Bend Allowance, Bend Deduction and K-Factor Tables in SOLIDWORKS

Article by Saeed Mojarad (CSWE) updated June 9, 2017


In this series of blog posts it was discussed what different terms like Bend Allowance, Bend Deduction and K-Factor mean and how we can calculate them for a specific sheet. You can read the previous post: What are Bend Allowance, Bend Deduction and K-Factor? And the post that explains how to calculate them here.

In this post you will see how to use these calculated values in order to make our own SOLIDWORKS Sheet Metal Bend Table.

Bend tables and gauge tables come into play when working with sheet metal parts in SOLIDWORKS. The location where SOLIDWORKS reads these tables from is set in Options > System Options > File Locations.

Select “Sheet Metal Bend Tables” or “Sheet Metal Gauge Table” to see the location where SOLIDWORKS reads the tables from.

SOLIDWORKS Sheet Metal Bend Table File Locations

Bent Table File Locations

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Bend Tables

Bend tables were the original tables used by SolidWorks to pull Bend Deduction, Bend Allowance or K-Factor values for use in calculating the flat pattern. SOLIDWORKS has provided some sample tables that you can use as a reference to make yours. You can find these sample tables under

SOLIDWORKS Installation folder\SOLIDWORKS\lang\english\Sheet Metal Bend Tables

You can simply edit a SOLIDWORKS Sheet Metal Bend Table and enter the values that were calculated in our previous posts to make your own table. You would need a separate bend table for each thickness of material. As an example I modified the sample bend allowance table based on our calculations as shown in the picture below:

SOLIDWORKS Sheet Metal Bend Table data

Bend table data

Using a Bend Table in a Sheet Metal Part

Now to use this table for a sheet metal part, all you need to do is to right-click on Sheet-Metal feature in the design tree and edit the feature. Then under Bend Allowance section select this new custom made table.

The problem with a SOLIDWORKS Sheet Metal Bend Table is that it can only control the Bend Allowance, Bend Deduction or K-Factor but the thickness and radius is still free to be changed manually.

Gauge Tables

Since gauge tables were introduced, all the parameters can be controlled base on the drop down selection which makes life much easier.

So when it comes to actually using these tables in SolidWorks do you use a gauge table or a bend table? The short answer is a gauge table.

When creating your own gauge table, again the best way is to use one of the sample tables supplied with SolidWorks and then just modify the values for your specific application. You can find sample gauge tables under:

SOLIDWORKS Installation folder\SOLIDWORKS\lang\english\Sheet Metal Gauge Tables

You need one separate excel file for each material that you have. You can add extra lines to the table to cover different thickness, bend angles, radii that you use in your company.

The important point when making a gauge table is that you must list the gauges from smallest thickness to largest. I modified the sample K-Factor gauge table based on my calculations in previous post as follows:

Gauge Table Data

Gauge Table Data

Using a Gauge Table in a Sheet Metal Part

To use your custom made gauge table all you need to do is to edit the Sheet-Metal feature and check off the gauge table checkbox in the property manager. Doing so let you to pick your table from the drop down menu. After that you can select the thickness (gauge) and the bend radius. Based on your selection SOLIDWORKS will apply the right K-Factor to your model.

SOLIDWORKS Sheet Metal Options

SOLIDWORKS Sheet Metal Options

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Saeed Mojarad (CSWE)

Saeed Mojarad is an application engineer at Javelin Technologies. He received his B.S from Mazandaran University, Iran; and his M.S. from École de technologie supérieure (ETS), Canada. He has several years of experience using SOLIDWORKS in different industries such as manufacturing and aerospace. Currently located in Calgary, he is helping SOLIDWORKS users all across Canada as a technical support and SOLIDWORKS instructor.