Creating a New Drawing

This task will show you how to create a new drawing with pre-defined views generated from a part.
Open the GenDrafting_part.CATPart document. Make sure no drawing is already open.

  1. From the menu bar, select Start > Mechanical Design.

  2. Select the Drafting workbench.

    The New Drawing Creation dialog box appears with information on views that can possibly be created, as well as information on the drawing standards.

    You can modify the drawing standards. To do this, click the Modify button.
    The New Drawing Creation dialog box will not appear if you did not previously open a CATPart or a CATProduct document.

  3. Select the views to be automatically created on your drawing from the New Drawing Creation dialog box, for example the Front, Bottom and Right icon.

  4. Click OK. A progress bar appears while the views are being generated from the opened CATPart.
Whenever the projected geometry color is the same as the sheet background color, the geometry color is changed to a more visible one, even if the Inherit 3D Colors option is selected in Tools > Options > Mechanical Design > Drafting > View tab. Thus in case of same color of the sheet and projected geometry, the inherited color may not be applied.
The resulting view position will depend on the CATPart you loaded before starting the Drafting workbench. In other words, the views will be positioned according to:
  • a plane you possibly selected in the part.
  • a planar surface you possibly selected in the part.
  • xy coordinates, in case you did not open a CATPart beforehand. In this case, you will only be able to define the drawing standards via the New Drawing dialog box.