Suppress/unsuppress error in sheet metal

[L.Greft]

I'm making a parametric part in sheet metal (Inventor 2019) and I want to switch between two different types of flanges. I've both made them and use a rule to suppress one flange and make the other one active.

I use the parameter "FLENSAFST" with two options "0" or "300". When the 300 is active it looks fine also when switching to 0 everything works like it should, but if I switch back to 300 I get an error in the extrustions because of a missing face. When using "Redefine" for the sketch it works again, but since it's a parametric part this isn't a solution for me.

The extrusion is nessecary and I'm only extruding the thickness, so this shouldn't be a problem.

Attached you can find the part, when opening the form you can click on "0" then choose apply and then switch back to "300". I hope someone can help me with this.

[WCrihfield]

I opened your part and launched the local form "Form 1", and switched the option (then clicked Apply) back and forth many times, without any problems.  It transformed the part each time, without showing any error messages.  I'm using Inventor 2021.1 though.

[L.Greft]

@WCrihfield thank you for letting me know.

This part will be a left side and I already made the top side, the top side works fine. The left side is a copy of the top one, but I redifined the first sketch so the orientation is correct. 

I also posted this in the "Inventor Forum" 6 hours ago, but haven't got a reply yet. I've spend all day so far trying to solve the problem within this part, but it doesn't matter what I do, everytime I get the same error. I also tried modelling it from the start instead of using "Save As", but no luck either.

[WCrihfield · Accepted solution]

90% of the time, when dealing with a series of Feature.IsActive() calls, and you're having troubles, it has to do with the order of things in the code.  When turning in-active features back on, you always want to turn them on in the order they were created.  When turning features off, you always want to turn them off starting with the last feature, then the next to last feature, etc.  Always keep dependency's in mind.  If a later feature (or sketch, or work feature, etc) depends on an earlier feature, and you turn that earlier feature off, it will cause problems.  When turning later features on, before the things they depend on have been made available, it will cause problems.

If I were you I would shuffle the order in which you are turning things on and off.  This will most likely solve your problems.

[WCrihfield]

@L.Greft 

Also, check the sketches that your extrude features are based on.  If they are set up so that you have to manually select one enclosed region out of multiple available enclosed regions in order for it to know which profile to extrude, that will cause problems too.  You want those sketches done properly.  The only 'non-construction' lines/geometry should be the 'closed' geometry of your extrude area.  No 'non-construction' geometry overhanging.  All other geometry that is not part of the profile to be extruded should either be deleted, or turned to 'construction' geometry.  When you click on the extrude command, it should automatically start to extrude the only available profile.  If it doesn't, you may have to make some adjustments to your sketch, in preparation.

[L.Greft]

@WCrihfield thank you so much for the help! I ordered the features like they were build, but I didn't suppressed the features starting with the last feature. It's a simple solution that once you make the mistake, you'll never make that mistake again.

Using the construction lines is a good idea, I know about it but don't use it as much as I should.  Thanks again!