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Parameter link/relations between parts

Sergey
14-Alexandrite

Parameter link/relations between parts

Hello.

 

Would anybody, please, make a detailed description of the parameter link between parts?

 

I want to assign the values of one part to the other, and by this, drive the second part (driven) by changing the dimensions of the first part (driving). For example, a plate of h=100mm and w=200mm, must drive another custom made plate, so that after the values of the first part (h and w) has been changed, the dimensions of the second plate changes accordingly.

 

Best regards,

Sergey

 

1 ACCEPTED SOLUTION

Accepted Solutions


@Sergey wrote:

Hello.

 

Would anybody, please, make a detailed description of the parameter link between parts?

 

I want to assign the values of one part to the other, and by this, drive the second part (driven) by changing the dimensions of the first part (driving). For example, a plate of h=100mm and w=200mm, must drive another custom made plate, so that after the values of the first part (h and w) has been changed, the dimensions of the second plate changes accordingly.

 

Best regards,

Sergey

 


Hi,

I think you have to assemble both parts into same assembly and then define relations.

In case that you want to modify dimension value, you must open this assembly, modify dimension value and regenerate assembly.


Martin Hanák

View solution in original post

6 REPLIES 6


@Sergey wrote:

Hello.

 

Would anybody, please, make a detailed description of the parameter link between parts?

 

I want to assign the values of one part to the other, and by this, drive the second part (driven) by changing the dimensions of the first part (driving). For example, a plate of h=100mm and w=200mm, must drive another custom made plate, so that after the values of the first part (h and w) has been changed, the dimensions of the second plate changes accordingly.

 

Best regards,

Sergey

 


Hi,

I think you have to assemble both parts into same assembly and then define relations.

In case that you want to modify dimension value, you must open this assembly, modify dimension value and regenerate assembly.


Martin Hanák
tbraxton
21-Topaz II
(To:Sergey)

One option is to use a Creo Notebook to define parameters that are passed to parts and used in relations to control the features in the parts. No assembly required to implement this using a Notebook. The Notebook allows for the definition of global parameters and relations that can be declared to any part. This is the method I would use for the scenario that you describe as there is a single file that controls all dependent models.

 

http://support.ptc.com/help/creo/creo_pma/usascii/index.html#page/assembly/asm/asm_three_sub/About_Notebooks.html 

 

Another option is to use the session ID to use dimension values from one part to drive another. If you pursue this be mindful of creating circular references. You will need to establish a master slave paradigm to avoid this issue. This will be done in the context of an assembly. Consider that once you use an assembly to establish dependency it will be required to load the assembly into session to make changes. This becomes quite unwieldy with large assemblies.

 

When I have used this approach, I create a design assembly that contains only the components needed to establish the propagation of the design intent and no other parts. These design assemblies exist only to act as a conduit for design intent management. This will greatly simplify design intent management and modification. 

========================================
Involute Development, LLC
Consulting Engineers
Specialists in Creo Parametric
KenFarley
21-Topaz I
(To:Sergey)

This comes up every now and then. Here's a past discussion of a similar nature.

 

Past Top Down Design Discussion 

 

It's something I do a lot, especially with lots of parts that need to interface with each other and are subject to changes.

Sergey
14-Alexandrite
(To:KenFarley)

I think the main reason of why it comes up from time to time is because of there are no any efficient way of doing it.

I would like to refer to Autodesk Inventor and feature that is used to link parameters of parts that an assembly is made of. It is very easy, convenient and efficient.

In my opinion something similar Creo must have. Anyway, I have found a solution of managing parts in the assembly by creating parameters in assembly mode as @MartinHanak  advised and linked them to the dimensions of parts.

tbraxton
21-Topaz II
(To:Sergey)

@Sergey 

Do you have the Creo extension that includes Creo notebook files (.lay extension)? If you do then you have the top down design tools to efficiently manage the design intent scenario you have asked about. The notebook is one of the tools available in Creo to control more than one model in a top down design scheme.

 

If you have not researched the top down design tools I would encourage you to do so. These tools enable Creo to increase productivity dramatically when applied effectively.

 

This is an simple example of a notebook used to configure critical parameters of an internal combustion engine architecture. Using this notebook it is possible to make design changes to multiple parts in seconds. The 2D drawing tools for Notebooks is inexcusable and the tool has not been updated by PTC in a long time but it is still relevant. It seems PTC want one to purchase Mathcad to use for Engineering Notebooks. 

 

There are relations defined in this notebook that are not shown here but this should give you an idea of how it works from a UI standpoint. The drawings  are not parametric and exist only to document items needed for the user to interpret the contents of the notebook.

 

Notebook for engine designNotebook for engine design

========================================
Involute Development, LLC
Consulting Engineers
Specialists in Creo Parametric
Sergey
14-Alexandrite
(To:tbraxton)

I will definetly study the notebook top down design method. Thank you for advise. Due to my experience in Autodesk Inventor I expected something similar in Creo as well.

 

Another question: As I know it is possible to manage parts from Mathcad. Is it possible to do so for an assembly?

 

 

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