Creating a Welding Symbol

You can create a geometry weld symbol between two elements.

Before you begin:
  • Open a drawing representation.
  • If you are an administrator, select the required parameters for welding in the Standard definition dialog box under Annotations > Welding. For more information, see Welding.
See Also
About Welding Symbols
  1. From the Annotation section of the action bar, click Welding Symbol .
  2. Select one or two elements defining the weld to determine the position of the leader anchor point.

    Note: Double reference selection is available only if the first selected element is a 2D geometry.

    Important: In the case of a view associative to a weld specification originally defined in the Weld Design app, select the weld representation.


  3. Move the pointer to position the symbol or you can snap the leader orientation on one of the privileged directions, and position the symbol.
    The leader segment turns to cyan color, indicating the snapping on the privileged direction.
    Note: If the leader is associated to two line references, it can be snapped on the horizontal and vertical directions, and also on the angle bisector line direction between the two line references. In this case, a positional link is created between the leader and the two line references.
  4. In the Welding Symbol dialog box, select the direction for the Weld text side and the Indent line side .

    Important:
    • In the case of a view associative to a weld specification originally defined in the Weld Design app, this dialog box is pre-filled in accordance with the 3D specification. The welding symbol is created associatively to the 3D specification. In this case, the parameters in the dialog box cannot be changed. For more information, see About Welding Symbols.
    • The Indent line side is available only when the welding symbol System-A is selected in the welding parameters of ISO standard.

  5. Enter the values in the required boxes.

    Notes:
    • When you specify the size of weld and length of weld, a new box appears above it for additional information.
    • The engineering symbols can be inserted in all the boxes except the box below plug symbol.

  6. Select the required weld symbol, complementary symbol and finish symbol.
    Notes:
    • The weld symbols are available depending on the selected standard.
    • When an elementary or a supplementary symbol is selected, another pair of these symbols appear above them.
    • When the plug weld symbol is selected, a box appears below it.
    • The staggered (Z) symbol is displayed in the welding symbol annotation only if a text is entered next to the staggered symbol.
    • In the Welding Symbol dialog box, the staggered symbol appears based on the welding staggered display parameter selected in the Standard definition dialog box. For more information, see Welding.
      • Usual: To display the staggered (Z) symbol in the welding symbol annotation.
      • Alternative: To offset the weld symbol on the opposite side of the reference line. Click the Alternative welding staggered display to activate the alternative welding staggered symbol.
  7. Optional: Add complementary indications like a field weld, weld-all-around, or a weld tail.
  8. Optional: Click Import file to import a text file.
  9. Optional: Click Reset to clear all the values.
  10. Click OK.

    The welding symbol is created.



    Note: The values entered in the dialog box are saved as user preference for next usage.
  11. Optional: Modify the welding symbol position by dragging it to the required location.
  12. Double-click the welding symbol to edit it. For example, click the weld text side to change the side of the text.