Sketch constrains linking to other parts in assemblies
Sketch constrains linking to other parts in assemblies
(OP)
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
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





RE: Sketch constrains linking to other parts in assemblies
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.
RE: Sketch constrains linking to other parts in assemblies
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?
RE: Sketch constrains linking to other parts in assemblies
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.
RE: Sketch constrains linking to other parts in assemblies