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Design configuration in NX

Design configuration in NX

Design configuration in NX

Hi folks,
I am back with a query.I just want to know the design configuration concept in NX. I got this query from one of my friends. So please correct me if I am wrong.Basically the requirement is to call the same feature into multiple files(similar to UDF) and suppress the unwanted features and retain the required features from the model.Quite similar to maintaining various configurations of the same design.Hope it is clear for the experts.

RE: Design configuration in NX

It sounds like you are describing a "part family". Look it up in the NX help files to see if it meets your need.


RE: Design configuration in NX

Yes as mentioned by cowski, You can suppress the required feature(s) using part family approach.

RE: Design configuration in NX

If you're talking about the configuration feature as in solidworks, John Baker outlined ways to control feature suppression through part attributes. I do this all the time using list attributes where you can choose an option which will supress the proper features or control feature sizes. This, of course, is not a udf feature added to an existing file but a separate part file which can be cloned and modified with a set list of options. It has advantages over part families in that it is a single file but is more difficult to set up. Your question is a little confusing to me in that it seems to be asking for something that isn't available in any cad program I'm familiar with.

NX Windows 10

RE: Design configuration in NX

Hi all,

I'm in the same case than sudhakarn.
@multicaduser : I'm interested about the solution from John Baker. Do you know where I can found the explications about it?

Thanks ahead.

RE: Design configuration in NX

Let me try to explain. The following is for NX11 but is similar to NX10 and previous versions.

1. File->Utilities->Attribute Templates
Enter an "Attribute Title"
Select "data Type" as "Number"
Change "Constraint Type" to "List"
Enter a list of numbers, say 1 through 9 each on a single line followed by enter.
Pick "OK" to finish.

2. File->Properties->Attributes tab
Locate the "Attribute Title". If no category was specified it will be in "<No Category>".
Pick the down arrow in the box to show the list typed in the "Attribute Template" dialog and pick one.
Pick "OK" to exit the "Properties" dialog.

3. Open the Expression dialog
Under the "Formula" column right click in the box and pick "Edit". Remember the NX10 dialog and earlier will be slightly different here.
In the "Edit Formula" dialog pick "Reference Part Attribute".
The "Attributes" dialog will pop up, pick the attribute entered in the "Attribute Template" dialog, the pick "OK"
In the "Edit Formula" dialog pick "OK"
Make sure "Attribute Expressions" is picked for the filter in the "Expression" dialog. The "p" number will be there in blue. My preference is to rename the "p" number and discard the expression being edited.

The expression can then be used to drive feature sizes.

This also works in reverse. I use string expressions, conditionals and concatenation to build strings which can be referenced by part attributes used in the bill of materials. If I get a little time to knock together an example I'll post it.

NX Windows 10

RE: Design configuration in NX

Hi Folks,
Thanks a ton for all your replies and ideas. Will check it out.

RE: Design configuration in NX

Thanks for your answer.

But my question is more complexe.
I would like to create an assembly with some arrangements. My assembly will be reprensented at 2 "states" : one state with all internal machinings and another one without internal machinings. So I think manage them with the arrangements.
So if I go to one of the parts, I need to create 2 states too who will be used on the assembly.
Do you know how I can create and manage it please? Knowing that I don't want to save these states in TeamCenter, so I can't use the part family.

Thanks ahead.

RE: Design configuration in NX

have you looked int the possibilities with reference sets?
We use that extensively when dealing with sheetmetal parts that are later machined.

RE: Design configuration in NX

For what you are mentioning we control this with Wave Links. It could also be done using promotions. So we would manage two different item #s. The Raw Material item# and the Machine item#. Hopefully this may help.

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