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rleseberg1-Visitor
1-Visitor
May 10, 2017
Question

PTC Tutorial on Createing Associated Peramiters: I need a bit of clarification

  • May 10, 2017
  • 1 reply
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PTC Tutorial on Creating Associated Parameters: I need a bit of clarification

Here are the specific instructions from PTC Support on:

How to create an Assembly Level Relation that controls the variable parameter value defined under a flexible Component in Pro/ENGINEER, Creo Elements/Pro and Creo Parametric.

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  1. Create a parameter, in the part model and name it asm_param.
  2. In the assembly select the component and Right Mouse Button > Make Flexible.
  3. Add the part parameter asm_param; click Set Displayed Columns in the Varied Items dialog. Add the Assoc. Param column and click Ok. Type asm_param as the Associated Parameter for the added parameter, and click Ok.
  4. Create an assembly parameter named param. Then create an assembly relation as follows:

              asm_param:FID_#=param

Where :

  • asm_param is the Associated Parameter
  • # is the feature id of the component

  param is the assembly level (driving) parameter

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Item1) and Item 2) are clear enough.


Item 3) is a bit nebulous to me.

What is to be done in the "New Values" column?

Item 4) is also a bit confusing.

The relation uses the FID, which id a Feature ID.

What do you write to actually drill down to the dimensions inside the feature?

If I have two dims to family table, I would assume that I would need to parameters, correct?

I would also think that I would need two relations, one for each dimension, again, correct?

Etc., etc., etc.

This step needs a lot of clarification for me to truly grasp it.

1 reply

P
psobejko1-Visitor
1-Visitor
May 11, 2017

Regarding item 3)

at the point when you defined the associated parameter, the "*" in the "New Values" column should change to the value in the base model (in the case of dimensions).

And as you found out in the other thread (Flexibility: One of two varied items gets locked. (Why?)) you shouldn't leave it set to "*"

Regarding item 4)

Each thing you plan to "control" has to have an associated parameter.  That is the mechanism through which Creo communicates which "instance" of a component in an assembly is being "changed" from its base version.  Note that the names of these parameters do not have to be unique, meaning that if you have 3 flexible "rods" assembled, each can have associated parameters called "LENGTH" and "DIAMETER".

The relations that control flexible components can be composed at the assembly relation level.  It is easiest to do so by using that [] icon in the relation editor (the "insert parameter" function).  When you launch it, change to look in "component" and select the flexible component, and then you will have the table with the associated parameters you defined for it and be able to insert the proper "code" into the assembly level relations.  So you see how the FID_# syntax identifies what component instance will be "changed".

Note that relations can also be written at the component level: launch relation editor, Look In "Component", select the flexible component, and then you will see the associated parameters listed in the "Local Parameters" section.  Also, you will notice that the FID_# syntax will not be present in component relations - because the system already knows what component will be "changed".

Hope this clarifies things a bit...

R
rleseberg1-VisitorAuthor
1-Visitor
May 11, 2017

Thanks for that Paul,

So, does the FID_# simply tell the editor which feature to look in?

Then at that point, can the dimensions be selected?

P
psobejko1-Visitor
1-Visitor
May 11, 2017

The :FID_# syntax tells the system, not the editor, how to regenerate the model...

I don't understand your question about the point at which dimension can be selected.  That is done when either making the component flexible in the assembly, or when predefining the flexiblity at the part level...

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