In this quick tutorial, we are going to show you the steps to add weld beads to an Assembly file in SolidWorks.
The Weld Bead feature allows you to add weld beads and weld symbols to your model. This feature provides a simple graphical representation and does not affect the performance of the model. This feature is not only helpful for adding beads and callouts for welding onto the assembly, but also allows you to calculate the length and material required for the weld. Weld beads are usually added to convey the information to the production team and this weld bead can also be propagated in the drawings.
To add Weld Beads in an Assembly, follow the given instructions:
1. Click on the Assembly Features in Assembly Tab and select the Weld Bead option. Or you can also go to.
There are 3 methods to add weld beads:
1. Using the Smart Weld Tool:
- Under Weld Path, click on the Smart Weld Selection Tool icon.
- Now your cursor will change into a pencil. Drag on the edges that you want to weld and they will automatically be selected.
Note: A weld bead can only involve two components. You cannot define a weld path among three or more bodies or between the faces of one body. Also, components of the same sub-assembly can’t be welded either. Open the subassembly document to add the weld bead.
2. Using the Weld Geometry option:
- With the Smart Weld Selection Tool turned off, under the Weld Selection menu, select Weld Geometry.
- Select the faces that you want to weld together.
Tip: Gaps between faces are supported.
3. Using the Weld Path option:
This option allows you to select the edges which you want to weld. Gaps between edges are not supported. Edges must lie on the surface of a body.
- With the Smart Weld Selection Tool turned off, under the Weld Selection menu, select Weld Path.
- Select the edges that you want to weld by clicking on them.
Tip: Click on the New Weld Path button to create additional weld beads. You do not need to click New Weld Path if you use the Smart Weld Selection Tool.
Tip: If Tangent Propagation is enabled then all the edges that are tangent to the selected edges will be welded.
- Click Define Weld Symbol to create and edit the weld symbol to be used for the selected weld.
- From / To Length: If you don’t want to weld entire edges then the length of the weld bead can be specified in this option by giving the start point of the weld and the weld length.
- Intermittent Weld: In this option intermittent welds can be created. These are not continuous but discrete welds (See the image attached below for example). The inputs are given either of the two ways:
- Gap and weld length
- Pitch and weld length
3. Click on the Green Checkmark to create the weld beads and symbols.
Tip: If the weld beads or symbols are not visible go to the drop-down symbol present along with the Visibility icon and select Show Weld Beads. If it’s still not showing make sure the Visibility icon is not selected (it will look like it’s pressed in if it is selected).
How can I edit the welds I just created?
After creating the Weld Beads, a Weld Folder is automatically generated in the Feature Tree. It contains all of the Weld Bead features and properties which can later be imported into a Drawing if needed.
To edit any of the welds, right-click on the weld you want to edit and select Edit Feature.
To find the properties of these welds, right-click on the Weld group and select Properties. You can view all types of information from Weld Material and Process to Total Welding Time and Cost.