Disallow propagation of Assembly Level Cut to Parts

[Pieface]

Is it possible to tell Creo to not propagate to lower level parts assembly level cuts?  I am sure it is, but I cannot locate how.  I am beginning to wonder if this is an issue with Sheet Metal?  The documentation states:

The feature was placed in the Sheet Metal part and no feature exists in the assy? 

I have created a layout for the purpose of displaying dimensional values of material being cut away (threads).  We are using Windchill and I cannot check out the part having the cut out.  I would like to check the assy into Windchill with no relationship/affect to the lower level part.  Have I used the wrong transaction to perform what used to be Intersect?

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[Chris3]

The way that PTC performs assembly level cuts is to create behind the scenes family tables and turn those features off at the part level and then on at the assembly level. Unchecking "Automatic Update" only stops it from creating family tables in every part. It still creates them in the ones that you select after you uncheck that box.

You never see this unless there is a bug that exposes it (which has only happen to me a couple of times).

If possible stay way from assembly level cuts. They can cause huge performance hits with large assemblies.

[Pieface]

Thanks for replying Chris,

     I had seen in the part I could choose "Automatic/Manual/No dependency":

This only has to do with how the feature updates.  My recollection is Pro/E or Wildfire would allow assembly level intersections to be assembly level only or assy and part level.  Has Creo lost this capability or am I mistaken on previous functionality?

[Kevin]

I think what you are showing to is a little different than an assembly cut feature. You specify the level at which the feature is to show on the intersect tab of the assembly cut definition.

[MartinHanak]

Hi,

I think you understand that Inheritance Cut is quite different feature than Assembly Cut. If you apply Inheritance feature then you are telling Creo that you want to propagate geometry of reference part into target part.

Probable solution ... delete Inheritance Cut and create Assembly Cut.

MH

[Pieface]

Thanks to everyone for replying.  The original cut was made with Component Operations>Cut Out.  Strangely, the part receiving the cut out had the feature placed in its Model Tree.  The feature was not shown in the assembly Model Tree.  I have been away from Creo for years and am playing catch-up.  Previously there was an Intersect Feature whose propagation could be controlled.  In other words I could tell Wildfire to only display the intersect at the assembly level and not the part.  I am unable to find that process/function in Creo.  We got the answers we were looking for but could not save them for future reference because I could not check out the part.