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Missing definitions in imported assembly and not movable geometries

Experimenter
Experimenter

Hello all,

I am working with NX MCD only a couple of days now and have some basic questions I could not figure out by myself until now. I am working on a simulation of an assembly, which was created in Solid Works and was saved as Parasolid. Because some components were missing when importing the whole assembly, I try to import them now afterwards.

My question now is how to import assemblies without loosing the connections between the parts. When opening a Parasolid in NX all the definitions are gone, which makes it pretty hard to move them around and define their position in the room. I only need these assemblies for visualization, so that their parts do not need to move separately. Is there an option in NX to define an assembly as a dead body?

On the other hand I was wondering why some assemblies do not show up in the assembly navigator and cannot be moved at all because they seem to be treated as parts. Why is it not possible to move simple geometry parts like assemblies?

Thanks for any help!

3 REPLIES

Re: Missing definitions in imported assembly and not movable geometries

Siemens Legend Siemens Legend
Siemens Legend

Hello ML_KE and welcome to the PLM Community,

 

it seems these are more general NX Questions rather than MCD.


ML_KE wrote:

 

My question now is how to import assemblies without loosing the connections between the parts. When opening a Parasolid in NX all the definitions are gone, which makes it pretty hard to move them around and define their position in the room. I only need these assemblies for visualization, so that their parts do not need to move separately. Is there an option in NX to define an assembly as a dead body?

If I understand you correctly there are multiple possibilities here depending on what you want to achieve:

If your assembly or subassembly is a collection of single Parts (e.g. because the imported elements from Solid Works are multibody parts) then you can create an NX Assembly of the selected Parts and afterwards move the new assembly as a whole.

ugraf_2017-10-23_08-43-38.pngugraf_2017-10-23_08-44-58.png

 

You can also make a linked copy of the solid bodies to another part with the "Wave Geometry Linker" command (it can be associative or not associative to the input bodies:

ugraf_2017-10-23_08-49-30.png

 


ML_KE wrote:

On the other hand I was wondering why some assemblies do not show up in the assembly navigator and cannot be moved at all because they seem to be treated as parts. Why is it not possible to move simple geometry parts like assemblies?


I assume with simple geometry parts you mean the solid bodies inside of the parts? If that is the case, then you could move them by setting the according Part as workpart or displayed part (to work in context of the part) and using the Move Object (ctrl+t) command.

 

Also If you going to do this quite often and want to stay true to the input files (and maybe maintain a link to them), then I would also suggest to use another exchange format: JT.

Because NX is capable to maintain the link to the input JT Files, you can modify your assembly and then update it more conveniently inside NX/MCD.

JT would also maintain your input assembly structure.

 

 

I would also suggest to attend an NX Training If you have the possibility to do so (depending on what region you are coming from there might be also some local options), especially since you just started in working with NX/MCD a couple of days ago.

 

I hope this could help already.

Best regards

Viktor

Re: Missing definitions in imported assembly and not movable geometries

Solution Partner Phenom Solution Partner Phenom
Solution Partner Phenom
If you use a bond constrain in assembly you can define components that are moving to better without constraining every single component

Ruud van den Brand
Pre-sales NX CAD
cards PLM Solutions

Re: Missing definitions in imported assembly and not movable geometries

Experimenter
Experimenter

The "Create New"-Option helped a lot with all of my problems. Now I can define the position of my new assembly within my original assembly by using constraints and it does not get torn apart. Smiley Happy The bond constrain also worked fine, I don`t know why I did not find that earlier when searching in the constrain options.

 

My other problem also got solved by creating new items of my solid bodys. They now show up in my assembly navigator and can be moved within the original assembly by using constrains. When moving the parts as workparts I could not place them in exact positions, so that the required precision was missing.

 

Thank you very much for your help!