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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?
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".
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.
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.
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.
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:
I tried to add underscore character manually ... see attached video adding_underscore.mp4
Are you also wondering what happened?