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Creo Parameters and Drawing Text Formatting

BreMiSt
1-Newbie

Creo Parameters and Drawing Text Formatting

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.

12 REPLIES 12
dschenken
21-Topaz I
(To:BreMiSt)

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

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).

TomU
23-Emerald II
(To:StephenWilliams)

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.

10.PNG

It's also worth mentioning the search order. When you place a parameter on a drawing without anything after it (:D, :1, etc.), the drawing does the following:

  1. Checks the active model. If the parameter is found, it's value is displayed. (Model level only, not feature level) The session ID of the active model will automatically be appended to the parameter. If later this model is removed from the drawing, all parameters that referred to it will convert to "dumb" text.
  2. Checks the drawing itself. If the parameter is found, a ":D" is appended to it and the drawings value is displayed. Once the ":D:" has been added, the parameter will ALWAYS display the drawing's value.
  3. Prompts you to enter a value. Once you do, the parameter string will be replaced with the value you entered. The text becomes "dumb" at that point and will never again prompt for a new value.
gbronke
5-Regular Member
(To:TomU)

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?

dnordin
14-Alexandrite
(To:gbronke)

The "+" to show modification was replaced by a logical parameter &PTC_MODIFIED:D (:D 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.

 

Regards,

 

Dan Nordin

 

seanmcdonn
11-Garnet
(To:TomU)

what does placing a ":1" at the end of a parameter do to it?  I understand that 😄 directs the parameter to pull from the drawing, but I can't seem to find documentation yet which explains what effect the ":1" would have

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.

TomU
23-Emerald II
(To:seanmcdonn)

What @pausob said is correct.  Any number after a colon is a session ID.  Placing a :1 after a parameter doesn't automatically cause it to refer to a drawing, it just refers to the second thing loaded into Creo's memory since the memory was last erased.  That particular session ID could be a part, assembly, or drawing.

 

If you want to refer to the parent model without knowing the session ID, use the syntax :MDL.  This will automatically resolve to the drawing's active model.

 

If you only want to refer to the current drawing, use ":D"

 

https://support.ptc.com/help/creo/creo_pma/r7.0/usascii/index.html#page/detail/to_retrieve_model_par...

 

seanmcdonn
11-Garnet
(To:TomU)

Such valuable information, thank you so much for responding! 🙏

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.

--
Doug Schaefer | Experienced Mechanical Design Engineer
LinkedIn
dbaum
1-Newbie
(To:BreMiSt)

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?

dschenken
21-Topaz I
(To:dbaum)

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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