Sketch constrains linking to other parts in assemblies 1

[CATPart]

Hi,

I come from intensive Catia V5 usage, and now I'm working as a consultant in company that uses NX 8.5. The problem
is that here there is no that one guy who is expert, so I don't have somebody to ask.

I'm a bit confused with constrains when making a sketch, sometimes I can constrain geometry to other sketches in assembly and
sometimes not, sometimes I can't even constrain to the sketches within the same part.

Please for help or link to some document that explains this, I don't have time to search the net because there is a deadline
to meet.

Regards,
DG

 

[SvenBom]

I guess that you didn't set the Selection Scope correctly. In that menu, you have three options:
entire assembly: you can select asssembly geometry
within work part only: you can select geoemtry of the work part. No other parts/geoemtry of the same assembly will be selected
within active sketch only: only the geometry of the current active sketch can be selected.

I have attached the image of this menu, so that you can find it easier.

 

[CATPart]

Thanks, but one more question... when I enter the sketch for editing, selection scope is set to ENTIRE ASSEMBLY, but as soon I click geometric constrains command I have only two options "Within work part only" and "Within active sketch"?

I am making one welded construction, my goal is to have one master model with sketch that defines positions and main dimensions, and that each plate is in separate file linked to the position in master model.

Any suggestions, or there are better ways designing welded constructions?

 

[SvenBom]

For creating an interpart link, maybe you should consider using a WAVE Geometry Linker. With this command, you can link curves, sketches, faces or entire bodies from one part into work part.
Also, when you set the Selection Scope to Entire Assembly, you can activate Create Interpart Link command. The icon for this command is on the right side of Selection Scope. Using this command, NX Will create a WAVE Link instead of you.
And for creating weldments, there is an application deticated to weld operation (insert/weld assistant). But you need a special license for weldment.

Also, you can create weld on the assembly level using WAVE links. You can copy all the neccessary faces from the part to the assembly level with wave links and then construct the welds.
Then there you have also Promote Body command, which copies the selected body to the assembly level. Again, you can use this for weldments. But if I remember correctly, the promote body is the old way of doing this and WAVE linking is the new way of making such copies.

And about geometric constraints. What you can do is first projecting the assembly lines to the active sketch with Project Curve command. Make sure, that under the Settings section you have Associative turned on. Then, use those projected curves when placing the geometric constraints.

 

[CATPart]

Thanks, I will check it...