To Add or Edit Weld Annotations in a Drawing View

Use welding symbols from the model, or create nonassociative symbols for caterpillars and end fills.

What's New: 2019.2

You can manually add weld annotations to a drawing view even if there are no weldments defined in the model. To change a weld annotation, you select the annotation and change values in the dialog box.

The annotations (caterpillar, end fill, and welding symbol) are not associated to weldments in the model file and do not update if the model changes.

If welding symbols or end fills were created in the model, you can retrieve them in the drawing view. Welding symbols and end fills update with changes to the model.

Add or edit welding symbols

Use Welding to create a welding symbol with a leader line. The line type, line weight, color, and gap for the symbol are determined by the weld symbol style.

Tip: If a welding symbol has been created in the model, manually adding a welding symbol creates a copy of the model welding symbol. It does not update if changes are made to the model welding symbol. To create a welding symbol that updates with the model welding symbol, right-click the drawing view, and select Get Model AnnotationsGet Welding Symbols.

If there are no model welding symbols, you can make a nonassociative welding symbol in the drawing view.

On the ribbon, click Annotate tab Symbols panel Welding . In the graphics window, click to set the start point for the leader line. Note: To associate the welding symbol with geometry, move the cursor over the appropriate edge, and then click when the edge highlights. Symbols that are associated with geometry move if you move the drawing view. Move the cursor and click to add a vertex to the leader line. When the symbol indicator is in the appropriate position, right-click, and then select Continue to place the symbol and open the Welding Symbol dialog box. The options in the dialog box are determined by the active drafting standard. (Optional) Select a symbol preset and modify if needed. If no preset exists, modify the settings as described below. Or, set the attributes and values for the symbol. To save the values as a Preset, click Create new preset . Learn more about presets - To Work with Presets Continue placing welding symbols. When finished, right-click and select Done.

To edit a nonassociative welding symbol, right-click a welding symbol, and select Edit Welding Symbol. In the Welding Symbol dialog box, change values as needed, and click OK. Welding symbols retrieved from the model must be edited in the weldment assembly.

Add or edit weld caterpillars

Use Caterpillar to add weld caterpillars to geometry in a drawing view. The caterpillar type, size, angle, and other formatting is determined by the weld bead style.

Tip: To create a caterpillar that updates with the model fillet bead, right-click the drawing view, and click Get Model AnnotationsGet Welding Annotations. If changes are made to the fillet bead in the model, the length of the caterpillar edge updates in the drawing view, but you must manually edit the caterpillar to change the leg length.

If there are no model caterpillars, you can make a nonassociative welding symbol in the drawing view.

On the ribbon, click Annotate tab Symbols panel Caterpillar . In the graphic window, select an edge in a drawing view. In the Weld Caterpillars dialog box, set the edges, start and stop points, direction and type for the caterpillar. If needed, click the Options tab, and then set the size information for the caterpillar. Click Apply to place the caterpillar.

Changing the caterpillar side - Once you have placed the arc legs of a caterpillar on the side of an edge, you can change the side on which they are placed. To do this, select the type for both sides in the Type area of the dialog box before you reselect the single side option. Once you have reselected the single side option, the caterpillar follows your cursor from one side to the other side as you move across the edge in the drawing view.

Changing the caterpillar from an entire edge to Start/Stop - Placing a caterpillar requires that you select an edge. If after selecting the edge you decide that the caterpillar should only display along a portion of the edge click Start/Stop on the Style tab of the dialog box and then select the start and stop points along the edge. The points that you select do not have to be geometric points - they can be approximate locations.

To edit, right-click a caterpillar, and select Edit Caterpillar. In the Weld Caterpillars dialog box, enter new values as needed, and click Apply. Click OK to close the dialog box.

Add or edit weld end fills

Use End Fill to add 2D end fill annotations to geometry in a drawing view. The size and other formatting is determined by the weld bead style.

Tip: To create end fills with model end fills, right-click the drawing view, and select Get Model AnnotationsGet Welding Annotations. If changes are made to the end fills in the model, end fills in the drawing update. If you customized the leg length of a preset type, you must manually edit the size.

If there are no model caterpillars, you can make a nonassociative welding symbol in the drawing view.

On the ribbon, click Annotate tab Symbols panel End Fill. (Optional) Select a symbol preset and modify if needed. If no preset exists, modify the settings as described below. You can save a preset at any time, see Step 7. In the End Fill dialog box, select the end fill type. If needed, click the Options tab, and set the fill pattern or color. Use scale with a pattern to adjust the appearance. To see changes, click Apply. In the graphic window, click to select an edge for the end fill. Move the cursor to position the end fill symbol. When the symbol is in the appropriate position, click to place it on the view. To save as a Preset, click Create new preset . Learn more about presets - To Work with Presets Click Apply to place the end fill and continue adding end fills. Click OK to complete the process. Custom Shape End Fill - To define a custom end fill, follow steps 1-4 above. Then, define the end fill in the graphics area. When done, click Apply or OK.

To edit an end fill, select the end fill on the drawing view, right-click and select Edit End Fill. On the End Fill dialog box, change values as needed or select an applicable preset. Click Apply to apply the changes and continue editing. When finished, click OK to close the dialog box.