Generating a New Drawing

You can generate a new drawing from a 3D representation. It is also possible to generate a standalone drawing representation.

In this scenario, the product structure containing the 3D Part is currently open, which lets you aggregate the generated drawing to this product.

Before you begin: Open a 3D Part representation and its product structure.
Related Topics
Defining a Sheet

  1. Click Start in the Bar, then select Mechanical > Drafting.

    Tip: From the menu bar, you can also select PLM Access > Drawing... to create a standalone drawing representation, or PLM Access > New... to create a product containing a drawing representation. You can also right-click an assembly or sub-assembly and select Insert > Drawing to create a drawing that will be automatically inserted in the current assembly.

    The Drawing / Representation DS dialog box appears.



  2. In the Drawing tab, optionally specify the representation kind, enter a name for your representation, and a description. By default, a name RepresentationX (where X is a number) is specified. For more about the Drawing tab and general representation attributes, refer to Infrastructure User's Guide: Creating an Object.

    Tip: Once the drawing representation is created, its attributes can be modified by selecting the drawing from the specification tree, then Edit > Properties.

  3. Click the Drawing Information tab.

    This tab lets you define various information related to your drawing.

  4. Select a standard.

  5. Select a sheet style. The Sheet Style section displays the corresponding values for:


    • Sheet format.
    • Paper size.
    • Global scale.

  6. Choose the orientation: Portrait or Landscape.

    Important: The last selected standard, sheet style and orientation will be used by default when creating a drawing.

  7. Select whether you want to create an empty sheet or a sheet pre-filled with certain views from your product:


    • Front, left, right, bottom, top, rear and isometric views.

    • Front, bottom and right views.

    • Front, top and left views.

  8. Clear the Insert drawing in [open product's name] option if you do not want to insert the drawing in the current product. This option is selected by default.

    Note: Two types of representations, shared or aggregated, are created depending on the availability of the option Insert drawing in [open product's name].

    • Shared representation: If you use any one of the following commands, then the Insert drawing in [open product's name] option is available and selected and the new drawing will be inserted in the product as a shared representation:
      • Start in the Bar, then select Mechanical > Drafting
      • PLM Access > Drawing...
      • PLM Access > New... > Drawing
    • Aggregated representation: If you use Insert > Drawing command from the contextual menu on the product or the 3D shape, then the option Insert drawing in [open product's name] is not available and, in this case, the drawing will be inserted in the product/3D shape as an aggregated representation.

  9. Click Finish. The View Creation Wizard dialog box appears. It will disappear as soon as the view creation process is completed.

Important: You can cancel the creation of multiple views during the process by clicking the Cancel button. This stops the creation of views that are not yet computed. However, the view which is being computed when you click the Cancel button is fully computed. For this reason, clicking Cancel has no consequence when creating or updating a single view.