Updating ANY parameter from the functions tab crashes Inventor

[Timothyrsands]

I'm looking for any advice on how to determine what is causing inventor to crash any time I attempt to update the attached part file.  If I change # of gear teeth, even a simple chamfer, Inventor cannot resolve the geometry, constraints, or something (that's me grasping a straws as I have no idea how Inventor software works under the hood).

Oddly enough, it just stops updating the part and becomes unresponsive.  I then have to force close the application.  I can suppress features, but it will do the same thing.  The weird thing is that it was working up until this afternoon.  I was able to update the parametrically driven part.  This is a stand alone part with no ties to any other files (aside from being used in an assembly, but that wouldn't affect this parent file).

Has anyone experienced the same thing? 

-Tim

[sundars]

Hi @Timothyrsands 

When inventor crashed did you get a chance to submit a crash error report? If you have done so, can you provide the Report ID or your email and I can look it up to see where its crashing. You can email it to me at: sundarsATautodeskDOTcom.

I did download your part and tried to see what happens with a parameter change. I tried changing num_teeth as well as some chamfer_leg length and in both cases, inventor goes into an excessively long compute. Its not typical and its caught up trying to compute Extrusion 23 and its child sketch (Sketch 28). Sketch 28 looks it has some projected loop. I didnt inspect the sketch, but that seems to be the root cause of the excessive compute.

You can try this as an experiment

1. Move EOP above Extrusion 23

2. Change your parameters

3. It should be instantaneous.

Is it possible that somehow the change in parameter might trigger some sort sketch compute issue - maybe a circular dependency or somehow created a complex condition which triggers an excessive compute? I didnt wait for it to finish but you could letting it run for a little while and see if it completes. I will log a defect on our side to investigate why its taking excessive amounts of time, but in the meantime, please do inspect your sketch and see if there is something obvious and let us know if you found anything.

Thanks

-shiva

[sundars]

@Timothyrsands 

Quick update. In Inventor 2022, I let the parameters change run its course and the operation completed in about 15-20 minutes. While it takes a long time, it does ultimately finish and I dont see a hang or a crash.

Let me know if you are still having issues or if you crash.

Thanks

-shiva

[Timothyrsands]

I was not able to generate a crash report since I was force closing the application from task manager.  I left the part to update for approximately 15 minutes (Went to cook dinner) and when I returned the part was still attempting to update/calculate the updates. 

I tried messing with iLogic and iLogic configurations but I don't really know what I'm doing there in order to generate some sort of report to share. If you have a link to instructions on how to do so, I can try that.

I messed around with sketch 28 and found it is having trouble calculating the large number of small radii and chamfers that are parametrically defined.  I erased the sketch28 and extrusion completely and recreated the sketch at the end of the part.  The same issue occurs.  I determined it is just inefficient and computationally intensive to setup the feature in this way.  I modified the gear width instead of trying to extend the gear width via a projection sketch.

Attached is the new part file.

Below is a screenshot showing the inefficient sketch where I projected the geometry of the gear teeth and attempted to extrude up 4mm.

[sundars]

Hi @Timothyrsands 

I dont see Sketch37 in the part you attached. Can you reattach the updated part?

thanks

-shiva

[Timothyrsands]

I erased sketch 37 in the model.  I only made a temporary sketch just to show what people should NOT do and then removed it from the part and shared the part file.  Here (attached) is the same part but with the sketch and extrusion included.  You can try to change the function parameters to see the error that continues to reliably occur.

[sundars]

Thank you @Timothyrsands 

I have created a defect INVGEN-60539 for us to investigate the slow performance - given that its a complicated sketch with a fair amount of computes, I am not suprised, but we will definitely investigate. What puzzles me is that even a slight change in paramater causes a massive update. I suppose the param change can affect more than just the sketch.

Thanks

-shiva

[johnsonshiue]

Hi Shiva and Timothy,

This is a very interesting case. I suspect the bottleneck is at how the face loop is recognized as a profile in Extrusion. I did a few tests as a comparison.

 - Delete the Extrusion but keep the Sketch. Parameter change is fast.

 - Instead of Extrusion, create a Boundary Patch based on the same sketch. Parameter change is fast.

Another data point, delete the Extrusion, change the parameter and recreate the Extrusion. It will be fast. Something is not done efficiently for sure.

Many thanks!