What the error looks like:
Inserting a cutlist table into a drawing, you may have come across this situation:
The length column shows an expression syntax, instead of an evaluated length value. This can occur for a variety of properties called out by cutlist table.
The cutlist table in the drawing is pulling information from the cutlist properties in the weldment part file. The cutlist properties are accessed in the weldment part file by right-clicking on a cutlist 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 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 create a weldment). To find out where the Weldment Profile Parts are stored, go to Tools>Options>System Options>File Locations>Weldment Profiles. The folder listed here contains a subfolder structure with the Weldment Profile Parts.
Opening the Weldment Profile Part corresponding to this Weldment Part and going to File>Properties, we can see that the description property is Rectangular Tube 4" X 3" X .25". We found the root of the issue.
There are two ways to resolve this issue, as detailed below.
The first solution is to change the description in the Weldment Profile Part so that it no longer contains quotation mark characters. After removing the quotation marks and saving the Weldment Profile Part, you may have to edit the Structural Member feature in your 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
What if we have hundreds of weldment profile parts, all with descriptions that contain quotation marks? It would take a long time to go in to each weldment profile part, remove the quotations marks and save. Luckily, there is another solution.
In Tools>Options>Document Properties>Weldments, there is an option labeled Rename cut list folders with Description property value.
With this checked, the cut list items pull the description from the Weldment Profile Part. However, if you uncheck this option, the cutlist items are given generic names "Cut-List Item1, Cut-List Item2, etc...". These generic names evaluate properly the text expression, resulting a successful evaluated value.
If you have any questions regarding this article, please contact technical support at US: 877.266.4469 CAN: 866.587.6803.