Annoying crashes

[Markaj]

Well all crashes are annoying, but I'd like to know what causes this↓↓;




Its Expert V27, on a 2022 Dell i7 laptop, 16GB RAM, Windows 11, with a secondary monitor. It randomly happens, sometimes something to do with working on a part in an assembly. Sometimes a part does odd things, like an extrude or something that worked previously will fail or reverse, or trying to put an axis in will refuse to work, or a cut that intersects another cut appears confused. Needless to say this will cause a load of failed constraints in the assembly.
Usually time pressure means I just swear a lot & remodel the part & assembly quickly without noting what might have caused it, but I've been using Alibre long enough to know the ropes.
Its only been doing it since upgrading to the above laptop/release V. I have a sneaking suspicion its a hardware glitch, although I do find Microsoft Teams calls will sometimes crash AutoCAD so who knows! TBH I have been tending to avoid using Alibre because being caught on the hop with the random crashes, so don't have much forensic evidence, - I'm hoping the answer might lie in the error code!
tia
Mark

 

[simonb65]

Click on the Details >> button and copy/paste the info to Alibre support with a brief description of what you were doing right before the crash.

HRESU:T : 0xC0000005 is an access violation, so the code is trying to access something that is either not valid or is in memory not belonging to the Alibre application! The details information will show what Alibre was trying to do at the time.

 

[Ex Machina]

You could also contact support and send them a package of the assembly. That might help. But let's see if someone in here knows more about that error than me...

 

[stepalibre]

I expereniced this and there is a thread/posts about graphics regressions in V27, or old hardware related problems.
These settings stopped it completely on my iMac/AMD gpu machine.

 

[stepalibre]

I don't know which setting or combination of settings fixed the error message but those settings seemed to solve the problem on my machine.

Here is the thread I mentioned:

v27 extra crashy?

I am having a much higher than normal amount of crashes. It can be trying open a file, edit a sketch, work in an assembly, I haven't detected a specific task that is a trigger. Running on a laptop and alibre is using the nvidia gaming card not the intel.

www.alibre.com

 

[Markaj]

Hmm well it appears to be a couple of rogue components in the assembly that behave strangely & basically throw everything after they go nuts. Have a look at the part 'Body' it looks fine on opening - and is. However if you go to edit any sketch, extrusion 2 (the back panel) realigns itself to a different plane. It has done this several times & been reconstructed from scratch several times & the assembly rebuilt several times. Each time I think problem solved - & then it comes back.
Is there a more bulletproof earlier release? Ive used Alibre since v15, & whilst its had its idiosyncrasies, this is definitely the most trying. Or is it possibly hardware/software or something else?!

 

[stepalibre]

Hmm well it appears to be a couple of rogue components in the assembly that behave strangely & basically throw everything after they go nuts. Have a look at the part 'Body' it looks fine on opening - and is. However if you go to edit any sketch, extrusion 2 (the back panel) realigns itself to a different plane. It has done this several times & been reconstructed from scratch several times & the assembly rebuilt several times. Each time I think problem solved - & then it comes back.
Is there a more bulletproof earlier release? Ive used Alibre since v15, & whilst its had its idiosyncrasies, this is definitely the most trying. Or is it possibly hardware/software or something else?!

What is this missing design? unrelated?

 

[Markaj]

Hi stepalibre - its the global parameters file, but it will open without them and behave in just the same manner.

 

[Markaj]

BTW this is another random error that pops up from time to time when I use the measure tool. I just click OK & carry on I'm afraid.

 

[stepalibre]

This is a critical issue. The model topology is change after only entering and existing a sketch.





This should never happen..

 

[stepalibre]

Hi stepalibre - its the global parameters file, but it will open without them and behave in just the same manner.

I need that file. The equations need to regen/update.

 

[Markaj]

Enclosed. But that behaviour you have found is exactly what has been happenning. Random failure or misbehaving of features on a couple of parts.

 

[stepalibre]

Thanks.
If you open the file and only hit regen all it will do the same.

 

[Markaj]

Yep its bizarre!

 

[stepalibre]

Hi stepalibre - its the global parameters file, but it will open without them and behave in just the same manner.

Yes, I wanted to check.

This type of behavior can happen when referenced geometry is changed. The upstream or last feature would select the next item in the list. So if an edge is removed from the list it will get the next edge in the list. When the model is updated it will create the behavior we see. This explains why the topology is changed instead of the model failing.

 

[Markaj]

So - are you saying that if a bit of geometry that is referenced has changed, say an edge, the feature that uses wont fail per se, but will just change its reference and move or alter? A bit like in Inventor maybe where it will tell you references have failed - but here it doesn't tell you?
It does sound plausible though, I do find 'project to sketch' works fine until you make an alteration.

 

[stepalibre]

So - are you saying that if a bit of geometry that is referenced has changed, say an edge, the feature that uses wont fail per se, but will just change its reference and move or alter?

Yes. This is a system failure if you don't know which feature is at fault.

A bit like in Inventor maybe where it will tell you references have failed - but here it doesn't tell you?

Yes. The software shouldn't allow this to happen or alert you. I'm going over your example to check if the equations are the cause. Can you share more info?

 

[stepalibre]

I think this issue was caused by saving the file without updating the parameters or something else. When you regen after opening, it will use different values. Alibre shouldn't allow a part to be saved in this state.

 

[HaroldL]

When I looked at the sketch for Extrusion<2> it had constraints from a Project to Sketch operation. It is odd that it re-associated to a different plane.

So, to see how or if it would rebuild correctly, I deleted the errant extrusion and sketch then recreated the sketch via Project to Sketch and Maintain association to source entities. I then recreated the extrusion and applied the same Depth parameter from the EE and rebuilt the model. The only "failure" I noted was the countersunk holes in the back, Upon editing the Hole feature and reselecting the Starting Surface the countersunk holes rebuilt.
I ran Regenerate All a couple of times, saved the part and reopened a couple more times and it has not erred on subsequent openings.

Can't say it is fixed permanently but it has been behaving well on my system.

 

[stepalibre]

When I looked at the sketch for Extrusion<2> it had constraints from a Project to Sketch operation. It is odd that it re-associated to a different plane.

This is the problem. The design data is not valid or to be trusted anymore. There is no data integrity if the topology can be changed in this way. The feature should fail. The system should not allow this. This breaks the parametric system.

So, to see how or if it would rebuild correctly, I deleted the errant extrusion and sketch then recreated the sketch via Project to Sketch and Maintain association to source entities. I then recreated the extrusion and applied the same Depth parameter from the EE and rebuilt the model. The only "failure" I noted was the countersunk holes in the back, Upon editing the Hole feature and reselecting the Starting Surface the countersunk holes rebuilt.
I ran Regenerate All a couple of times, saved the part and reopened a couple more times and it has not erred on subsequent openings.

What if it happens again. This is a core feature of a CAD system that is breaking.