Creating a Welding Symbol

This task will show you how to create a welding symbol. You can set text properties either before or after you create the text.
Welding symbols

You can add the following welding symbols according to the dedicated standard.

Name AWS ISO JIS
Back
Corner Flange NA
Edge Flange
Edge
Fillet
HV Flare
V Flare
Inclined joint NA
Melt Thru NA NA
Permanent backing strip used NA NA
Plug
Removable backing strip used NA NA
Scarf NA NA
Seam
Spot
Spot JIS NA NA
Single-bevel butt
Square butt
Single-J butt
Single-U butt
Single-V butt
Single-V butt with broad root face NA NA
Single-bevel butt with broad root face NA  NA 
Steep-flanked Bevel butt NA NA
Steep-flanked V butt NA NA
Stud
Surfacing
Surface joint NA
Consumable
Transparency
Overlay

Complementary symbols

You can add the following contour symbols according to the dedicated standard.

Name AWS ISO JIS
Concave face
Convex face
Fillet weld with smooth blended face NA NA
Flat face
Flush finished NA NA

Finish symbols

You can add the following finish symbols according to the dedicated standard.
 

Name AWS ISO JIS
C
F
G
H
M
R
U

 
Complementary indications
Field weld
Weld-all-around
Weld text side (up or down)
Indent line side (up or down)
Weld tail
Alternative welding staggered display
Reference
Open the Brackets_views03.CATDrawing document.

  1. Click the Welding Symbol icon from the Annotations toolbar (Symbols sub-toolbar).

  2. Select one or two elements defining the weld to determine the position of the leader anchor point.

    Double reference selection is available only if the first selected element is a 2D geometry. 
    You can press the Alt key to orient the annotation in the vertical direction.

  3. Move the pointer to position the welding symbol and then click at the required location.

    The annotation can be snapped in horizontal and vertical directions, or along the bisector of the angle between the two reference elements.

  4. In the Welding symbol dialog box, select the direction for the Weld text side and the Indent line side .
    • In the case of a drafting 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 modified.
    • The Indent line side is available only when the welding symbol display System-A is selected in the welding parameters of ISO standard.

  5. Enter the values in the required boxes.
    • 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 welding symbol, complementary symbol and finish symbol.

    • The welding 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. Add complementary indications like a field weld, weld-all-around, or a weld tail.

  8. Click Import file to import a text file.

  9. Click Reset to clear all the values. 

  10. Click OK.

    The welding symbol is created.

    The values entered in the dialog box are saved as user preference for next usage. 

  11. If needed, 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.
  • If you have selected the Use style values to create new objects option in Tools> Options> Mechanical Design> Drafting> Administration tab, the Welding creation dialog box is pre-filled with custom style values (as defined in the Standards Editor). In this case, Properties toolbars and the Tools Palette are disabled during the creation of the welding symbol.
    On the other hand, if you have not selected this option, the Welding creation dialog box is pre-filled with the last entered values (if any). In this case, Properties toolbars and the Tools Palette are active during the creation of the welding symbol.
  • You can reset the current style values in the Welding creation dialog box at any time using the Reset button.
  • You can close the tail (reference) using a rectangle variable-size frame . For more information about adding frames, refer to Adding Frames or Sub-Frames. 
  • At any time, you can modify the welding symbol. To do this, double-click the welding symbol to be modified and enter the modifications in the displayed dialog box.
  • You can import a plain text file (.txt) to use as a reference (specification, process or other) by clicking the Import File button. 
  • The welding symbol is automatically updated when the drawing standard is switched. For example, from JIS to ISO. During the switch, if a welding symbol is unavailable in the target standard, it is replaced by an underscore.