# Spotlight on Features: Sheet Metal Bend and Gauge table working rules (Part II)

In the February blog we looked at the sheet metal bend and gauge table working rules

This month will be looking what happens when bend or gauge table problems appear and how those problems relate to the working rules.

There are two general types of table problems.

The warning messages (Fig. 1) displayed by SOLIDWORKS are the following: 1) The Bend Table has an Invalid Format.

This message will be displayed only when one of the bend or gauge table rules is broken.

2) The thickness/Bend Radius/Angle of this Bend Fell Outside the Bend table”

This message will be shown when some sheet metal parameter of the part (i.e. Bend Radius, Thickness or Bend Angle) is not contained within the table data limits.

Let’s look at a few problems when we encounter this message. (Fig. 2), shows the user has a part with a 7.5 degree bend angle. The bend table for this particular part has a 15 degrees minimum angle. Therefore, the user should change the table and add a 7.5 degree or a smaller angle to the table. If the user adds a 7.5 degrees angle then the table will use this bend angle parameter. If the user adds a smaller than 7.5 degrees angle, then the system will interpolate between this value and the 15 degrees angle to find the needed parameter. Another common problem is when dealing with the bend table precision. The user must be sure that the values displayed in the table matches the precision in the excel editor. In (Fig. 3), the user has a 0.12 inches Bend Radius. However, when clicking on that specific cell, the precision of the value is actually 0.123 inches (Fig. 4) When using a gauge table, the property manager will display the bend radius value as 0.12 inches (Fig. 5) Therefore, the part will have a 0.12 bend radius. However, when unsuppressing the flat pattern, SOLIDWORKS will read the table and get the actual value (0.123 inches). Because the actual part has a bend radius of 0.12 inches and the system reads the table values as 0.123 inches. The part bend radius value is smaller and hence falling out of the range of the table.

Below we have a more explicit sample of the same problem. The user has inserted a gauge table (Fig. 6) He is using a 14 Gauge value. This has a thickness of 0.0747 inches and a bend radius of 0.031 inches.
The part will be created using these values.

The user then inserts a bend table. When unsuppressing the flat pattern the same message is displayed.

As we can see in Fig. 7, the bend radius for the 0.0747 inches thickness is 0.03125.
This value is larger than 0.031. Hence the problem. Next month we will explore bend calculation tables. #### Mario Iocco

Sr. Technical Customer Support Engineer, SolidWorks, Americas.
Mario Iocco is a veteran CAD user. He started as a Mechanical Engineer first working in 2D with AutoCAD, moving on to 3D using  both SW and some  of the other CAD software on the market. He began his career with SolidWorks over 15 years ago. He started in R&D working on many of the new functionalities developed at the time -eDrawings, Sheet Metal, Weldments, etc. In the last few years, he moved to TS., working closely with VARs, Mario wrote the sheet metal functionality best practice manual, as well as creating hundreds of Sheet Metal Knowledge Base articles. He has presented webinars  on "Sheet Metal Tips and Tricks" and "Sheet Metal Bend Tables". 