Concentric alignment in part not assembly.

[vnet]

Hi, is there a way to align in a concentric way one body to another inside of a part not an assembly.
What I want to align to is not in the common xyz direction it is angled.
Once aligned how do I move the part in the direction of the angled axis that I just aligned to, meaning distance.

Thanks,Buddy.

 

[mmauldin]

I think I understand what you asking, but I'm not sure.
Attached is an example of using move face (align axis to vector) to orient the body and then using move face (point to point) to move the body to a reference geometry that controls the distance. If you want a 0 distance, the point to point could reference the end face of the second body.

 

[SDETERS]

ctrL T Or try move object. Have looked into this? Just a quick thought.

 

[vnet]

Yes I know about move or ctrl T.If I have a simple 3" block and one hole drilled into the block at some very strange angle and I import a part that is a shaft the same size as the hole, then how can I align the shaft to the hole in a concentric way, not in an assembly.

Thanks, Buddy.

 

[multicaduser]

Would direct editing features like "make coaxial" and "linear dimension" work?

NX 12.0.1.7 Windows 10

 

[vnet]

I made a block and drilled a hole then imported the shaft part and aligned with synchronous make coaxial then created an axis.
How to move shaft in direction of axis?
Also when two bodies are in the same part and you use synchronous methods from one face of one body to the next face of another body how do you drag the rest of the faces with the move.

Thanks Buddy.

 

[mmauldin]

Do you need an exact position?

If not, you can use synchronous modeling>move face linear and drag into position.

If you do, create a datum plane perpendicular to the hole at the desired position and use move face linear. Use measure distance to get the distance from the cylinder face to the datum plane for your move distance.

 

[vnet]

Thanks, All this should work decent.Is there a way to make these two same moves with the move command.
If you think about it I am using synchronous methods to move an object not edit it's geometry.
Thanks, Buddy.

 

[jerry1423]

What I would do (since the hole is where you want it relative to the shaft) is
[li]Remove the Parameters of both bodies[/li]
[li]Break them into two separate components[/li]
[li]Bring them together using assembly constraints[/li]
Let us know if you need instructions removing the parameters, and breaking them into two separate components.
Since you are working syncronous, removing the parameters won't affect anything, but the two solid bodies won't be linked together

Jerry J.
UGV5-NX1884

 

[vnet]

Yes, I would say that is the easy solution however,if you look at the original post,I want a solution for part only,I already have two "dumb" bodies.
One of them was imported as a part,in the normal xyz position,and then moved with synnchronous methods coaxial and linear direction.
If I were on the board of NX I would say why not add these types of "Moves" to the move command instead of trying to use synchronous methods which I usually attribute to single body geometry edits,or one face of a dumb body that I am referencing to another dumb body.
Why as a work around should I have to create an assembly and then what,save as a single part just so I can make those two moves.
Let's say I make an assembly and do the two moves through mate relations,this is unrelated but can I save or export everything in an assembly as one part?

Thanks,Buddy

 

[PSI-CAD]

Hi,
If uou can loose parameters, you can export to parasolid file on solid and the other to another parasolid file.
Then create a new part and import both parasolid files.

Regards
Didier Psaltopoulos

http://www.psi-cad.fr

 

[Arkance/PhoeNX]

If you've got dumb bodies, transform would do what you're after.

See attached video.

Anthony Galante
Senior Support Engineer


NX4 to NX CR with almost every MR (18versions)

 

[vnet]

Nice,I thought there was a way to make those moves.
I work with dumb bodies all the time.

Buddy.