets are the two solids, and all else are surface bodies. With VOR on, I get a half dozen errors on surfaces. All I need here are bolt downs, motor attachment, and hose attachment locations.
All the same, your example images explain the situation better than I have ever seen.

Tom G wrote: ↑Fri Apr 23, 2021 10:13 am ...
Turning off irrelevant errors helps reduce delays in (large) assemblies and drawings which contain this product.
...

I understand, that's ok. As long as you're sure that the errors really are irrelevant.

Tom G wrote: ↑Fri Apr 23, 2021 9:40 am Nailed it, Dan. Thanks! The same errors returned right away. I'm turning that back off. Happier w/o it.

It's not often that I get to say, "What did I do right?"

So just so you know....those errors aren't gone. They just aren't being checked for. Anyone else opening that part with VOR on WILL see those errors.

Also, leaving errors in there can mess with how well mates apply to the part and how well things show up in drawings.

So....buyer beware...

dpihlaja wrote: ↑Fri Apr 23, 2021 10:26 am So just so you know....those errors aren't gone. They just aren't being checked for. Anyone else opening that part with VOR on WILL see those errors.

Also, leaving errors in there can mess with how well mates apply to the part and how well things show up in drawings.

So....buyer beware...

..yep, the red lipstick is still there..

matt wrote: ↑Fri Apr 23, 2021 10:17 am I understand, that's ok. As long as you're sure that the errors really are irrelevant.

Every body is so short sighted. Yes, you can have a surface-based representation of your purchased component. That my be ok for the design aspect- you mentioned you only need space-claim and mounting locations. But what about everything else this affects!
Think about drawing views and the update its going to take on resolving the hidden lines for all the surfaces. Think about your drawing views that show all these goofey lines and stuff because you might actaully have surface that intersect and the HLR process can't resolve.
Think of your assy and GPU as you move up through your design structure.
You may only care about what you need to do your job. But the company and your customer cares about the quality of work. It affects them as well!
Quality data impacts your design, your documentation, your quality, your manufacturing and your customer. Don't SKIMP out on your 3D data quality.

My rant for Friday!