topic Combine/merge Creo prameters in darwing table in 3D Part & Assembly Design

Combine/merge Creo prameters in darwing table

MT_8208729 — Tue, 04 Feb 2025 22:12:35 GMT

Hi Community,

(Creo 10.0.4.0)

I'm setting up templates for new drawing templates and want to have a field in the title box about the export file name:
1-00001234_01.stp
<Part_numnber>_<Version>.stp
&<parameter_name>_&<parameter_name>

It looks for parameters the underscore "_" is breaking the definition, it needs a separator. What is the correct way to combine two parameters without space or with a character?
Is there any markdown available for Creo tables?

Re: Combine/merge Creo prameters in darwing table

Kotom-Eng — Tue, 03 Dec 2024 11:02:42 GMT

You are in the wrong forum.

PTC has two CAD systems: Creo+ and Creo Parametric and Creo Elements Direct.

Which makes it confusing.

More, for Creo Elements Direct:

- The 3D software name is Modeling, and

- The 2D software name is Drafting.

For Creo+ and Creo Parametric, use only this tab:

You should move your post to this community to have a better chance to get an answer.

To move your post, click on the three vertical dots on your initial post and click on "Notify Moderator".

Re: Combine/merge Creo prameters in darwing table

KenFarley — Tue, 03 Dec 2024 11:59:41 GMT

This is one of those weird behaviors of referencing parameters in drawings.

It's as if Creo needs to see a space as a separator in order to interpret the parameter correctly. But, it only needs this the first time the parameter is used and evaluated.

What I do for similar things is first define the text as

&part_number _&version

Let it evaluate that, it fills in the parameter values, etc.

Now I delete the space before the "_" character, and you get what you really want.

Re: Combine/merge Creo prameters in darwing table

MT_8208729 — Tue, 03 Dec 2024 12:05:18 GMT

Thank you, I tried, however it still broken after I delete when it is evaluated.
Im looking for a solution what I can use in the template.frm files: evaluate during load or sheet setup update.

So far only hacked with keeping the "space" there and change font locally to 0.1, so it is very small font space delimiter.

Re: Combine/merge Creo prameters in darwing table

KenFarley — Tue, 03 Dec 2024 14:21:37 GMT

Yes, it seems this trick only works for text that is being typed in and manipulated.

I've also noticed that a lot of the tricks for inputting text seem to have been disabled by in the latest versions of Creo due to a different approach to text formatting in general. For example, I thought it would be possible to specify that the different parts of the text are distinct by putting in something like

{0:&part_number}{1:_}{2:&version}

but that doesn't work, either.

Something that would work but is a pain if you have a lot of models you need to do this for is to have another parameter that is built with a relation in the model. Define another parameter like file_name

Then add a relation to "build" it:

file_name = part_number + "_" + version + ".stp"

Then in the format call out &file_name.

Maybe someone else has a clever way to do this in the latest Creo versions, but if not this is a possible solution.

Re: Combine/merge Creo prameters in darwing table

MartinHanak — Wed, 04 Dec 2024 07:31:23 GMT

Hi,

it looks like underscore character is problematic.

I created format with table. Its single cell contains &delka:MDL_&sirka:MDL-&vyska:MDL

My model contains above mentioned parameters:

When I create a drawing I get following result:

underscore character disappeared

I tried to add underscore character manually ... see attached video adding_underscore.mp4

Are you also wondering what happened?

Re: Combine/merge Creo prameters in darwing table

MT_8208729 — Fri, 06 Dec 2024 10:37:43 GMT

Üdv Martin! 😉

It looks like it is a bug or missing syntax/markdown to combine text in tables.
So far there is two possible solition:

Custom parameter: proposed by @KenFarley

file_name = part_number + "_" + version + ".stp"

Space hack: just add a space before the point and change font size to 0.1, it works so far. However the syntax looks weird, don't understand how this works:

Ref.: N/A Remove sharp edges Install all A2-SS Helicoils Geometry CAD file: &PART_NO:mdl{11: }_0&PART_ISSUE:mdl{14: }.stp

PS: not sure if there is any new solution/view for table editing mode, literally I cant see anything when editing it, only works in the note properties view.