To Use Model Weld Annotations in a Drawing

How to add them and control their update behavior.

Welding symbols and annotations from a weldment model can be automatically added to a weldment drawing view when it is placed. When you use model weldment annotations, they are associated with the model and update when the model is changed.

You can also add weldment annotations to an existing drawing view.

Tip: If a welding symbol or end fill was created in the model, manually adding a welding symbol or annotation in a drawing view creates a copy. It does not update if changes are made to the model welding symbol or end fill.

• To create a welding symbol that updates with the model welding symbol, right-click the drawing view and select Get Model AnnotationsGet Welding Symbols.
• To create an end fill that updates with model end fills, right-click the drawing view and select Get Model AnnotationsGet Welding Annotations.

If there are no model welding symbols or end fills, you can make a non-associative welding symbol or end fill in the drawing view.

Create reusable weld symbols using Presets

You can create reusable weld symbols and end fills using the Presets feature. To learn how to use presets see: To Work With Presets.

Add weldment annotations when creating a drawing view

When you place a drawing view of a weldment model, you can add welding symbols and annotations from the model. The assembly must be active in the weldment assembly to access its weld annotations. If necessary, on the Quick Access toolbar, click Return to exit the weldment environment.

On the ribbon, click Place Views tab Create panel Base . On the Component tab, set up the view: Specify the weldment model. Select the view orientation from the list or click Change View Orientation to set up a nonstandard view. Specify the scale, label information, and display style. In the Weldments box, select Welds. On the Options tab, in the Display box, select Model Welding Symbols, Weld Annotations, or both. In the graphics window, move the preview to the desired location, and then click to place the view.

Add model weldment annotations to a drawing view

You can add model welding symbols or annotations to an existing drawing view of a weldment.

1. Select the view in the browser or graphics window.
2. Right-click, and then select Get Model Annotations from the menu.
3. Select either Weld Annotations or Welding Symbols.

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 will 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 non-associative welding symbol in the drawing view.