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mneumueller18-Opal
18-Opal
May 7, 2021

Multibody - How to display, use or call-out a body parameter – Part 2 (new in Creo 8.0)

  • May 7, 2021
  • 4 replies
  • 22183 views

Hello everyone and welcome back to the multibody blog series. This post also attempts to answer another body parameter related question:

How can I display call-out a body parameter in a generic way?

We received a question and enhancement idea from customers adopting Creo 7.0 asking for Leader Note Callouts for Bodies, similar to existing notations available for models, features etc as described in the Creo help here.
(in short: Previously, when attaching a leader note to a model (component) you can get the value of a specific parameter for the attachment model. This can be achieved with the following syntax: &<param_name>:att_mdl  e.g &BOM_PART_NO:att_mdl)

 

An analogue workflow is now supported for body parameters. We implemented and added this to Creo 8.0. This enhancement allows you to call out the values of body parameters into a leader note that is attached to that body.

To call out the value of a specific body parameter, you need to use the following syntax inside the leader note that is attached to that body:

&<body-parameter-name>:att_body

For example, if you have a body parameter called Description, you could create a leader note with the callout &Description:att_body  or call out the body’s material using &PTC_ASSIGNED_MATERIAL:att_body

 

When you create a leader note with this syntax, Creo Parametric checks the body to which the note leader is attached. If the called parameter exists for that body, then the body parameter gets evaluated and the parameter value is shown in the note.

In the case of an assembly, Creo Parametric looks for the called parameter in the body of the component to which the note is attached.

The callout is supported for all the environments and modes that already support :att_mdl.

 

Example:

All bodies have a DESCRIPTION parameter called out using &Description:att_body 

image

 

 

Thanks for reading. I hope it was informative.

 

Back to Creo 7.0 & 8.0 Multibody Home: Start Here!

 

Enjoy!....Martin

    4 replies

    M
    mstols7-Bedrock
    7-Bedrock
    July 27, 2021

    Thank you Martin really good tip.

     

    What about calling parameter information inside the material itself in a note? Can you show the user defined parameter information inside the material, that has been assigned to a body in a note?

     

    For normal parts we can create a relation [material_param("PARAMETER","MATERIAL")] in the template that will pull the material parameter information and and show it in a note. But we cannot do this for bodies in a start part.

     

    Any suggested workarounds?

    M
    mneumueller18-OpalAuthor
    18-Opal
    November 4, 2021

    Hi,

    not sure what exactly you are after. 

    Are you talking about start-parts for multi-material models with pre-defined bodies ? 

    Would the association of materials to these bodies also be pre-defined?

    can you elaborate on your intent , what are you trying to achieve?

    O
    OlssonOlsson7-Bedrock
    7-Bedrock
    March 7, 2024

    I have the same problem as @mstols mentioned.

     

    If you could help @mneumueller  this would greatly help.
    I'd like a startpart ready for single/multibody. Building on the old startpart logic, i'd like to be able to pull material names in with a "clean" description.

    for 1 body i'd like the resulting string in the value field to be
    GALVANIZED STEEL (not galvanized_steel)

     

    for a multibody i think I need to work with table repeat regions instead, to look something like this:
     

     

     (User defined body name)(PTC_CONDITION)(... any material file parameter)
    layer 1 Cool green material...
    layer 2Super blue material...

     


    Picture1.JPG

    M
    mneumueller18-OpalAuthor
    18-Opal
    March 7, 2024

    Unfortunately that is not that straight-forward as there is no relation support within bodies.

    Otherwise you could have just created a body relation to call  the above function.

     

    So, currently not really supported.

    But: If you know upfront how many bodies you need and create them as empty bodies in the start part (so you have their Body IDs) you could of course create part-level relations

    MATERIAL_1=material_param("PTC_MATERIAL_DESCRIPTION",PTC_ASSIGNED_MATERIAL:BID_-5778)

    MATERIAL_2=material_param("PTC_MATERIAL_DESCRIPTION",PTC_ASSIGNED_MATERIAL:BID_xxxx)

    ...

    and then assign a parameter to each body holding 

    body 1:   MY_MATERIAL = MATERIAL_1

    body 2: MY_MATERIAL = MATERIAL_2

    ...

    and then call out the body parameter &MY_MATERIAL:BID_xxxx

    But yes, this is limited to situations where you create the required bodies as empty bodies upfront in your start part.

    O
    OlssonOlsson7-Bedrock
    7-Bedrock
    March 7, 2024

    Hey thank you @mneumueller for the quick reply.

     

    I think the workaround is useful! The start part can also aid as a guide for the user and just be populated with sample bodies.

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