StephenThor
Mechanical
I'm looking to display a part feature (a machined profile as a revolved cut) in one assembly arrangement and hide it in another arrangement. Is this possible?
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Hide part feature in arrangement
- Thread starter StephenThor
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I'm looking to display a part feature (a machined profile as a revolved cut) in one assembly arrangement and hide it in another arrangement. Is this possible?
multicaduser
Industrial
"Arrangements" in NX are for components. It sounds like you're looking for the Solidworks feature "configurations".
One option in NX is to create an assembly containing all the versions of the part with a corresponding arrangement for each. Another is to create a single part with features that can be suppressed, which can be done several ways. Then when the part is added to an assembly it must be renamed and the correct feature group is suppressed or not as needed. A third way is to wave link the part and delete the unwanted feature. Then again a part family could be created with all the options and the correct part added.
With NX there are many ways to do one thing, maybe someone else has other options.
NX10.0.0.24 MP1/Windows 7 Service Pack 1
One option in NX is to create an assembly containing all the versions of the part with a corresponding arrangement for each. Another is to create a single part with features that can be suppressed, which can be done several ways. Then when the part is added to an assembly it must be renamed and the correct feature group is suppressed or not as needed. A third way is to wave link the part and delete the unwanted feature. Then again a part family could be created with all the options and the correct part added.
With NX there are many ways to do one thing, maybe someone else has other options.
NX10.0.0.24 MP1/Windows 7 Service Pack 1
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StephenThor
Mechanical
Lets try option one. How do I "create an assembly containing all the versions of the part with a corresponding arrangement for each." Do I have to make a copy of the part in order to do that? If so, I'd prefer to keep everything inside of one part file.
multicaduser
Industrial
Here is another way to do this and it's in one file.
1. create the part (say a casting) to the point where it's complete, then extract a body at that point with time stamp enabled and name it say "casting"
2. add another feature, say a milled surface, and extract a body at that point also with time stamp enabled, and cal it "milled surface"
3. add drilled holes for the finished part
4. create a reference set for each of these three solids and add only that solid to it
Then when you add this part to an assembly simply display the proper reference set. There are multiple solids but everything is in one file and all parameters are intact.
NX10.0.0.24 MP1/Windows 7 Service Pack 1
1. create the part (say a casting) to the point where it's complete, then extract a body at that point with time stamp enabled and name it say "casting"
2. add another feature, say a milled surface, and extract a body at that point also with time stamp enabled, and cal it "milled surface"
3. add drilled holes for the finished part
4. create a reference set for each of these three solids and add only that solid to it
Then when you add this part to an assembly simply display the proper reference set. There are multiple solids but everything is in one file and all parameters are intact.
NX10.0.0.24 MP1/Windows 7 Service Pack 1
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StephenThor
Mechanical
That is what I ended up doing and it meets my needs well. Thanks
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