How to show SOLIDWORKS Sub-weldment Components in a Drawing Cut List

Article by Mehdi Rezaei, CSWE updated November 17, 2017

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In SOLIDWORKS, a Weldment model usually includes many numbers of components which show in the cut list table. To reduce the rows in the cut list to a manageable number or to create sub-groups for the model, one can group components and save them under a sub-weldment folder. As a result, the cut list table in Drawings will show only one row for each sub-weldment. At the manufacturing stage, you would need to show all of the components in the cut list including the sub-weldment components. We are sometimes asked, in technical support, “how do I show a SOLIDWORKS sub-weldment in my cut list?” The answer is provided in this article.

The image below depicts a weldment part and its drawing which includes balloons to components plus the cut list table. We are going to select the top frame of this model and create a sub-weldment. Note that components could be selected from feature tree or from the graphics area. To select components in graphics area, you need to activate “Filter Solid Bodies”. Otherwise, faces, edges, or vertices of the components would be selected by clicking on each component. The “Selection Filter” toolbar could be shown all time by checking it off under Tools > Customize > Toolbars or it can be toggled on and off with shortcut key. The shortcut key for Filters toolbar is F5.

Note: To select weldment components in graphics area, the “Filter Solid Bodies” must be activated. Otherwise, only faces or edges of the components would be selectable.

A Sample Weldment Model in SOLIDWORKS

Create SOLIDWORKS Sub-weldment

Once the intended components are selected, right-click on the free space on graphics area and select “Create Sub-Weldment”. As a result, a folder will create in feature tree under cut list folder. Also, the cut list in the drawing environment will change. All subweldment components would show in one row and with the same item upon assigning balloons. Exactly the same as bill of material for a subassembly of a top level assembly. However in case of assembly drawings, the bill of material could be adjusted to show all components whether they belong to a subassembly or not. Despite bill of materials, cut list tables do not have an option to show subweldment components along with the rest of components. This will require a workaround to show sub-weldment components as well.

A Group of Weldment Components Could Create a Sub-Weldment

Insert into New Part

In order to show sub-weldment components, the sub-weldment components need to be inserted into a new part. Either right-click on the sub-weldment folder and select “Insert into New Part”, or activate Filter Solid Bodies and select the components in the graphics area and right-click on free space on graphics area. Then, make sure “Cut list properties” is checked off under properties window on the left. Clicking the green check mark on top of the properties window will open a new part file with the sub-weldment components in it. The image below demonstrates the steps of inserting sub-weldment components into a new part file.

Sub-weldment Members Must Be Selected to Insert into a New Part. Then Cut List Will Show its Members

Finally, the new part must be inserted into the same drawing as the main weldment drawing or maybe into a separate drawing page. The cut-list of this new part will have all the sub-weldment components as demonstrated below.

Sub-weldment Cut List vs. Main Weldment Cut List

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Mehdi Rezaei, CSWE

Mehdi is a Certified SOLIDWORKS Expert (CSWE) and works near Vancouver, British Columbia, Canada