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DIM Styles


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I have created a drawing sheet with the border,title block, and dimension styles. I then changed the name and saved it in the templates folder. In the 'new' dialog box, I now have my drawing template to choose. When I start it, the border and title block are right but the dimension style is back to the original. Where as when I open the idw file from the template folder, everything is right. Any suggestions?
Inventor will load the dim styles from the style library. To save your styles, open the blank drawing you created then go to 'format' & 'save styles to style library'. This will overwrite the Inventor styles with you own ones.
You need to save the styles you changed in your template file to the styles library. There is a conflict between the styles library dimension style and the template dimension style. When this occurs, the styles library takes precedence.
I created a Standard style, called F. F is a variable in this case, call it anything you want, i.e. Fraction. I then created a DIM Style called F. I then set up all the dim features that I wanted under DIM Style F. Finally, I created a new Object Default Style called, F. Under the newly created Object Default Style, F, make sure you adjust the Object Type (Dimensions) to the newly created DIM Style F. Everything should match up. The Standard, F uses the DIM Style F as instructed to by the Object Defaults for Dimensions called F. For all of the Standards, under the Availble Styles tab, make sure that you select all of the dimensions that you want available for use in any one Standard. If Decimal is your Active Standard, but you have made Fractions available , you can switch styles on the fly when you need to. I.e., you can pick a single dimension, or multiples, and at the top of the screen will be a pull down of all dim styles that you have made available. Pick fraction and the dimension(s) change to Fraction. When finished pick save and then close. Under Format, Save styles to Style Library.

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