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How to create drawing file Automatically while creating the 3d solid model ?


How to create drawing file Automatically while creating the 3d solid model ?

I searching about the creating standard formatting drawing which include views, sec.views, material,BOM,temp. etc...

I just know about it will created "START PART" saving all parameter & template and then drawing file is created automatically but how it will be created ? I don't know step by step procedure?pls help me..

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You'd need to do something like this:

1. Create a drawing template and put in it format, all views you nedd, BOM tables, notes and so on.

2. Name the drawing template with name of your start part (you can check it's name using template_xxx option in and save it in template folder, so it resides next to actual part file.

3. In, set the option rename_drawings_with_object to part, assembly or both, depending on your needs.

4. Now, every time you create and save a new part (or assembly) model, it'll also save its drawing, based on template you created, in the directory, where you save your part.

Also know that when you create the format files, any text that is filled in from the part/assembly data has to be added in tables, not just text. These are filled in by "relations" included in your part or assembly files. if they do not exist as relations, you will be prompted for each entry. It is best for your start part or assembly to have these relations included although they can be imported from a text file after the fact.

Do not make the mistake of not keeping a backup copy of your formats if you use the default install location. Software updates will delete these folders.

This is a nice little video for setting up default views along with some other stuff:

Hii.!! Lukasz Mazur

hyeee it's done....I am able to doing drawing file of part and Assy simultaneously ..
it's create drawing file that Assy or Prt...wit my decided views...

Thank You..

Glad we could help, Samrat

Yeah, glad it's working as intended

Hi..Lukasz Mazur

As per ur steps i am following it,and it done properly ...but last few days it was not working..

when i create new shortcut of creo parametric and Change it's "Start in" Path with new then it was working...

but while using my old it's not working....

Maybe you have a path statement in the new that is not in the old

how i find Path statement in

You can edit the file in a text editor. Look for format path statements.

I try to find ...but i can't that i attached my config file ...


That is a very long list of mapkeys. When you have the problem, are you using the mapkeys? Try it without the mapkeys.


Your paths contain spaces. for those to work you need to put them to quotation marks.

Like this:

drawing_setup_file "C:\PTC\Creo 1.0\Settings\Drawing.dtl"