having a problem replacing a part family in assembly

[aluminum2]

I created a part family named model 1. I made another assembly and brought in model 1. Chose my part in the family called part 1. I try to right click to replace component with model 1 and select model 2. I get the error message failure to load part.

Is there something else I have to do with the part family file. I would like to change from one part of the family to another without having to delete the original and bring in a new one. Kind of defeats the purpose if I cant.

 

[cowski]

If all you want to do is switch between 2 versions of a part within the same assembly, you should look into arrangements. With arrangements you would add both parts to the assembly and in arrangement 1 suppress component A, and in arrangement 2 suppress component B.

 

[aluminum2]

The reason why family of parts, to me, would be effective is because you only have to work on one part. Like add dimensions, drafting, or assembly constraints to one. If you have two instances, wouldn't you have to do everything twice?

 

[cowski]

When you generate parts from the family table, each member is an individual part file. You can't switch out family parts 'on the fly' so to speak.

What do you have and what exactly are you trying to accomplish? This forum has a lot of members, I'm sure someone here has done something similar and will be able to give a preferred workflow or tips/tricks.

 

[JohnRBaker]

To start with, what version of NX are you using as we've made some changes recently?

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

http://www.siemens.com/plm

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[aluminum2]

I am running NX6

I would like to be able to switch from one part in the family to another and have all of the mates be the same. If I do drafting, I would like not to have to re-link my dimensions. If I want to use a variation of the part in an assembly, I would like to switch to it without doing any updating myself.

 

[looslib]

What is the reason for switching one family memeber for another?

If you have a bolt (memeber1) in an assembly and find it too short, you can switch/substitute another bolt (member2) and maintain the relations and annotations in your drawing. The reason they maintain is becasue they were created from the 'same' master file.



"Wildfires are dangerous, hard to control, and economically catastrophic."

Ben Loosli

 

[JohnRBaker]

OK, what you need to do is change your Assembly Load Options so that you include in your list of Search Folders the location of where your Part Family master template files are stored. This way, the system will automatically find the Master Template and it will be the one offered as the replacement which will then allow you to select a new family member.

As for maintaining your current Assembly Constraints, as long as in the Replace Component dialog you have the Settings option 'Maintain Relationships' toggled ON, you shouldn't have any problems if you actually replace one family member with another. Even if you were to manually choose a different Master Template, for example replacing a Hex Head Cap Screw with a Socket Head Cap Screw, as long as the 'mating' faces/edge were given common user defined names (which is the case with the NX Reuse library parts) you can perform the same replacement without losing Constraints.

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

http://www.siemens.com/plm

UG/NX Museum:

http://www.plmworld.org/p/cm/ld/fid=209

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