How to edit sketch relation from program of a part?

[MB_3972011]

Dear all, 

i would know how to edit a sketch quote relation from the program file of a part. 

I am creating relations on the fly, so to speak, and I cannot access them at a later time in order to modify them. I began by making the parameter, NTHICK, equal 1.5. For many extrusions I have entered NTHICK as the dimension value and Creo/Pro will ask me if I would like to establish a relation for the dimension. I click yes and a relation is created. I can verify this by double clicking the dimension and then I'm told that it cannot be modify becuase it is controled by the relation d256 = NTHICK; this is good, its what I want. The problem is that I cannot access the relation to change it. Going to Tools>Realtions doesn't work--the realtion is not there. Please help.

As this was done in  many parts i would know if there is any update on this topic.

Older similar post

https://community.ptc.com/t5/3D-Part-Assembly-Design/cannot-find-created-relations/td-p/410952

Thanks

[tbraxton]

Set the relations editor to the appropriate context to access the relations (see pic below). As a general rule I would not create sketcher relations except for the use of trajpar in variable section sweep surfaces. There are of course exceptions to this rule but from your description of using a parameter to set the thickness of extrusions sketcher relations do not seem like the best option.

Depending on how you created the relations they may be sketcher or feature relations based on your post.

[MB_3972011]

Any chance to edit the parameters from program of the part?

At least to show them inside according to edit them?

[tbraxton]

You are asking if when running Pro/Program for a part model in Creo if the user can be prompted to enter a value for a parameter when the program is run? If this is the question, then yes this is supported.

Input function : About Input Parameters and Prompts

[MB_3972011]

The question is if i can edit the relations that are controlling sketch quotes from the PART Pro/program. 

Up to now i can't see these relations.

Thanks

[tbraxton]

If you invoke the edit design option, you will get this interface and there is a relations section indicated by the yellow in the pic below. When you edit the parts design are there any relations showing in the Program?

[MB_3972011]

can't find the relations following this procedure, i have to do it with sketch opened, any suggestion?

[mkajdan]

We don't use sketch relations either because when troubleshooting a model they can be hard to identify or find.

Dimensions shown in the sketch that are used in sketch relations.

The same dimensions shown outside of the sketch in part mode.  These are what are used to create relations to sketched features in the part.

The same dimensions shown outside of the sketch in assembly mode.  These are what are used to create relations to sketched features in the assembly.

If you create your relations in part mode or assembly mode you will be able to view/edit them without entering into the sketch.

[KenFarley]

Something I learned long ago, it seems that the relations used within features, in the sketcher, are only visible within the sketch. This likely has to do with the namespace for the sketch, since you'll notice that the relations in a sketch have dimensions like sd1, sd2, etc. Those names are only valid within the scope of the currently open sketch. Edit another sketch within the same model, you might see the same names for different things. For example, I just opened a random model of mine and saw sd16 used in two sketches.

I would guess that the Pro/PROGRAM stuff is only able to use part or assembly level relations, therefore you will not be able to see sketch relations. If you are using a part parameter to set a bunch of sketch dimensions, you just need to change the parameter value to change all of your sketches, so you might not need to see the sketch relations in the Pro/PROGRAM stuff, though. You just have to be sure you've done all the assignments correctly in the sketches.

[tbraxton]

PTC documentation states that: All relations valid in a Creo Parametric model can be entered in a Pro/PROGRAM design.

This implies that feature and sketch relations can be entered although I see no examples of this in the documentation. I have never attempted to use sketch relations with Pro/program.

https://support.ptc.com/help/creo/creo_pma/r11.0/usascii/index.html#page/fundamentals/program/relations.html 

[MB_3972011]

Thanks a lot to everyone, as i didn't know about this "problem" i've used the function of entering the value directly in the sketck as it seems extremly simple and wasn't creating a lot of stuff written in the relations thinkng that maybe were written in the program only instead of inside the sketch relations.