[Creo 7.0] Is there a way to retreive a part parameter by its name is assembly drawing?

[AD_10765291]

Hello All,

I have a an multiple assemblies which contains part with same name but different parameters. Is there a way to retrieve the parts parameter by its name.

For example:
My assembly has p1.prt, p2.prt and p3.prt. They all have a parameter weight.
In drawing I want to do something like this "&weight:p1.prt".

Is there a way to do this?

[tbraxton]

Yes, this is possible. It can be realized through the use of the session id of the parts.

The syntax when using the parameter in a note is as follows: "&PARAMETER:session id # "

Where # is replaced by the session id (0,1,2.....) for the model containing the parameter of interest.

To find the session ID of a model, use the following: Tools > Relations > Show > Session ID

Using a Session ID of a Component in Assembly Relations (ptc.com)

[AD_10765291]

Is there a way to use part name? Because the session id will change in different assemblies but the part name will remain same.

[tbraxton]

If you are looking to list the part with the weights on the drawing, then the method shown by @StephenW is easier than using session id. You may be able to save that table or place it in a drawing template so that it will automatically populate the cells. I do not believe that you can predefine values in a repeat region so you may get more info than what you need with this method (weights for all  parts that have the parameter).

[AD_10765291]

I used weight for an example but there are some other parameters that I want show using notes. I need to show these notes near the part view in the assembly drawing.

[tbraxton]

You could try creating an annotation note(s) in the parts and then show those notes on the top-level assembly drawing. I have not tested this, but it might work for your scenario. If that fails in the context of only having the assembly model driving the top-level drawing then you can create a separate drawing for each part as needed and insert that sheet into any other drawing, this will bypass the use of session id in the assembly drawing.

[StephenW]

Easiest way to get part parameters to an assembly drawing is via a repeat region table.

I use the system parameter for weight (pro_mp_mass) and a part paramter (description1) for the description in the example below

[AD_10765291]

I actually need to use it in notes. I can't use it with tables.
Is there a way to do something similar in notes?

[pausob]

Not sure if this helps, but if you are doing this in a drawing, then try attaching a leader note with this type of text:

&PARAMETER:att_mdl

This will display the value of PARAMETER from the model to which the note is attached...

You can also call out parameters that belong to body, edges, etc... See this System Parameters for Drawings help page.

If you don't want that leader line, then I think you have to use session ID to get at the part parameter of the particular assembly component.

[MartinHanak]

Hi,

you can:

• add p1.prt as second drawing model
• set p1.prt as active drawing model
• create note containing &weight
• set assembly as active drawing model