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..
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 config.pro) and save it in template folder, so it resides next to actual part file.
3. In config.pro, 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:
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 config.pro then it was working...
but while using my old config.pro it's not working....
Your paths contain spaces. for those to work you need to put them to quotation marks.
drawing_setup_file "C:\PTC\Creo 1.0\Settings\Drawing.dtl"