I am trying to create a Format that uses parameters to fill out the title block on our drawings. When I create a drawing, Pro prompts me for values for each parameter, but once I have entered the values, the parameters do not show up in my list of parameters for the drawing. Is there a way to get a drawing to inherit the parameters from its format?
Are you asking how a drawing can inherit it's parameters from the model when using template/formats?
Yes, I am trying to get my drawings to inherit the parameters from their respective formats. This way, I can use a format, and it will bring over parameters like title, revision, and drawing number, and then I will be able to edit them within the drawing if needed. Right now, the drawing prompts me to enter values when I bring the format in, and then it prompts me again each time I create a new sheet. When I create a new sheet, I'd also like it to autofill the same values that I have already specified.
The variables have to be placed in tables. You cannot simply place a note as the variable. Strange but true.
I did create individual tables in my title block area for the variables to go into. And I have the parameters created in the Format parameters.
Can you post the file so I can see what is happeing?
parameter entered in format table cell using format &myparameter must exist in drawing model (not in format).
When you create new drawing using a format, then Creo copies table defined in format into drawing and looks for &myparameter in a drawing model. If the parameter exists then Creo put its value into table cell. I the parameter does not exist, then Creo asks user to enter a value.
Once I enter parameters values for it after they are prompted, is there a way to have the drawing have those parameters in its parameter table? Instead, I can currently no longer access the parameter to change it once I enter it from the start.
standard procedure is:
1.] create start model containing all requested parameters
2.] create format using parameters present in start model
3.] create real model using start model (termplate)
4.] create real drawing using format
In such case there is no need to enter parameter values manually.
In case that you entered parameter values manually in the drawing and later created parameters in drawing model, then you can try:
a.] enter &myparameter into drawing cell
b.] remove format from the drawing and assign it once again
Our drawings are typically multiple parts, not just one part, so having the parameters assigned to the start part would just not work. We were also hoping to use the parameters to easily change revision levels acrossed all of the drawings. If I need to create the parameters every new drawing, then it really isn't saving any time.
If you need an advice, you have to explain your situation precisely.
? how many drawing models are placed in your drawing
? are drawing models parts, only (or do you use assemblies or some combination)
? explain the contents of table (does it contain parameters from one model or several models)
? other info ...
The number of parts and or assemblies vary greatly among our drawings.
The table contains parameters specific to the drawing, ussually the assmebly not necessarily specific to the parts on that given page. However, we do not want to be assigning these parameters to the assmeblies or other parts, but instead be able to define them within the drawings.
Actually, I think I figured out a solution on my own by bringing the format into a template, and then using a template instead.
Thanks for your help,
Your way of using PTC Creo is a bit unusual, Michael. Relations are tied to models, be they parts or assemblies. With multiple parts in a drawing, this makes it a little more troublesome.
Another issue that often comes up when you have multiple sheet drawings is that the format doesn't like variation from one sheet to the next. There are a few built in variables that can be used, but you cannot use the same format if you want to, say, change the title of the second sheet. What I am getting at is that sustainability too is a bit cumbersome.
For the issue at hand, can I recommend installing a "data part" into the drawing which only has the relations needed for the format? This would resolve the issue of changing revision data in one location, for instance.
If you enter the prompts for a new drawing to fill in the format, the relations are not built. The variable is simply over-written by the text you entered. I suppose it simply doesn't have a place to put the data. However, you can edit this text with the normal text editor. You have to double click the table's cell to activate the editor.
I suspect you will need to develop a way of working with what you have available. I will copy and paste text from drawing to drawing when time is of the essence. I have developed the tables for a generic format but if a client provides a format, I really don't have much choice unless they want me to develop a format specifically for Creo. That doesn't happened often since they pay by the hour.
I think the idea of a data part for this option sound fairly unique. Have you used it before?
Ummmm... no... but it is as logical as any other solution I can think of.
I was thinking that in an assembly, you would have these relations defined and so if the assembly does not exist, another "common" element must be used. Why not an "empty set"?
Typically I only have one model and I know that it takes a little more care to have multiple models in a drawing. I have had issues with models following the drawing's default scale, for instance.
As for the relations, you can actually assign them to the specific part while in the drawing by selecting it. How the format picks them up from that particular part is another question.
I ended up making the format with the parameters, and then a drawing with that format, and the parameters added in. I then am using that drawing as a template. This allows me to use all my parameters, and the title block is filled in on every new sheet I create.
Glad you got this worked out, Michael.
That works for most things Martin. But in a windchill environment how do you stop creo from clearing fields that link to parameters that are only assigned after the first check-in?
For example "&ptc_wm_revision: D" and "&ptc_wm_created_by: D" [obviously there should be no space between the : and D]
You have two options.
Is it possible to link the parameters from creo title block with the model name, so that all the model names gets updated automatically when i put it in trail file?
The model filename will display in a note as &model_name (can be used in the title block format)
The drawing name can be accessed from &dwg_name (can be used in the title block format)