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This will be rather long but here we go...
1. Open SolidWorks, make sure you have no parts, assy open. You should have a blank SW.
2. Create a new drawing, chose a frame that you want from provided templates.
3. Go to option and the tab "Document properties". All settings on this tab is unique for this file. So if you want to allways have two decimals, select Units, select your unit system and number of decimals in the table. Here you can select that a Length dimension should have two decimals (.12) and an Angle dim one decimal (.1)
4. When all settings are done, click File - Save as. In the Save as type field change to Drawing template, chose a nice name, ie. GerryTenplate.drwdot.
Now you have a document file template. Next step is to adjust the sheet itself.
5. Right-click in the drawing area and chose "Edit sheet format".
6. Zoom in the title header.
7. As you can see there a some coding, ie. $PRP:"SW-File Name". All these are ordinary notes that with correct coding collect properties from the drawing file. If you instead insert a note where you write $PRP:"SW-Author" it will collect the info from the properties found under File - Properties - Author. Here is a list of some more examples:
SW-Author = Author field in Summary Information dialog box
SW-Comments = Comments field in Summary Information dialog box
SW-Configuration Name - Configuration name in ConfigurationManager
SW-File Name = document name, no extension
SW-Folder Name = document folder with backslash at the end
SW-Keywords = Keywords field in Summary Information dialog box
SW-Last Saved By = Last Saved By field in Summary Information dialog box
SW-Subject = Subject field in Summary Information dialog box
SW-Title = Title field in Summary Information dialog box
8. When you have fixed your title header, right-click in the drawing area and chose "Edit sheet" to return to non-editing mode.
9. Click File - Save Sheet Format, chose a file name, ie. Gerry-A-landscape.slddrt.
10. You are done!
Next time you want to make a drawing simply select your own templates.
Some remarks that are good to know about:
A. Make a backup copy of your own templates since they will disappear during upgrade of SolidWorks (unless you save as under B).
B. You could chose to save all private templates in a folder of your own (=outside of SolidWorks main folders), ie. on your network so everyone can use the same templates. In order for each computer to find these templates you need to change the Options - File locations and Add your network paths.
C. You can create how many templates you want. One sheet format for each size, as well as portrait-landscape versions. Maybe you need some templates in metric sytem others in inch, maybe some where your customers logotype is inserted etc.
D. You can create your own properties in File - Properties and they can then be used in your drawing. Maybe you would like to have a custom property for Project (which actually already exist as a selection in drop-down list). If so then just add that property and refer from the sheet format back to this property.
E. With SW2009 you can make a Manager tab where your necessary properties can be selected without the pain to go via File - Properties. I still have not installed SW2009 yet (was waiting for SP1.0 which now is available) but if you need help how to make this tab I guess our fellow forum members can provide instructions.
Good luck with creating your drawing template.
Thanks - will try this out tomorrow.