Features fail randomly in stable model some time after

[georgebirch]

This has happened a few times in my career but this time it's annoying all of us in the team.

A part has been released for manufacture - a faily complex injection molding with a hundred or so features.

The model was released, the geometry all fine, no failures or invalid surfaces etc. And there are no references to any external files

But, weeks after release, when fiddling with some parts in the assembly, or even just randomly, a fillet or draft feature suddenly fails and we have to fix it (carefully making sure it is still identical to the released part)

We are using GrabCAD as our PDM system, maybe this is part of the issue

Any wisdom appreciated

[DanPihlaja]

Is this setting turned on?

If not, my advice is to turn it on and leave it on.

[Jordan Brown]

Is this setting turned on?
image.png

If not, my advice is to turn it on and leave it on.

That is a lesson we learned as well. When we do our surfacing and get hundreds of features everything must be perfect. We would sometimes get to the end of a complex part, and then have something fail way up in the first firth of the tree.

If nobody uses it, then sometimes the problems are masked over and never found. But if someone has this setting turned on later everything can explode.

[RichGergely]

That is a lesson we learned as well. When we do our surfacing and get hundreds of features everything must be perfect. We would sometimes get to the end of a complex part, and then have something fail way up in the first firth of the tree.

If nobody uses it, then sometimes the problems are masked over and never found. But if someone has this setting turned on later everything can explode.

Doesn't matter if it is turned on later or not. If you put a new version of Solidworks on your computer, as default, when it rebuilds it does the in-depth rebuild = the same as verification on.

This is why you would see designs that worked perfectly fine in in a old version suddenly go back years later it doesn't rebuild. The problem is likely that it was always there it's just the new version by default does in-depth rebuilds on old files until it is saved to new version with the rebuild.

[SPerman]

I don't know how much of an impact it has in 2022, but turning that on will slow things down.

[RichGergely]

This has happened a few times in my career but this time it's annoying all of us in the team.

A part has been released for manufacture - a faily complex injection molding with a hundred or so features.

The model was released, the geometry all fine, no failures or invalid surfaces etc. And there are no references to any external files

But, weeks after release, when fiddling with some parts in the assembly, or even just randomly, a fillet or draft feature suddenly fails and we have to fix it (carefully making sure it is still identical to the released part)

We are using GrabCAD as our PDM system, maybe this is part of the issue

Any wisdom appreciated

As Dan says tick verification on rebuild and in addition to that do regular Ctrl+Q on complex parts.

Worth noting - Sometimes, on certain complex parts or mates first rebuilds fail, BUT, doing a second rebuild suddenly it fixes and continues working fine. What seems to be the common factor in this behaviour is simply editing a feature.

[DanPihlaja]

I don't know how much of an impact it has in 2022, but turning that on will slow things down.

image.png

Agreed. It is a slower cycle time.

And there are times where I have had to turn it off to deal with a problematic casting from a supplier.

but for the most part, I leave it on.

[bnemec]

Agreed. It is a slower cycle time.

And there are times where I have had to turn it off to deal with a problematic casting from a supplier.

but for the most part, I leave it on.

Hope it's ok to jump in, a bit off topic. Is this a place where we could use the "freeze bar" to help reduce build time? In theory, if we have that check box checked to do a "verification on build" then once those early features are build and known to be good we can freeze them and only rebuild new or edited features.

I've heard bad things about the Freeze bar, causing problems, but not verifying on build can cause issues to "hidden" as well. IIRC the problem with the freeze bar is when someone pulls it down below a feature that has external ref. But if it does what they say it does it seems like a good tool when used properly.

[Jordan Brown]

I think that the freeze bar would depend on your workflow. When we have extensive surfacing work to do, we design the surfaces in an independent part, export the final thing as a parasolid, and then import into a part that we use in our assemblies. It is certainly a little more work if you need to edit things later, but it also gives a lot more stability to your assembly.

As for verification on rebuild, again, we only use it when we are working on the external part. We turn it off when working in large assembles to save on the rebuild time.

But if the complex geometry needs to be parametric then I think that both the Freeze Bar and using parasolids are out the window.

[DanPihlaja]

Hope it's ok to jump in, a bit off topic. Is this a place where we could use the "freeze bar" to help reduce build time? In theory, if we have that check box checked to do a "verification on build" then once those early features are build and known to be good we can freeze them and only rebuild new or edited features.

I've heard bad things about the Freeze bar, causing problems, but not verifying on build can cause issues to "hidden" as well. IIRC the problem with the freeze bar is when someone pulls it down below a feature that has external ref. But if it does what they say it does it seems like a good tool when used properly.

External references and the freeze bar don't play nicely. However, if there are no external references, I use it all the time!