How to prevent the sheet bodies being automaticaly added to the "Model" Reference set ?

[stephlouv]

There is a "Model" reference set coming with new model files.
Component and solid bodies are automaticaly added to it, that's fine.
But in my case, sheet bodies are also added but we don't want that.

We don't need the sheet bodies but we are using them often (Linked face) to model weldings.
And we then must always remove them afterward. Annoing and counter productive.

Thanks in advance


"My english is bad ? That's why i'am french."

 

[cowski]

For NX 7.5 or higher:

File -> utilities -> customer defaults -> Assemblies -> site standards -> reference sets -> change option to "solids priority". Save the settings and restart NX for the change to take effect. Moving forward, only solids will be automatically added to the reference set (unless there are no solids and only sheet bodies in your file).

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[JohnRBaker]

To control what gets added automatically to the Model Reference Set go to...

Customer Defaults -> Assemblies -> Site Standards -> Reference Sets

...and check to make sure that the 'Contents' option is set to 'Solids Priority'. Now this does NOT mean that only Solid bodies will be included in the Model Reference Set just that if there IS a Solid body it will be included and the Sheeet bodies will not. Now if there are ONLY Sheet bodies then they WILL be included since NX assumes that THEY are the 'model', but if at least one Solid body is present IT will be what gets added to the Model Reference Set.

Now as for your comment that 'Components' are also being included in your Model Reference Sets, unless there is some specific reason why you want this to happen, we would recommend that you NOT use Reference Sets to control the content of an Assembly. This is considered a poor practice and is generally avoided. This is why there is an additional option in the above Customer Default location to control this and it should NOT be toggled ON.

John R. Baker, P.E.
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Product Engineering Software
Siemens PLM Software Inc.
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Cypress, CA
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[stephlouv]

Perfect !
Many thanks.

"My english is bad ? That's why i'am french."

 

[cowski]

The 'solids priority' option mentioned above works on geometry created within the part file itself. When you start wave linking geometry into your file, it will be added to the current reference set. You will have to remove these later if desired (either manually or by way of a journal).
thread561-344591

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[jerry1423]

Delete the Model reference set in the model file, then recreate it with add components automatically unchecked.
It's probably best if you do this with all of the (assembly and drawing) files that it is used in not open.
You will then have to add bodies to this reference set manually from this point forward.

 

[stephlouv]

@cowski.
I see there is a check box also for "include WAVE Linked Bodies".
We will uncheck it as we have welding models starting from this function.

@J.R.
I've well understood why RefSet must not be used at assembly levels.

"My english is bad ? That's why i'am french."