Making Hole active also makes Corner seams active

[sijcooke]

Hi, Please can someone help with this. I have attached my ipt, which is from inventor 2023.

If you open it, run Form1, tick PERF_TOP, and click run.. there are errors because the corner seams become active.

If you view the code in the rule, All PERF_TOP should do is make the Hole3 active or not.

This issue also happens if you just make hole3 un suppressed.

Thanks any help would be appreciated... don't know if its just me or not but i feel i am constantly fighting with software these days.

[aurel_e]

When you tick that PERF_TOP, it is showing an error in the hole sketch.

Fixing that error, will solve your issue.

[sijcooke]

Thanks, but there is no issue with the hole sketch. The sketch is fine. The issue is that inventor is stupidly making the corner seams active.. this in turn may cause an issue with the sketch if the geometry has changed.. but the corner seams should be activate to start with.

[BDCollett · Accepted solution]

You can do the same steps here with Model States to suppress features on/off. If you still want to use iLogic, you could even just test the steps with Model States.

The reason it fails though, is that Sketch10 for Hole3 references geometry from LH-Corner1 and 2. 

You cannot reference geometry that is going to be non-existent when suppressed.

See the pink dots in Sketch10. The hole sketch is not "fine"

You need to re-think the design when you are working with parts like this that have geometry being suppressed. It can be tricky to dimension sketches if the origin axis/point is not in a logical place for what you are modelling.

Sketch10 is easy enough to fix and edit the coordinate system to match the origin.

Works perfectly after.

[sijcooke]

Thanks,
How would you edit the coordinate system to correct the hole sketch? I know
you right click on the sketch and click 'edit coordinate system'... but
where would you set the datum point?

[BDCollett]

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@sijcooke wrote:
Thanks,
How would you edit the coordinate system to correct the hole sketch? I know
you right click on the sketch and click 'edit coordinate system'... but
where would you set the datum point?

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It doesn't really matter where you set it, it just needs to not be referenced to something that you are suppressing, as when you do (in the case of the Corner seams here) it loses reference.

The Origin point in this case is best, because it is static and cannot be suppressed.

Edit the coordinate system, pick the coordinate origin, then select the origin point from the browser. Do the same for the x coordinate to the x axis from the browser. If it is facing the wrong way, select 'Flip Axis'.

It should end up like this:

[johnsonshiue]

Hi! Select the origin point on the sketch coordinate -> select the center point of the part. Also realign Sketch X with Origin X -> right-click -> Ok. This will remove the dependency between Sketch 10 and the Corner Seams.

Many thanks!

[sijcooke]

Thanks for your help, much appreciated.