Boolean Object Selection Issue - CREO 7.0.4.0

[D_Hale]

I am running CREO Parametric 7.0.4.0 on Windows 10.

I would like to use the boolean cut function to match some mating geometry. I've watched a few videos on how its done and it seems rather simple.

I was having issues so I created 2 cubes and a practice assembly, however when I try and select the geometry to be used as the cut, it will not let me select it.

I do see a feedback message in the bottom left that states: "Reference cannot be uesd due to the scope setting of NONE for Environment."

I could not find an obvious setting in the config to make this adjustment to locally.

Any ideas?

[pausob · Accepted solution]

I'd look in the "reference control" section of the assembly options page of the configuration editor:

If these are configured via a .sup file, you might have to ask your CAD admin for more help...

[D_Hale]

Nice!

That setting was the one. Thankfully I was able to make an adjustment. Will have to add that to my running config.pro tweaks.

Thanks for the quick answer!

[tbraxton]

External ref scope control preventing the component selection.

Setting this config option should resolve the issue.

default_ext_ref_scope

Category: Reference Control

Description: Set default scope for externally referenced models. All - Any model. None - Only current model and children. Skeletons - Any component in model's assembly and higher skeletons on branch. Subassembly - Only components and children in model's assembly.

Values: all, none, subassemblies, skeleton_model

Default Values: all

You should understand the implications of doing this as it is dangerous. In general, I would not invoke boolean operations in assembly mode.

[D_Hale]

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You should understand the implications of doing this as it is dangerous. In general, I would not invoke boolean operations in assembly mode.

Curious as to why that is?

I don't disagree, I'm just wondering...

If I wanted to create a mating part for the bottom of a coke bottle where the geometry is sweeping and complex, this seems like a really useful way of producing that instead of re-building it from a scratch solid.

I can see the advantage of the scratch-solid being discrete and independent geometry references for prints.

Is it for traceable geometry? Or other reasons?

Thanks for the response.

[tbraxton]

Doing this in assembly mode and setting the ref scope control all increases the risk of creating unintended external references and circular references which can make modifying designs very difficult.

An external copy  geometry or merge feature would be preferrable, and you also have multibody modeling available in Creo 7. Any of these methods can be used in part mode with a clear path created to the parent object.