To Create a DWG Template from an AutoCAD File

You create a DWG template from an AutoCAD file by opening an AutoCAD drawing file and specifying a new standard.

You then edit the new standard and Object Defaults style. Finally, you purge unused styles. If you want, you can also save the template styles to the Styles Library. If the AutoCAD file is an AutoCAD drawing template (.dwt), you must rename a copy as a DWG file (.dwg) before opening it in Autodesk Inventor.

Open the Template

  1. In Inventor, click File Open. From the Files of Type list, select AutoCAD drawings (* .dwg). Then select an AutoCAD DWG file, and click Open.
  2. Save the file as an Autodesk Inventor DWG file in the Templates folder.

Create a New Standard

You create a new Standard style based on an existing style you select. Before you edit the style, you remove the old Standard and object defaults styles to avoid confusion when editing the styles later.

  1. In Inventor, click Manage tab Styles and Standards panel Styles Editor to open the dialog box.
  2. In the style list browser, expand Standard at the top of the list, and right-click the Default Standard (ANSI) style. Select New Style from the context menu.
  3. Name the new standard style and click OK.
  4. In the style list browser, double-click the new standard to activate it.
  5. In the style list browser, expand Object Defaults and right-click the Object Defaults (ANSI) style. Select New Style from the context menu.
  6. In the New Style Name dialog, enter a unique name for the new style, verify that Add to Standard is checked, and then click OK.
  7. In the style list browser, right-click the old standard style and select Purge Style and Sub Styles. Click Yes in the Purge Unused Styles and Sub-Styles dialog.

Edit the Standard

  1. Select the new standard in the style list browser.
  2. Click the Available Styles tab.
  3. Select Dimension in the Style Type list, and then specify the dimension styles in the template you want to include in the standard.
  4. Specify Layers and Text in the Style Type list.

Edit the Object Defaults Style

  1. In the style list browser, select the new Object Defaults style.
  2. Find the Linear Dimension object in the Object Type list.
  3. Click the corresponding value in the Object Style column to change the default dimension style for linear dimensions to one of the dimension styles from the template.
  4. Click the corresponding value in the Layer column to change the default layer to one of the template layers.
  5. Repeat step 4 to remap dimension and text objects to use template styles and layers. Remap the rest of the objects that are not dimensions or text to use template layers. (Such objects have no corresponding object styles in AutoCAD, so their object styles can be left alone.)
  6. Click Save to save the Object Defaults style, and then click Done.

Purge Unused Styles

If there are styles you want to keep but you did not select them in Object Defaults, you can select them on the Available Styles tab in the standard to prevent them from being purged.

  1. In Inventor, click Manage tab Styles and Standards panel Purge.
  2. In the Purge Styles dialog, for each style, click the corresponding value in the Purge? column to select or deselect the style to purge.

(Optional) Save to the Styles Library

You save the styles in the template to the Styles library for future use and sharing. Because you created a new standard style and object defaults style, you do not receive styles conflict messages when using this template if you do not save to the library.

Parent topic: To Work with Templates for Drawings