Migrating from Inventor 2022 to 2025 – problems with iLogic driven parts and extrusion input geometry profiles changing

[curtwatson1]

We are attempting to migrate from Inventor 2022 to Inventor 2025 and noticed several iLogic driven parts within our assembly behave differently between the two versions. Changing the part in Inventor 2025 is much more problematic. When iLogic is used to update the sketch parameters the model will break and cause several extrusion input geometry profiles to need to be redefined in Inventor 2025, but this does not happen in Inventor 2022.

I’ve attached the representative part file in Inventor 2022 format below. I’ve also recorded two screen recordings illustrating how the part will change (and break) when the controlling parameter is changed using a simple form when the part is modified from within both Inventor 2022 and 2025. In Inventor 2022 the sketch occasionally needs correction, but in Inventor 2025 the extrusion input geometry profiles often change, and this is more time-consuming to correct.

I don’t think this is an iLogic or coding issue within the part but more a change in how Inventor 2025 processes the parameter updates. I would really appreciate it if someone could explain why this is occurring and provide any recommendations on how best to correct this behavior so we can continue to move forward using Inv 2025 without increasing the time it takes to change our model. Has anyone else experienced this when migrating to a newer Inventor release? Could this be a bug that should be reported?

Thanks in advance for any help!

Inventor 2022 Example

Inventor 2025 Example

[andrewiv · Accepted solution]

Do you need the extra profiles on that sketch?  If you make it so that the sketch only has the one closed profile then it will be correct.

[curtwatson1]

Thank you!  Editing each sketch by changing the outside circle to a construction line and adding arcs/lines to close the geometry again where needed is a workaround which appears to correct the issue in Inventor 2025.   It's no longer necessary to edit the extrusion feature and re-select the correct input geometry profile. 

However, Inventor 2022 did not seem to have this issue...  I'm sure we'll run across it again with some of our other models that use shared sketches or have extra profiles.  This seems to be a bug in Inventor 2025 since previous versions were able to "remember" the correct profile geometry for extrusions when parameters are changed.

[johnsonshiue]

Hi! I took a quick look at the part and the iLogic rule. I guess this is a limitation in the way the Sketch12 is solved. The arc length and the thin profile may have inconsistent behaviors because the result depends on the solve order. The arc length needs to be solved the last. However, the sketch solver isn't sequential when solving a sketch.

Maybe you want to break the Sketch12 into separate sketches so that the sketch solve becomes sequential. I am also able to reproduce the same behavior in 2022.

Many thanks!

[curtwatson1]

Mr. Shiue,

I've been trying to figure out how one would go about breaking Sketch12 into separate sketches for the Baffle extrusion so the sketch solve becomes sequential.  Everything I've tried seems to "break" worse than it did before...

However, limiting the profiles as @andrewiv suggested seems to have corrected the "re-selection" of input geometry behavior the model was exhibiting for me in Inv 2025 and now the model works again (at least it works like it did in Inv 2022).

Thank you both!