Solid Edge

Process-Specific Weldments

1 Jan, 2003 By: J. Fred White

The Weldment environment in Solid Edge provides a set of commands that are tailored for the efficient construction of a weldment. Weldment is not a standalone product; it is an environment in the Solid Edge suite (similar to Solid Edge Part, Sheet Metal, Assembly, and Draft). Weldments are created using an existing assembly document, such as the one shown in Figure 1, as the basis for the new weldment document.

Figure 1. Creating a new weldment in Solid Edge usually begins with an existing assembly document that serves as the basis.

Creating a Weldment

Use the Weldment command on the Insert menu to select an assembly document. The Weldment Parameters dialog box allows you to select the parts in the assembly that you want to include in the weldment--including all the assembly parts in the weldment isn't necessary. For example, you may have placed a shaft part in the assembly to assist you in designing the assembly but not want to include the shaft in the weldment document. The parts you select are inserted in the weldment document so you can add weld-related features and labels.

The Feature PathFinder tab on the EdgeBar tool is divided into the following four process-specific categories that correspond to how weldments are created and modified in Solid Edge:

  • Managing the components in the weldment
  • Preparing the components for welding
  • Adding weld-bead material and weld labels
  • Machining the weldment

Managing the Components

The Weldment Components section on the Feature PathFinder tab displays the list of components included in the weldment. The individual parts in a weldment are associative part copies of the original part documents and behave similarly to the parts in an assembly document: they are separate solid bodies and you can control the display of the individual parts.

You can use Show and Hide on the shortcut menu to control the display of the individual parts in the weldment. You can also use the Show All Weldment Components and Hide all Weldment Components on the shortcut menu to control the display of all parts in the weldment.

If changes are made to the parent assembly or any of its parts, the symbol adjacent to the assembly listing in Feature PathFinder changes to show that the weldment is not up-to-date with respect to its parent assembly. To update the weldment, select the assembly listing in the Components section, and then click the Update Link command on the shortcut menu.

When creating weldments, you often need to prepare the part surfaces first. For example, you may need to chamfer the edges where parts are welded together. The Surface Preparation button on the Feature PathFinder tab activates commands that allow you to construct chamfers, cutouts, holes, and so forth. When constructing profile-based features, such as cutouts and holes, you can specify which parts in the weldment the feature will affect. After you have drawn the profile and defined the feature extent, the Select Parts Step allows you to specify the parts from which you want to remove material. Any parts that lie within the range of the profile and extent are automatically selected. Selecting the parts automatically saves considerable time when working with large assemblies. If you do not want to remove material from all the selected parts, you can hold down the CTRL key and click any highlighted parts to remove them from the select set.

Adding Weld-Bead Material and Weld Labels

The Weld Beads button on the Feature PathFinder tab activates commands you can use for adding weld-bead material. You can construct fillet welds, protrusions, revolved protrusions, and swept protrusions that represent weld bead material. When you add weld bead material, the bead volume is used when you calculate the physical properties of the weldment.

The Fillet Weld command adds weld-bead material based on two sets of surfaces you define. The Fillet Weld Options dialog box allows you to define the fillet weld characteristics you want. For example, you can define the size and shape of the fillet by specifying the setback distance properties and define the weld symbol characteristics for the fillet weld. Weld-bead material can also be defined using the protrusion commands on the Features toolbar when the Weld Beads section is active.

You can use the Label Weld command to label the edges you want welded together. The Label Weld Options dialog box allows you to define the weld symbol attributes you want. The edges you label will display in the active Construction color. This color change makes it easier for you to see which weld-bead protrusions still require weld-label attributes. The Label Weld command will also compute the bead volume for physical properties calculations.

Stitch Welds

You can use the Stitch Weld command on the Features toolbar to modify an existing fillet weld or a weld bead protrusion to create an intermittent weld.

When you create a stitch weld feature, you first select a weld path, which can be the edge of a fillet weld, or the edge of the weld bead protrusion you labeled. After you select the path, you select the start end of the stitch weld. You can use the Stitch Option list on the SmartStep ribbon bar or the Stitch Weld Options dialog box to specify the stitch definition you want. The options are Stitch, Stitch + Offsets, and Offsets Only.

You can also use the Stitch Weld Options dialog box to define the stitch-weld properties. For example, when you set the Stitch + Offsets option, you must also specify the start offset length (A), bead length (B), gap length (C), and end offset length (D) on the Stitch Weld Options dialog box, as shown in Figure 2.

Figure 2. The Stitch Weld Options dialog box allows you to define the stitch-weld properties. In this case, after selecting the Stitch + Offsets option, you specify the start offset length (A), bead length (B), gap length (C), and end offset length (D).

Post-Weld Machining

You can also define post-weld material removal features, such as cutouts, holes, and so forth. As with the surface preparation features, you can use the Select Parts Step to specify which parts the feature will modify.

Creating Drawings

You can create a drawing of a weldment and its component parts in the Draft environment. When creating a drawing for a weldment, you can also create drawing views that document the process-specific stages of the weldment process. In addition, the Weld Symbol command allows you to extract weld-symbol labels defined in the weldment into your drawing. When you set this option, drawing view edges that have weld labels applied in the weldment document are highlighted so you can extract the labels into the drawing.


The process-specific approach makes it easier to create weldments in Solid Edge because only the commands you need are active. And as you add features to your weldment, the features are added to the proper process-specific category in Feature PathFinder, making it easier to evaluate and edit the weldment later.

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