with Creo 2 and WindChill 10.1,
We create a part (block) and a drawing, with properties in the titleblock. (ex Material)
We save both in the workspace part and drawing.
In the workspace, we set the values in the drawing ex. Material = Steel
The drawing titleblock does not update (material always empty)
Every time We MUST change the title block with itself,
so the properties are updated properly.
1. How to avoid substitution?
2. What we have to check, to get the correct values in the drawing?
Thanks in advance
Mario, I am moving this to the CAD Integration community.
In the meantime, is Material a parameter you have defined in the drawing or on the part? Are you changing the value in drawing or part?
If the parameter is defined in the drawing then the title block needs to use &MATERIAL:D, if you want it to pull the parameter value from the associated model you need to use &MATERIAL in the title block.
thanks for the quick replay.
We have material both in part and drawing.
We use &MATERIAL:D, in the title block
We set here the value, in the drawing attribute material.
But the only way to display the value, is to replace the
Titleblock with itself.
Than Creo ask for all the attributes defined, we just press enter for each request.
At the end, correct values are displayed.
Thanks, best regards
If Creo is prompting you for the parameter value, then that means the parameter does not already exist in either the drawing or the model. Once you enter a value this way, the value becomes "dumb" and it will not change, even if the parameter is later added to the model (or drawing).
I would use the part file MATERIAL for my drawing and not have to enter an additional parameter for the drawing.
Set up a relation so the MATERIAL parameter is populated from the part itself when you define the part material in File - Prepare - Model Properties.
Do you have the CREO parameters shared with Windchill attributes?
we have the drawing in Creo,
than switch to workspace and set the attributes there.
But the drawing does not reflect the changes.
Seems that attributes are present in the windchill workspace.
But at the end what we are trying/asking, is the "correct" way to setup the drawing template,
in a way that if user fill properties in windchill, they are filled in the drawing title block
Thanks in advance for any info
Ah, okay. When you make changes in the workspace, you need to reload the models into Creo. Think of making changes in the workspace as similar to another completely different user making changes. You won't see the changes until your reload the models in your workspace.
Again, it's perfectly fine to make the attribute changes in the workspace, just make sure reload the model after doing so. (Erase from session, then reopen.)
But even if we close the drawing
and reopen the drawing from the workspace,
attributes are not updated.
Just replacing the title block solve the issue.
But it cannot be like this, sure we are missing something
and we cannot figure out what's wrong.
Try going to the drawing and doing a "Switch Dimensions" and a "Switch Symbols". See if you notice a difference in what is displayed before the format is replaced and what is displayed after.
(Creo 3.0 locations - not sure on Creo 2.0)
(These ones are parameters that exist in our models.)
we did that and yes, we see the correct info.
So everything "looks" correct, but we just get the info updated replacing the title block.
thanks for the help
So just to be clear, the underlying parameter names look correct (both before and after format replacement) but the displayed values are incorrect (until after format replacement)? What happens if you "Update Tables" or "Update Sheets" (without replacing the format first)?
- underlying parameter name ok
- update tables and update sheets, done but nothing change
The "strange" thing, is that if you change the parameter value in the drawing, is updated in the workspace
so Creo->WindChill seems to work
Is WindChill->CReo that is not working
For me is a "bug", since everything looks fine, but id does not work...
This is a known issue we deal with daily, which I dont feel everyone follows here.
Certain parameters are not available at the time you create the drawing, until you check it in. Like the version for example. There is no version for the parameter to pull from when you create the drawing from a new part (or stand alone drawing) so you are prompted to add dumb text and break the association or hit enter and its left blank.
You found the only workaround, and that is to replace the table/block after check in, or re-add the parameter. In most cases, the parameters are available from the model. For us, it is primary the version from PDMlink that causes us problems. Again...there is no version until you check it in.
We had to 'educate' our users to check-in the model BEFORE creating the drawing for all parts. This will populate the Windchill parameters with the proper values which are pulled into drawing formats. We had a policy that all models and drawings were to be at the same revision level and we pulled model parameters for the format information.
If Creo is asking you for those values, then the parameters are not part of the empty drawing. What is happening, when you re-add the format, is a function that prompts to create the parameters based on text fields in the format.
Look to see the location of the empty drawing that is copied as a basis for your drawings is stored, and add those parameters to that empty drawing.
You don't get asked the first time because someone ignored the prompts and probably deleted the information from the template drawing(s).