Problem

When inserting a Cut List table into a drawing, if the syntax is incorrect, the cut list will show an expression syntax instead of an evaluated value. This article will go over how to resolve this issue. This can occur for a variety of properties called out by the cut list table.

The cut list table in the drawing is pulling information from the cut list properties in the weldment part file. The cut list properties are accessed in the weldment part file by right-clicking on a cut list item and selecting "Properties".

In the Cut-List Properties window, we can see that the error causes the Evaluated Value for most properties to be the same as the Value/Text Expression.

SOLIDWORKS is unable to calculate a value from the given text expression. Taking a closer look at the text, we can see why. The example text contains quotation mark symbols in locations that make the solver unable to evaluate the expression.  

Where are these extra quotation marks coming from? The entire Rectangular Tube 4" X 3" X .25" string is being pulled from the description of the Weldment Profile Part (part that contains the sketch profile that is used to create a weldment).

Solution 1

The first solution is to change the description in the Weldment Profile Part so that it no longer contains quotation mark characters.

1. Open SOLIDWORKS and go to Tools > Options > System Options > File Locations > Weldment Profiles to check where the Weldment Profile Parts are stored
2. Open the weldment profile part file and go to File > Properties

3. Review the Properties values for syntax errors. In the example below, the quotation marks can be seen in the Description property.

   

4. After removing the quotation marks and saving the Weldment Profile Part, sometimes we also need to edit the Structural Member feature in the Weldment Part and re-select the profile for the changes to take effect.

Now that the description does not contain quotation marks, the cutlist properties in the Weldment Part and cutlist table in the Drawing evaluate successfully

Solution 2

If there are hundreds of weldment profile parts, all with descriptions that contain quotation marks, it would take a long time to go into each weldment profile part, remove the quotation marks, and save. Instead, we can modify a Document Property setting to resolve the issue.

1. Open SOLIDWORKS and open a Drawing with the issue
2. Go to Tools>Options>Document Properties>Weldments
3. Check "Rename cut list folders with Description property value" and click "OK"

With this checked, the cut list items pull the description from the Weldment Profile Part. However, if we uncheck this option, the cut list items are given generic names "Cut-List Item1, Cut-List Item2, etc..." These generic names evaluate the text expression properly, resulting in a successfully evaluated value.

For additional support, existing customers can submit a ticket or new customers can contact Hawk Ridge Systems.