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BreMiSt1-Visitor
1-Visitor
August 6, 2014
Question

Creo Parameters and Drawing Text Formatting

  • August 6, 2014
  • 2 replies
  • 23859 views

Hi all,

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:D". 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.

2 replies

D
dschenken1-Visitor
1-Visitor
August 6, 2014

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:

Examples:

&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.)

&todays_date

&model_name(:session id)
&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.)

&type

&format (size)

&linear_tol_0_0 et al

&angular_tolerance_0_0 et al

&current_sheet

&total_sheets

&dtm_name

&part_note - This is display starting on the next new line

&sym(name of symbol)

&<parameter_name>:att_mdl

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.
&bom_part_no:att_mdl
&bom_description_asm:att_mdl

Also available -
Param_name:att_edge Edge
Param_name:att_feat Feature
Param_name:att_mdl Model
Param_name:att_cmp Component

    S
    23-Emerald III
    StephenW23-Emerald III
    23-Emerald III
    August 7, 2014

    Dave did a great job of getting them down.

    The "&PROI_REVISION:D" is the revision of the drawing as reported by the proi_revision parameter from intralink. When you add the ":D" (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).

      P
      19-Tanzanite
      pausob19-Tanzanite
      19-Tanzanite
      April 17, 2021

      Can you give an example?

      without seeing the context, I'd guess that it's the session ID of the component whose parameter is being referenced in the note / relation.

      D
      dbaum_2003191-Visitor
      1-Visitor
      March 21, 2016

      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?

      D
      dschenken1-Visitor
      1-Visitor
      March 21, 2016

      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.

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