What happened to my assembly? - Graphical Issues

[SPerman]

I was working in my assembly, and all of a sudden instead of the normal shaded with edges view it now looks like this:

In addition, if I try and rotate the model at all, it just disappears, and the only way I've found to bring it back is to select a pre-defined view. And then it disappears again as soon as you try and rotate.

I tried restoring to a saved custom setting, but that didn't help. I've toggled realview graphics on and off.

After further searching it appears to be limited to this asssembly and a few of its sub assemblies. Is it possible they've become corrupt?

SW2020SP5. Enhanced graphics is ALWAYS off.

[AlexLachance]

Try to do a save as that creates a new file and see if the new file is fixed. Sometimes doing that purges some data and fixes minor issues.

I've never seen something like that. Maybe your graphic card updated itself..? Have you tried "Emulate OpenGL" if possible..?


Edit: Maybe look into the document properties and see if the image quality somehow switched by itself.

[SPerman]

I rolled the assemblies back to their previous version, and that has solved the issue. I didn't lose too much work because the parts I was working on were unaffected. But I did lose a couple of hours chasing and fixing this. A couple of hours that will come out of my weekend.

[JSculley]

I was working in my assembly, and all of a sudden instead of the normal shaded with edges view it now looks like this:

image.png

In addition, if I try and rotate the model at all, it just disappears, and the only way I've found to bring it back is to select a pre-defined view. And then it disappears again as soon as you try and rotate.

I tried restoring to a saved custom setting, but that didn't help. I've toggled realview graphics on and off.

After further searching it appears to be limited to this asssembly and a few of its sub assemblies. Is it possible they've become corrupt?

SW2020SP5. Enhanced graphics is ALWAYS off.

This is the behavior you will see if one or more components are positioned far, far away from other components. If everything 'disappears' when you zoom to fit, that's also a sign. If a predefined view makes things 'reappear', it likely just means that the out of position part is far away in the direction normal to your screen. If you use the SHIFT key along with an arrow key to rotate the model 90 degrees and then Zoom to Fit it will seem to disappear again. When this happens to me, I click on a part or subassembly in the feature tree and then Zoom to Selection. Repeat until the wayward component is found. Once you have it, you can add a mate to force it back to the other parts which will correct the display issue and then add a distance or limit mate to keep it from running away again.

[SPerman]

Thank you! That makes sense. The strange graphics display had me chasing the wrong thing.

[SPerman]

In hindsight; a couple of years ago I came across a bug where a hole wizard sketch added a point at 1km,1km (or whatever the extents are.) My best guess is this happened again yesterday. I had a hole wizard in a part that wouldn't rebuild after I added some points and I couldn't figure out why. I finally just deleted the feature and rebuilt it. Thinking back to yesterday when the hole wizard problem started, which assemblies were affected, when I suppressed the feature, and when I unsuppressed the sketch, things line up. So rolling back the assemblies did nothing but create a little more work for me. It was suppressing the sketch and/or rebuilding the feature that solved it.

[bnemec]

In hindsight; a couple of years ago I came across a bug where a hole wizard sketch added a point at 1km,1km (or whatever the extents are.) My best guess is this happened again yesterday. I had a hole wizard in a part that wouldn't rebuild after I added some points and I couldn't figure out why. I finally just deleted the feature and rebuilt it. Thinking back to yesterday when the hole wizard problem started, which assemblies were affected, when I suppressed the feature, and when I unsuppressed the sketch, things line up. So rolling back the assemblies did nothing but create a little more work for me. It was suppressing the sketch and/or rebuilding the feature that solved it.

Thanks for sharing Scott.

Solid Edge taught me when a single file is bad on any workstation/user to just start suppressing features from the bottom up. Most of the time that reveled what bit of "code" went bad in the file. (I consider history-based modeling as a very high level and specialized WYSIWYG programming language.) But I would not have thought to do that when the problem seemed so much a graphics issue.

[len_1962]

also try CONTROL Q it will sometimes fix graphic glitches