Parameter Entry not working in new template

[tzych-2]

I am trying to create a new template from a working form. In the form I am prompted for parameters when I create a new drawing. When I create a template from this form, I am no longer prompted for these parameter. I followed the instructions in the LMS lesson and entered &parameter_name when prompted for the parameter during the creation of the template.

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[MartinHanak]

Timothy,

&parameter_name must be entered into table cell.

Martin Hanak

[tzych-2]

When the template is created the &parameter_name:D is entered into the cell.

[MartinHanak]

Timothy,

I have found some info in https://support.ptc.com/appserver/cs/view/solution.jsp?n=CS51521

Martin Hanak

[tzych-2]

When you start CREO to make a new drawing template the TOOLS tab to place the drawing in template mode is not available until format file is loaded.

[MartinHanak]

Timothy,

it seems to me that in Creo Parametric 2.0 M070 everything works well.

1. I created prt0001.prt containing mypar (value=mytext)
2. I created frm0001.frm containing table (the cell contains &mypar)
3. I created drwtemplate.drw - I activated Tools tab and clicked Template icon, then I changed A4 size to frm0001
4. I created drw0001.drw using prt0001.prt and drwtemplate.drw

See uploaded data.

Martin Hanak

[tzych-2 · Accepted solution]

I was finally able to get the template to work by opening an empty drawing, placing the drawing into template mode,  going to LAYOUT-->SHEET SETUP and clicking on format to browse for my format file. CREO should allow TEMPLATE MODE to be selected before creating a drawing.

The format I was using has drawing parameters in 2 tables. This may have cause the issue.

[MartinHanak]

Timothy,

to replace a format, you can also click SIZE tag at the bottom of the graphics area.

Martin Hanak

[tzych-2]

Thanks for the tip.