iPart half suppressed sketch won't suppress for some reason

[Hunteil]

I have an iPart (with family table) in Sheet Metal. I'm making a right and left hand version and I've made these many times except this has an angle so that means my center locations can't rely on the origin planes... Anyways I created a cut and suppressed it in the table... it suppresses but the sketch for some reason will not suppress with it causing sketch doctor to complain. Why can't I turn this sketch off? You can see the error is caused b/c the projected geometry is missing from the original right hand variant that is off atm. This is to be expected, which is why I'm trying to suppress the cut feature w/it's sketch. 

See attached image

Also I have another cut feature in my document that I suppress and Compute and it's sketch suppresses automatically.

using 2022.1.1

[S_May]

@Hunteil 

please upload a pattern IPT.

[Hunteil]

Attached.

Cut7 is the cut I'm testing on this version.

Picking member2 will cause it.

[Hunteil · Accepted solution]

So as far as getting a left or right hand of the sheet metal part. I have a solution. Use Mirror and pick "Mirror Solid" And "Remove Original" and pick the plane you need. Then in the Table, add the Mirror and Suppress Compute it as needed. I have forgotten about the Mirror Solid tool. This helps a ton I hope this helps others unaware as well. Thank you.

So the original issue is useless now.

[johnsonshiue]

Hi! I suspect this is related to soft dependency vs hard dependency. The sketch was not fully "suppressed" due to the fact that it was not fully dependent on the source geometry. The dependency was probably only on an edge to help define the sketch coordinate system. This means if the source geometry isn't available, the sketch can still compute (though with limited associativity).

Please feel free to share an example here. I would like to understand the behavior better and see if my suspicion was right.

Many thanks!

[Hunteil]

@johnsonshiue 

The example was uploaded in an above reply.

[mluterman]

I'm doing this all the time. See below. go to the "Other" tab in your iPart table. In the right-hand pane, where it says "Click here to add value"-that's where you enter the sketch (exactly, verbatim as shown in the Browser tree, i.e. Sketch16 with capital and no spaces, like Browser tree). Then, once you accept it, it adds it to the list below and you change each iPart instance to "Suppress" or "Compute".