I am hoping someone can point me to a good resource.
I am working with a drawing that contains various text entities to include text in the drawing format, text in notes, and text in other tables. As I stumble through drawing creation or revisions I notice that these various text entities contain parameter callouts and text formatting code. I understand and appreciate this approach as things like drawing revisions will automatically update if the appropriate parameter is used. Also, for example, being able to put boxes around a portion of text in a note is important for flag notes and such.
I'd like to be able to understand the "code" used to make the most of this capability. Does anyone have a good resource that explains the formatting code and how to use it?
As a specific example here is something that accidentally worked but I can only guess why:
I was having trouble getting the drawing revision to update from "-" to "A" in my drawing format. The table cell properties for the revision showed the parameter "&PROI_REVISION:1" which resulted in "-" in the revision block. After some time playing with this code I changed it to be "&PROI_REVISION". I'm not sure why this worked but it did. I suspect that the former was pulling the value of the revision parameter of the part shown in the views and the latter was pulling the value of the rev parameter of the drawing but this is just a guess. I don't like having to guess to get something to look correct. Let me emphasize LOOK CORRECT because even though the rev now shows "A" I'm still not sure if that is truly the drawing revision. I need to be sure.
Any help would be greatly appreciated.
It's not guessing as much as reading all the documentation. No one can help determine the correct drawing revision except someone in your organization. However, I can give some hints about parameters:
&total_holes where total_holes is a parameter or the name of a dimension
&d31:45 where d31 is the name of a dimension and 45 is the session ID of the component the dimension is from (Use Info/Switch Dimensions to show the symbolic names used on a drawing and to see the related session IDs.)
&annotation_name(:session_id) (example Change_record note in the model tree ->&Change_record.)
&scale (this is the default scale of the active model on a drawing. If there is more than one model for a drawing the value for this may not represent what is correct for the model shown on any particular sheet.)
&linear_tol_0_0 et al
&angular_tolerance_0_0 et al
&part_note - This is display starting on the next new line
&sym(name of symbol)
The system will search what it's attached to fill out the parameters, assuming it has those parameters. Watch out for cross sections, you have to attach to a surface not an edge, the edge belongs to the assy, not the sectioned component.
For a note with a leader, this shows two lines, the first with the parameter bom_part_no, and the second with the param, bom_description_asm.
Also available -
Dave did a great job of getting them down.
The "&PROI_REVISION" is the revision of the drawing as reported by the proi_revision parameter from intralink. When you add the "" (colon D if it decides to change it to an emoticon), it reports the parameter associated from the drawing (as opposed to the part or assembly).
If you want to use the native Windchill parameter instead of the old Intralink parameter, it's called "PTC_WM_REVISION". There are actually a bunch of different Windchill parameters you can use.
It's also worth mentioning the search order. When you place a parameter on a drawing without anything after it (, :1, etc.), the drawing does the following:
System parameters, things like &scale and &format, as opposed to model or drawing parameters must be all lower case. Typing &scale will get you the scale of the drawing in the note, typing &SCALE or &Scale will get you, literally, &SCALE or &Scale in the note.
Does anyone know how to do dynamics notes? I'm looking to utilize my FIND # from my BOM in my sheet notes but whenever I add a part to my BOM the numbers that correspond to my part in the notes has to be manually changed. Is there a way to set in a note a specific cell in a column of the rpt.index that is the FIND # column?
The BOM number is fixed to the table and the balloons linked to the table. There is no way to use the index number in a note.
As a bit of interest, you can have more than one table in a drawing associated with an assembly and have entirely different index numbers in that table, or a simplified rep associated to the table and different item numbers.
We used to use the old proi_version parameters because we would get the little + sign next to it if it was modified and not checked in. with the new PTC_wm that goes away completely. I am guessing because its reading from Windchill and not the Workspace?
The "+" to show modification was replaced by a logical parameter &PTC_MODIFIED ( for the drawing). You can use this parameter to indicate YES/NO or TRUE/FALSE depending on your drawing setup .dtl option yes_no_parameter_display.
You can look at https://community.ptc.com/t5/Creo-Modeling-Questions/Looking-to-add-an-indicator-on-the-drawing-if-t... for a method of showing the "+" in the corner of the drawing.