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How to transfer Inheritance Feature Part number

AnthonyC
6-Contributor

How to transfer Inheritance Feature Part number

Hello,

 

What would be the best way to get the inheritance part number into a drawing. 

 

I am using creo with windchill

 

My scenario is that i would like to be able to refer to this in a drawing automatically, i have been trying to see if there was a method with the parameters but when i create the inheritance feature, the file name is the only thing i can refer to, which the file name and PN do not always match. 

1 ACCEPTED SOLUTION

Accepted Solutions

In TEST.PRT create a relation

 

NUMBER = PTC_WM_PART_NUMBER:IID_206

 

where 206 is an ID of the inheritance feature

View solution in original post

10 REPLIES 10
tbraxton
21-Topaz II
(To:AnthonyC)

Refer to the article I posted in this thread. There is a zip file in my first post in that thread you can download and read. It explains how to deal with relations and parameters in the context of what you are doing (excluding any Windchill quirks which it does not address).

 

https://community.ptc.com/t5/3D-Part-Assembly-Design/Inherited-models-with-vardim-dimensions/m-p/802980 

========================================
Involute Development, LLC
Consulting Engineers
Specialists in Creo Parametric
AnthonyC
6-Contributor
(To:tbraxton)

thanks for the fast response. 

You will have to be patience with me, as i am fairly new to Creo.
AnthonyC_0-1673450398891.png

I am unable to add the PTC Part number or the CAD number (which matches the PN) to the varied items field. i assume its something to do with them being locked and auto generated by windchill, as i could pull two values that i create.

I suppose i need to somehow create the relation of the original PN, have that as a parameter in the new/machined PN. 

tbraxton
21-Topaz II
(To:AnthonyC)

If those parameters are Windchill generated and locked, then I would not expect that they would be variable so not a surprise that they are not valid entries for inclusion as a varied item in an inheritance feature. 

 

You should be able to concatenate a string with the master model part number (or another parameter) to create a new part number string for the as machined model. Can you verify that you are able to pass the part number parameter from the master model to the derivative model through the inheritance feature?

========================================
Involute Development, LLC
Consulting Engineers
Specialists in Creo Parametric
AnthonyC
6-Contributor
(To:tbraxton)

yes i was,

 

i followed  ysinitsyn response and it does what i wanted.

In TEST.PRT create a relation

 

NUMBER = PTC_WM_PART_NUMBER:IID_206

 

where 206 is an ID of the inheritance feature

AnthonyC
6-Contributor
(To:YaroslavSin)

thanks! this worked

is the ID always the same or can this vary from part to part?

 

i assume i can rename 'number' to whatever i want to

 


is the ID always the same or can this vary from part to part?

Yes, ID will change from part to part

 

i assume i can rename 'number' to whatever i want to

NUMBER in my example is a model parameter name. You can set any you want.


 

AnthonyC
6-Contributor
(To:YaroslavSin)

thanks for the fast response

 

is there a way to automatically pull this number of the ID?

 

or is it just a manual process? 

 

ID is generated during a feature creation automatically by the system.

I think, if you create a template model with an inheritance feature and will use this template as starting point for new models, changing a source model for the inheritance feature, than the ID will be always the same.

Well, when writing the relation, you can follow this process to "look in" the inherited model for the parameter to pull:

pausob_0-1675031350113.png

The feature ID that identifies inheritance will be "automatically" written into the relation...

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