Cut List Folder management in the Weldment Part – CSWP Weldments

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To properly utilize the weldments features for Solidworks an understanding of the cut list structure is required. Once the Weldment feature is added to a part a few changes are made, including a change from “Solid bodies” to “Cut-List” in the feature manager. This cut list can be linked to drawings and passed to a machinist to facilitate the cutting of proper profile lengths. Consolidating items for the cut list is important, a weldment that requires 40 structural components may only contain 3 or four distinct parts. Grouping of identical items and specifications is done through a folder structure as a part of the “Cut-List” feature.

A new weldment part will contain a cut list with all of the items. Each is named and numbered according to the last feature to modify the part . Before a cut-list can be used in a drawing the folder structure must be added. This can be done by right clicking and checking the “Automatic” or “Update”, for the purposes of the CSWP it is most likely that the “Automatic” feature should be used.

Once the “Automatic” feature is click the Cut-List will be organized into folders. A folder is created for each unique part, with a quantity noted in parenthesis. My simple example was a rectangular box with a single cross member which created 4 folders, one each for the length/width/height members and another for the cross member.

If more members are added they will not necessarily get their own folder automatically, despite the name “automatic”. Each item will be added after the folders and items that are not contained in a folder will not propogate out to the drawing Cut-List or BOM. This can be useful if a body which will not require a cut, such as a rivet or weld bead, is added for visual purposes.

Clicking update again will add a new folder to the cut list for any new items. If it matches other items it will be included in that folder. If not it will create a new folder. Folders are named in order and the number of items in each folder is clearly noted in the folder name.

Folders Can be renamed to help orgainze things. The name of the FOLDER will be the “Cutlist Item Name”, this is a field that can be easily added to a Cut List table on a drawing. The name of the actual cut list item (or body) is not as easy to add to a table.

All items in the folder are named based upon the last feature to modify that body (Structrual Member 1). The order within that feature [1] denotes the first item created in the feature, [2] the second and so on. Items can be manually added to folders by dragging and dropping them. For most applications though the drag/drop feature should be avoided as the software does a fairly nice job of grouping items together correctly.

It is important to note that it is not just the profile and length that will create a new folder, a new material will as well. The overall material can be assigned to the part in the normal fashion, by right clicking the material feature in the feature manager, but some items may be a different material.

When a weldment part has bodies that are made of different materials it will be noted below each body. Each body is treated uniquely and the material is one of the fields that is compared before grouping items for the cut list. In the below image two of the members are called out as Aluminum alloy (although welding steel to aluminum in this configuration is not advised). Because each of these items is a different material from the part material an added notation is made in the Cut List and Cut List Folder. This material field can also be used to populate a field for a Cut List BOM on a drawing.