Generating a New Drawing

You can generate a new drawing from a 3D representation.

You can also choose a suitable method to create a reusable or an aggregated drawing.

It is also possible to generate a stand-alone drawing representation. See Creating a Drawing Interactively.

This task shows you how to:

Before you begin:
  • Open a 3D shape representation and its product structure.
  • Select Always check that the range of the drawing matches the represented product check box in Me > Preferences > App Preferences > 3D Modeling > Mechanical Systems > Drafting > Drawing, under Drawing Generation.
See Also
Using Drafting with the Design Range Management

Generate a Drawing Using Add > Content

You can create a new drawing using the Add > Content command.

  1. In the top bar, select Add > Content or press Ctrl+N.

    Tip: You can also right-click an assembly or sub-assembly and select Insert > Drawing to create a drawing that can be automatically inserted in the current assembly. In this case, an empty drawing is automatically inserted as a reusable representation under the active product, and it is not set in editing mode.

    The New Content dialog box appears to list the Favorites and the Most Recently Used objects.
  2. Right-click Drawing in the list and select Set attributes at creation.

    This allows you to define the drawing parameters before its creation. However, if you do not select this option, the drawing is initialized with the default parameters, (these parameters are: standard, sheet style, sheet orientation, generative view configuration - if applicable, product attachment).

  3. Click Drawing.
    The Drafting app is loaded and an empty drawing representation is created. The first empty sheet, Sheet.1 is created in the tree. The drawing is inserted in the product.

    However, if you had selected Set attributes at creation in the context menu of Drawing, then, the Drawing dialog box appears allowing you to define the drawing parameters.

  4. In the Drawing tab, give a title for your drawing, and a description. By default, a name drwXXX (where XXX is a number) is specified. For more information about the Drawing tab and general representation attributes, see 3DEXPERIENCE Platform User's Guide: Other Services: Add: Creating New Content.
    Tip: Once you create the drawing representation, you can modify its name by right-clicking the drawing in the tree, and then selecting Properties.
  5. Select an appropriate range in the Design Range list.
    If the ranges of the drawing and that of the product/3D area parts are not matching, the Entry creation failed message appears and the drawing is not generated.
  6. Select the Drawing Information tab.
    This tab lets you define various information related to your drawing.
  7. Select a standard.
  8. Select a sheet style. The Sheet Style section displays the corresponding values for:
    • Sheet format
    • Paper size
    • Global scale
  9. Choose the orientation: Portrait or Landscape.

    The last selected standard, sheet style, and orientation are used by default when creating a drawing.

  10. Select whether you want to create an empty sheet or a sheet prefilled with certain views from your product:
    • All views
    • Front, bottom, and right views
    • Front, top and left views

    If the ranges of the drawing and that of the product/3D area parts are not matching, the message Current range does not allow view generation is displayed in the select views list.

  11. Select the Insert drawing in [open product's name] option to insert the drawing in the current product.

    By default, this option is selected.

  12. Click OK.

    The View Creation Wizard dialog box appears. It disappears as soon as the view creation process is completed.

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

Generate a Drawing Using the Compass

You can generate a drawing using the Compass in the top bar.

From the Compass, click Drafting to create a stand-alone drawing representation.

In this case, if the range of the drawing and that of the product is not compatible, a warning message of Scale compatibility problem appears in the 3D View Extraction dialog box.

For example, if the product/3D area part is of large range, and the drawing preference is defined at normal range (or vice versa), then the message Scale compatibility problem appears.

The following two scenarios are possible based on whether you have specified the attributes at creation:

  • If you have not specified the attributes at creation, use the following steps:
  1. Click OK in the 3D View Extraction dialog box.
    The drawing range is automatically adapted to the range of the product/3D area part (regardless of the range stored as a preference in Me > Preferences > Common Preferences > Parameters, Measures, and Units > Units > Design Limits, under Design Range for new Parts and Products) and the drawing is created.
  2. Click Cancel.
    It uses the default range and therefore the Entry creation failed message appears. When you click Close, the message dialog box closes without generating the drawing.
  • If you have specified the attributes at creation, use the following steps:
  1. Click OK in the 3D View Extraction dialog box.
    The Drawing dialog box appears to display the drawing preference range in the Design Range list. You can change the range to adapt to the product/3D area range.
  2. Click OK in the Drawing dialog box.
    The drawing is generated matching with the product/3D area part range.
  1. Optional: Click Cancel in the 3D View Extraction dialog box.
    The Drawing dialog box appears to display the drawing preference range in the Design Range list. In this case, the Drawing Information tab displays the message Current range does not allow view generation.
  2. In the Drawing tab, change the drawing range to make it compatible with the product/3D area in the Design Range list.
  3. Click OK in the Drawing dialog box.
    An empty drawing is generated matching with the product/3D area part range.

If the ranges of the drawing and that of the product is compatible, the Drafting app is loaded and a drawing representation is created. The first sheet, Sheet.1 is created in the tree and also displayed in the Sheet Browser. The drawing is inserted in the product as a reusable representation.

Create a Reusable Drawing

You can create a reusable drawing that can be instantiated under several products.

  1. From Me > Preferences > App Preferences > 3D Modeling > Mechanical Systems > Drafting, expand Drawing, and under Drawing Creation, select the Make the drawing reusable check box.

    This check box is available for selection only when Insert drawing in represented product or part check box is selected.

  2. Create a drawing using any of the following methods:
    • From the Compass, click Drafting.
    • In the top bar, select Add > Content and select Drawing in the New Content dialog box.
    • From an existing 2D layout representation, use Drawing Batch Utility. For more information, see 3D Modeling Apps : Mechanical Systems: 2D Layout for 3D Design User's Guide: Working in Integration with Drafting: Generating Layouts and Drawings using the Batch Monitor.
    A reusable drawing is created.

    The reusable status symbol is visualized in the drawing editor window.

  3. To reuse an existing aggregated drawing, right-click the drawing in the tree and select Make reusable representation.

    An aggregated drawing can be reused but a reusable drawing cannot be aggregated.

Lock a Drawing

You can lock a drawing.

  1. In the Compass, click Social and Collaborative Apps and select Collaborative Lifecycle.
  2. From the Collaboration section of the action bar, click Lock .
  3. In the tree, select a drawing.
    The drawing is locked. This drawing can be edited only by the current user.
    Note: The locked status symbol is visualized in the drawing editor window.

Create an Aggregated Drawing

You can create an aggregated drawing that is aggregated within a single product and cannot be reused with other products.

In the context of a product, right-click the product in the tree and select Insert > Drawing.
An aggregated drawing is created under the product. The drawing node is added to the tree with an icon.
Note: A drawing created by this method is aggregated irrespective of the selection of Make the drawing reusable check box in Me > Preferences > App Preferences > 3D Modeling > Mechanical Systems > Drafting > Drawing.