Long time NX/UG user, new to Creo. In an assembly, If I set a component to "exclude", what does it actually do? What I understand is it sort of "closes" or suppresses it where it isn't visible or uses any memory or resources of the computer. If I exclude a part and then save the assembly, it will not remove the part, right?
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Dumb Creo Question about Representations 1
- Thread starter mwessel
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Representations are lists of operations applied to the master representation.
They have the side effect of freezing components that reference items that are excluded, so that regeneration doesn't fail, even if it probably should.
They also cause excluded parts/components to be skipped during assembly retrieval -if- the simplified rep is opened. If the master rep is opened Creo does not automatically free the excluded parts from memory. Usually there is no benefit to automatic freeing because it is rare to operate on only one rep of an assembly during a session, but the user can manually Erase - Not displayed at any time to clean them out.
The one area that using reps will cause problems is this - if a rep is opened and excluded parts are Erased doing a Save-As Backup will not save the parts required to retrieve the assembly; it will only save the current parts. All is not lost - if the missing parts are added to the Save-As backup directory, the assembly will be OK. I guess if you open exactly that Rep the assembly would also be happy, but as soon as a full regen requires those parts Creo will start looking to retrieve them.
One thing that Reps let the user do is to include Reps defined in lower level parts and assemblies, which can save a lot of memory. There are a few pre-defined reps in every assembly, such as Symbolic (which has no geometry content), which can allow huge numbers of parts to be retrieved. Why would no-geometry parts be good? Creating BOMs.
Best of luck and check out PTC Community.
They have the side effect of freezing components that reference items that are excluded, so that regeneration doesn't fail, even if it probably should.
They also cause excluded parts/components to be skipped during assembly retrieval -if- the simplified rep is opened. If the master rep is opened Creo does not automatically free the excluded parts from memory. Usually there is no benefit to automatic freeing because it is rare to operate on only one rep of an assembly during a session, but the user can manually Erase - Not displayed at any time to clean them out.
The one area that using reps will cause problems is this - if a rep is opened and excluded parts are Erased doing a Save-As Backup will not save the parts required to retrieve the assembly; it will only save the current parts. All is not lost - if the missing parts are added to the Save-As backup directory, the assembly will be OK. I guess if you open exactly that Rep the assembly would also be happy, but as soon as a full regen requires those parts Creo will start looking to retrieve them.
One thing that Reps let the user do is to include Reps defined in lower level parts and assemblies, which can save a lot of memory. There are a few pre-defined reps in every assembly, such as Symbolic (which has no geometry content), which can allow huge numbers of parts to be retrieved. Why would no-geometry parts be good? Creating BOMs.
Best of luck and check out PTC Community.
natepiercy
Mechanical
I describe the "Exclude" state as the happy middle-ground between Hide and Suppress. With Hide, your part disappears from view, but it's still fully present in the model, so (aside from a bit on the rendering end) it doesn't reduce any of the stress on your system. Additionally, a hidden component is still calculated in your mass properties. When you suppress a component, you also end up suppressing the components that reference the original - certainly not always ideal. And then there's Exclude. Excluded components are "considered, but not really there" - see below example.
Say you have an assembly of parts A, B, and C. C is fully and solely constrained to B, and B is fully and solely constrained to A (A is fully defined, say Default).
If you hide B, B disappears from view. A mass properties calculation will still take B into account.
If you suppress B, B and C will both be suppressed. A mass properties calculation will take neither B nor C into account.
If you exclude B, B will disappear from view, while A and C will remain. A mass properties calculation will not take B into account, but will take A and C into account.
Furthermore, if you move A, C will also move, as the empty placeholder of B moves with A, and C moves with the empty placeholder of B (you may need to switch your assembly back to master rep for this to update, though).
Say you have an assembly of parts A, B, and C. C is fully and solely constrained to B, and B is fully and solely constrained to A (A is fully defined, say Default).
If you hide B, B disappears from view. A mass properties calculation will still take B into account.
If you suppress B, B and C will both be suppressed. A mass properties calculation will take neither B nor C into account.
If you exclude B, B will disappear from view, while A and C will remain. A mass properties calculation will not take B into account, but will take A and C into account.
Furthermore, if you move A, C will also move, as the empty placeholder of B moves with A, and C moves with the empty placeholder of B (you may need to switch your assembly back to master rep for this to update, though).
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