List of Creo System Parameters for Drawings

Have you wondered how to pull the weight of the 3D model into Creo Drawing and wanted to update whenever a change happens in the 3D model in creo? yes, It can be possible with the List of Creo System Parameters for Drawings. Not only that there are so many numbers of system parameters for Creo Drawings that actually help you to create a more engineered drawing.

These Creo System Parameters for Drawings are very useful while in detailing. They are listed below according to Mass property parameters, dimension parameters, User defined parameters, Drawing Sheet properties, Product Data management related Parameters.

List of Creo System Parameters

Mass Property Parameters

[Material should be assigned to the model]

&pro_mp_mass	Display the total Weight of the entire model
&pro_mp_density	Display the total Density of the entire model
&pro_mp_volume	Display the total Volume of the entire model
&pro_mp_area	Display the total Area of the entire model
&pro_mp_cogx, &pro_mp_cogy, &pro_mp_cogz	Display the Centre of the gravity about X, Y, Z coordinates for the entire model
&pro_mp_Ixx, &pro_mp_Iyy, &pro_mp_Izz	Display the Moment of inertia about x, y z-axis for the entire model respectively

Tags: Creo System Parameters, Creo parameters in drawings, System parameters in creo

Dimension Parameters

&d#	Displays a dimension in a drawing note, where # is the dimension ID.
&ad#	Displays an associative dimension in a drawing note, where # is the dimension ID.
&rd#	Displays a reference dimension in a drawing note, where # is the dimension ID.
&p#	Displays an instance number of a pattern in a drawing note, where # is the pattern ID.
&g#	Displays a gtol in a drawing note, where # is the gtol ID.

&angular_tol_0_0

Specifies the format of angular tolerance values in a note from one to six decimal places.

Tags: Creo System Parameters, Creo parameters in drawings, System parameters in creo.

User Defined parameters

&<param_name>	Displays a user-defined parameter value in a drawing note.
&<param_name>:att_cmp	An object parameter that indicates the parameters of the component to which a note is attached.
&<param_name>:att_edge	An object parameter that indicates the parameters of the edge to which a note is attached.
&<param_name>:att_feat	An object parameter that indicates the parameters of the feature to which a note is attached.
&<param_name>:att_mdl	An object parameter that indicates the parameters of the model to which a note is attached.
&<param_name>:att_pipe_bend	An object parameter that indicates the parameters of the pipe bend to which a note is attached.
&<param_name>:att_spool	An object parameter that indicates the parameters of the spool to which a note is attached.
&<param_name>:EID_<edge_name>	An object parameter that references edges.
&<param_name>:FID_<feat_ID>	An object parameter that includes a feature parameter in a note by ID.
&<param_name>:FID_<FEAT_NAME>	An object parameter that includes a feature parameter in a note by name.
&<param_name>:SID_<surface_name>	An object parameter that references surfaces.

 

Sheet Property Parameters [Creo System Parameters]

&sheet_number	Displays a drawing label indicating the current sheet number.
&sheet_name	Displays a drawing label indicating the current sheet name.
&det_scale	Displays a drawing label indicating the scale of a detailed view. You cannot use this parameter in a drawing note. Creo Elements/Pro creates this parameter with a view and places it in notes automatically. You can modify its value, but you cannot call it out in another note.
&dtm_name	Displays datum names in a drawing note, where the name is the name of a datum plane. The datum name in the note is read-only, so you cannot modify it; unlike dimensions, a datum name does not disappear from the model view if included in a note. The system encloses its name in a rectangle as if it were a set datum.
&dwg_name	Displays a drawing label indicating the name of the drawing.
&format	Displays a drawing label indicating the format size (for example, A1, A0, A, B, and so forth).
&linear_tol_0_0	Specifies the format of dimensional tolerance values in a note from one to six decimal places.
&model_name	Displays a drawing label indicating the name of the model used for the drawing.
&parameter:d	Adds drawing parameters to a drawing note, where the parameter is the parameter name and :d refers to the drawing. .
&<param_name>:mdl	Adds a model parameter to a drawing note, table cell, or drawing Program where <param_name> is the parameter name.  Using the :mdl suffix prevents the drawing from switching the parameter reference from the model to the drawing (&parameter:d) if the model parameter cannot be located.

&scale	Displays a drawing label indicating the scale of the drawing.
&scale_of_view_detailed_bar
&sym(<symbolname )	Includes a drawing symbol in a note, where symbol name is the name of the symbol.
&todays_date	Displays a drawing label indicating the date on which the note was created in the form dd-mm-yy (for example, 2-Jan-92). You can edit it as any other nonparametric note, using Text Line or Full Note.   If you include this symbol in a format table, the system evaluates it when it copies the format into the drawing. To specify the initial display of the date in a drawing, use the configuration file option “todays_date_note_format.”
&total_sheets	Displays a drawing label indicating the total number of sheets in the drawing.
&type	Displays a drawing label indicating the drawing model type (for example, part, assembly, etc.).
&view_name	Displays a drawing label indicating the name of the view. You cannot use this parameter in a drawing note. Creo Elements/Pro creates it with a view and places it in notes automatically. You can modify its value, but you cannot call it out in another note.
&view_scale	Displays a drawing label indicating the name of a general scaled view. You cannot use this parameter in a drawing note. Creo Elements/Pro creates it with a view and places it in notes automatically. You can modify its value, but you cannot call it out in another note.

Product Data management related Parameters

&pdmdb	Displays the database of origin of the model.
&pdmrev	Displays the model revision.
&pdmrev:d	Displays the revision number of the model (where :d refers to the drawing).
&pdmrl	Displays the release level of the model.

Tags: Creo System Parameters, Creo parameters in drawings, System parameters in creo

Content Credits: Creo help Center [http://support.ptc.com/help/creo/]

Repeat Region Creo Parameters