NX unite command issue - tool and target do not form complete intersection

[Atharva_Mechanical]

Hi Everyone,

I am trying to unite a body in the assembly I have and I keep running into this error - tool and target do not form complete intersection...

Details -
In the screenshot you can see the model I am working with. Funny thing is that this is a part file and not assembly (parts are made by multiple bodies, as shown in SS for the part navigator tree). I am trying to group / combine relevant bodies so that I may save them as a part with proper name, that way the bigger assembly I am working on would make sense for the next person who works on it. In tis case, I want to create two bodies, fence and machine.
For this, I am using Unite command. While executing this command I keep running into this error. I am guessing the tool and target are not touching so this keeps happening. Is there any way around it? Some other command may be?

I am really looking for a command which will work as blanket operation which will reduce my work. This will potentially be useful in other cases where I am dealing with even larger assemblies.

Thanks
Atharva D

 

[cowski]

In this case, I want to create two bodies, fence and machine.

Rather than uniting everything into 2 bodies, I'd suggest using feature groups to gather the fence bodies into one group and the machine bodies into another group. Name each of the feature groups appropriately.

Also note that you can rename individual features in the part navigator to help quickly identify one body from another.

I am trying to group / combine relevant bodies so that I may save them as a part with proper name, that way the bigger assembly I am working on would make sense for the next person who works on it.

You do not have to group the bodies before saving them to another file. You can use File -> export -> part... to export multiple bodies to a new part. Or, if you want the currently displayed part to be your assembly, you can use the "new component" command, then select the bodies you want in the new component. This will create a new part file, add the selected bodies to it and add it to the display part as a component. This can be a quick way to build up an assembly from individual bodies like what you have.

www.nxjournaling.com

 

[Bleaker]

The red dot tells you where the problem is, most likely some sort of distance tolerance issue. You can sometimes "fix" it by twiddling the tolerance value, but a lot of the time it's some sort of geometry problem that you might want to address before this thing is created IRL.

 

[Toost]

Why the Unite ?
As Cowski mentions, Use the "Create new Component, select all bodies for the fence, tick the delete originals and you have moved all these bodies to a new file.
As you have noticed , NX does not care if "1 partfile" contains 1 single solid body or multiple. Other systems might "bother" about this.
There is nothing wrong in having multiple solids in the same file, NX has been working this way since the introduction of solid modeling in NX ( way back in the 80:ies)

I see only one reason and that would be if you are trying to hide from a customer how a machine is designed internally. Then i would like to unite all up and delete internal features.

Regards, Tomas

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