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CREO 5; Piping; where is the length of a pipe stored?

wbottis
12-Amethyst

CREO 5; Piping; where is the length of a pipe stored?

Hello, can someone tell me what the parameter is called where the length of a pipe is stored?  I'd like to reference this in a drawing table so there is a link between the drawing and the pipe?  Thanks.

7 REPLIES 7

Hello,

 

For a non-solidified pipe, you can select "Piping Info" and change the Definition dropdown to Segment. From there, by selecting Info at the bottom you can see the length.

 

For solid pipes segments, the two parameter names are "LENGTH_CENTER" and "LENGTH_PRE_CUT" that you call out in 2D drawings.

 

Cheers,

John Piotrowski, Co-Founder & Product Manager
CadActive Technologies - www.cadactive.com

What is the difference between "non-solidified" and "solidified" pipes?  I am trying to apply this to a flexible pipe.  Upon creating a note in the associated drawing and entering '&LENGTH_CENTER', the pipe length does not appear.

Before they are solidified, pipes in Creo are just features, not solid geometry. By solidifying pipes, you create solid geometry that has mass and other properties than can be called out downstream. See document (here) on how to solidify a pipe/hose.

John Piotrowski, Co-Founder & Product Manager
CadActive Technologies - www.cadactive.com

After solidifying, will the pipe update itself if the routing changes?

Yes, you just need to regenerate. See more info (here).

 

Cheers,

John Piotrowski, Co-Founder & Product Manager
CadActive Technologies - www.cadactive.com

It looks like when transitioning a solidified pipe assembly into a drawing and then adding a note with '&LENGTH_CENTER' still does not register and display the length.  Only when you add the solidified part model to the drawing via 'drawing models' independently and having it be active will register and display the length.  This will suffice for a drawing with one pipe, but how to differentiate lengths for a drawing with more than one pipe?

wbottis
12-Amethyst
(To:wbottis)

It looks like you repeat the process of adding the hose assembly model and then the solidified part model for that hose assembly to the drawing.  Add a note with parameter '&LENGTH_CENTER' with the solidified part model active and the length of the active model will register and display in the note with a suffix (session ID) to differentiate it from the length of the previous hose that was added to the same drawing.

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