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T
TC_954367510-Marble
10-Marble
February 10, 2025
Solved

SMT_THICKNESS is not updating in multibody after unlink

  • February 10, 2025
  • 2 replies
  • 1395 views

Hi Community!

 

As per https://www.ptc.com/en/support/article/CS416999 in order to be able to modify the sheetmetal parts' thickness easily after creating them, we choose to "Unlink from Part" by default (in our start part). But it seems it solved one problem while created another: The problem is that the SMT_THICKNESS parameter is not updated after altering the model thickness. Therefore extracting the material thickness is not possible now 😕

Is there another parameter we can use in order to display the thickness?

 

Thanks in advance!

-Tibor

Best answer by TC_9543675

Hi Martin thank you for your input,

 

Based on the thread you linked, I was able to find out how to display it on the drawings! The key is here: "If you know upfront how many bodies you need and create them as empty bodies in the start part... "

 

So if the sheetmetal's start part is already "unlinked" then I'll know the body ID upfront (in my screenshot it is -5778) so that I'll be able to reference this in the form:

&SMT_THICKNESS:BID_-5778

With this callout I'm able to retrieve the correct thickness. What's also great in this solution is that it works with legacy sheetmetals as well (we have a lot of sheetmetal parts created in Creo4). Somehow the body ID seems to be always -5778 even if the part is later converted to sheetmetal from an extrude or something.

 

TC_9543675_0-1739270273950.png

 

Thanks!

-Tibor

2 replies

tbraxton
22-Sapphire II
tbraxton22-Sapphire II
22-Sapphire II
February 10, 2025

If you think there is a bug and Creo is not working to specification, then open a case with PTC tech support.

 

What version of Creo are you working in? If you want assistance from the community then post a test case (models) for this problem that you have found so we can investigate the issue.

T
TC_954367510-MarbleAuthor
10-Marble
February 11, 2025

It's not that Creo not working as intended. The intended working is changed with introduction of multibodies. It is in Creo 11.0.2.0

Please take a look at the attached files.

The problem is that after "unlink" the SMT_THICKNESS is not the parts' true thickness (marked with red in the upper left section 1mm vs 5mm)

 

TC_9543675_0-1739257051296.png

 

What parameter can get the true thickness (5mm in this case)?

 

Thanks

-Tibor

M
MartinHanak24-Ruby III
24-Ruby III
February 11, 2025

Hi,

your sheetmetal geometry is included in Body 1. Look at body parameters - you will find SMT_THICKNESS parameter. Unfortunatelly I have no idea how to display this parameter in drawing table.

MartinHanak_0-1739265456527.png

 

M
MartinHanak24-Ruby III
24-Ruby III
February 11, 2025

https://community.ptc.com/t5/Creo-Parametric-Tips/Multibody-How-to-display-use-or-call-out-a-body-parameter-Part-2/ta-p/820592

    T
    TC_954367510-MarbleAuthorAnswer
    10-Marble
    February 11, 2025

    Hi Martin thank you for your input,

     

    Based on the thread you linked, I was able to find out how to display it on the drawings! The key is here: "If you know upfront how many bodies you need and create them as empty bodies in the start part... "

     

    So if the sheetmetal's start part is already "unlinked" then I'll know the body ID upfront (in my screenshot it is -5778) so that I'll be able to reference this in the form:

    &SMT_THICKNESS:BID_-5778

    With this callout I'm able to retrieve the correct thickness. What's also great in this solution is that it works with legacy sheetmetals as well (we have a lot of sheetmetal parts created in Creo4). Somehow the body ID seems to be always -5778 even if the part is later converted to sheetmetal from an extrude or something.

     

    TC_9543675_0-1739270273950.png

     

    Thanks!

    -Tibor

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