New Drawing of a Model

Create a new drawing of a part or assembly.

Drawing Label

• When you create the first work drawing, the drawing will inherit some of the model's archive data.
• If you edit the model's archive data, the changes will not be updated to the model drawings.
• The label of the first drawing is the same as the label of the model.
• To the next drawings is added number label.

  For example:

  

  The number of drawings is not limited.

Create a New Drawing of the Model

1. Open a part or an assembly in the working window.
2. If necessary, activate a certain configuration of a model, which you wish to create a new drawing.
3. Do either of the following:
   • Double-click Drawings in the tree.
   • Move the cursor on Drawings, and select the context-sensitive function New Drawing.
4. Select the properties of the new drawing in the New Drawing dialog box.

   New Drawing dialog box

   For example:

   • Projection. The default setting is Eur, and the alternative is USA. Select the parallel projection or indicate the projection in the model by clicking Select a and selecting the face.
     
   • Other projection: Select the projection, Perspective, for example. In the case of an assembly, you can select Explosion etc.
   • Select from model: Indicate the model face to define the projection.
   • If the model is a sheet metal part, you can select Automatic Dimensioning. Select Settings.

     Automatic Dimensioning
     Automatic Dimensioning Settings

5. Drawing mode: Select OpenGL Shading + Wire Frame, for example.
   • Select the lines to draw in the drawing: Center Lines, Hidden Lines etc.
   • Select how to draw the lines: As Shape Lines, for example.
6. Select Advanced: The selected drawing mode defines the available choices.

   For example, the OpenGL Shading mode opens a dialog box, where you can select properties.

   

7. Click OK.
8. Save the drawing with the File> Save function.

   The image below displays the location of a drawing's projections in relation to each other when using the one-flip method (default). The projection line will be highlighted when the cursor is near the projection area. The projection line is not drawn on a printout.

   The program names the drawing with the projection names: VIEW1, VIEW2 etc. The name of the projection features the name of the part/assembly from which the drawing was made as a prefix.

   The projection names are presented in the Drawing-tree, if you double-click the drawing in the feature tree of the Part or Assembly.

   

   Projections in a drawing: