Combine/merge Creo prameters in darwing table

[MT_8208729]

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?

[Kotom-Eng]

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".

[KenFarley]

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.

[MT_8208729]

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.

[KenFarley]

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.

[MartinHanak]

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?

[MT_8208729]

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:

1. 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.