Generating Welding Symbols on a Drawing

You can automatically generate welding symbols and information on a drawing in the Drafting app.

Welds are extracted only in the Drafting view in which the weld section is perpendicular to the view.

In other views, welds are not extracted.

Before you begin:
  • You have the appropriate Drafting license.
  • To create and use generative view styles, clear the Disable generative view style usage option in Me > Preferences > App Preferences > 3D Modeling > Mechanical Systems > Drafting> Administration tab.
See Also
About Weld Lengths in Annotations
Weld Annotations
  1. Open the assembly containing the weld and edit the weld feature. Our example uses a fillet weld.


  2. In the Fillet Definition dialog box, click the Manufacturing tab.
    Multiplicity is set to Single.
  3. Click Cancel.
  4. Create a new drawing.
    You are now in the Drafting app.
  5. Select the xml standard file in the Generative view style dialog box.
  6. From the View Layout section of the action bar, click Front View and select a face on the assembly.

    The preview appears in the Drafting app.



  7. Click on the drawing to generate the front view.



  8. From the Annotation section of the action bar, click Welding Symbol View and select the weld on the drawing.

  9. Click on the sheet where you want to create the annotation.
    The weld annotation is created with the information specified in the weld feature: weld thickness and length values appear.



    Tip: The Welding creation dialog box that appears lets you customize the welding symbol. For more information, see the Drafting User's Guide: Working with Annotations: Working with Symbols :Creating a Welding Symbol: Creating a Weld Symbol.
  10. Click Cancel in the Welding creation dialog box.
  11. Back to the Weld Design context and edit the weld feature, modify its thickness.
  12. Click OK in the Fillet Definition dialog box.
  13. Back in the Drafting app, click Update All .
    The thickness is updated.



    Important: A weld annotation is not associative in position when the weld feature is moved in the assembly.