How to setup predefined mates???? 1

[AaronH]

All,

When I insert a library part (let's say a fastener) it gives me a list of predefined mates to choose from for orienting the part. I want to include this functionality with library parts that I model. However, I can't seem to figure out what it's called in NX. Solidworks calls it "Mate References". Can someone tell me what NX calls it so that I can figure out how to do it? I've been through the doccumentation and so far haven't been able to find it, but I know it's there (somewhere).

Thanks in advance,
Aaron

 

[JohnRBaker]

What version of NX are you running, and if it's NX 5.0 or later, are you using Mating Conditions or Assembly Constraints?

John R. Baker, P.E.
Product 'Evangelist'
Product Design Solutions
Siemens PLM Software Inc.
Industry Sector
Cypress, CA

http://www.siemens.com/plm

http://www.plmworld.org/museum/

To an Engineer, the glass is twice as big as it needs to be.

 

[AaronH]

Ahh... I knew I forgot a piece of vital information... NX 4.0 mating conditions.

 

[JohnRBaker]

OK, first create your model as a Part Family file. Then add this part (the actual Part Family master part, NOT one of its member parts) to a typical assembly and mate it like you would expect it to be normally mated. Now with the Mating Conditions dialog open, go up to the 'Navigator' section and select the item with the names (not the mates) of the two parts being mated, press MB3 and select Remember Constraints (it should be the last item on the list of options). You'll get a message indicating that the constraints have been recorded so just hit OK and continue. Now after this is completed you MUST save your new Part Family master file (you don't have to save the Assembly since the data that is needed has already been moved to the master part file).

Now when you drag your Master Part Family template into an assembly and after you've selected the family member you wish to create, the system will then ask you to select only the necessary references in the assembly to properly Mate the Component.

And that's about it.

John R. Baker, P.E.
Product 'Evangelist'
Product Design Solutions
Siemens PLM Software Inc.
Industry Sector
Cypress, CA

http://www.siemens.com/plm

http://www.plmworld.org/museum/

To an Engineer, the glass is twice as big as it needs to be.

 

[AaronH]

It's got to be done using part families? Seems like an aweful lot of effort for something so simple. I really wasn't planning on creating a family of the parts. I just have to insert a fair number of the same part and would like to make mating a bit easier/faster. Solidworks will let you create mate references for any part super easy. Not so with NX?

Thanks,
Aaron

 

[JohnRBaker]

No, it does NOT need to be done using Part Families, but when you said that you wished to create your own Library Parts, I guess I automatically thought of a Family of Parts.

Anyway, you can do this same thing with ANY model which you wish to add as a Component to an Assembly, following the procedure I outlines above.

John R. Baker, P.E.
Product 'Evangelist'
Product Design Solutions
Siemens PLM Software Inc.
Industry Sector
Cypress, CA

http://www.siemens.com/plm

http://www.plmworld.org/museum/

To an Engineer, the glass is twice as big as it needs to be.

 

[AaronH]

Nice!! Worked as described. Thanks very much. Is there a way to remove those predefined constraints from the part file if one ever wanted to do so and/or can they be overwritten simply by peforming the Remember Constraints option again?

Aaron

 

[JohnRBaker]

You have to go back and repeat the process to make any changes.

John R. Baker, P.E.
Product 'Evangelist'
Product Design Solutions
Siemens PLM Software Inc.
Industry Sector
Cypress, CA

http://www.siemens.com/plm

http://www.plmworld.org/museum/

To an Engineer, the glass is twice as big as it needs to be.