Using coordinates to to mate to the assembly in NX8.5

[dgberry]

I am new to NX8.5. Years ago I used NX3. I've also used most cad programs except for Catia.

My question is this; When creating a new assembly and then inserting a part into it, I want to use the assembly coordinates and have the part constrained to it.

 

[JohnRBaker]

Not a problem. First make sure that there is a Coordinate System in both the Component part file and the empty Assembly. In the Component part file, either add the Coordinate system to the Model Reference set or better yet just use the 'Entire Part' Reference Set when adding the Component to the assembly. OK, now when adding the Component to the Assembly, if you're using the 'By Constraints' Positioning option, when the Constraint dialog comes up, set the Type to 'Touch Align' and the Orientation method to 'Align'. Now in the preview window of the Component, using QuickPick, select the 'Coordinate System' in the Component part and then select the 'Coordinate System' in the Assembly part file and hit OK and the Component will now be Constrained CSYS to CSYS.

Anyway, give it a shot.

John R. Baker, P.E.
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[looslib]

You just want to position the component by an offset value from the initial XYZ dataum planes? That is possible but loses the value of the assembly constraint routines. Alot would depend on how complex your assembly is, too. I would not want to do that for a car or an aircraft, but a mold might be doable.
You can also create additional datum planes in relation to the initial ones to mate your components against. This may work better if you have a component at an angle from the main datums.
I found it best to position my initial component to the datum planes then mate additional components to either surfaces on a prior component or additional datum planes.


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Ben Loosli

 

[dgberry]

John,

That worked, except that I changed it to "Pref Touch". It then moved right to the point.

Thanks

Dan