# Understanding sheet metal flat pattern and folded mass specifications

In SOLIDWORKS 2016 we implemented an additional way to view the weight of a sheet metal body. This new property is called “Flattened Mass.” (Fig. 1.)

A sheet metal body has a folded state and a flat pattern (flatten) state. In the past, the custom property mass of a sheet metal body referred to its folded state. Some customers did not know which weight we were offering when it came to the definition of custom properties.

In (Fig.2) we see a Power Supply box in the folded state.

By checking the mass property reported by SOLIDWORKS, you see that its weight is 155.49 grams (about 0.34 pounds). (Fig. 3)

If you unsuppress the flat pattern feature (Fig. 4.)

Now check the mass property in the same way, you see that this is 153.24 grams (0.33 pounds) (Fig. 5)

The weight difference (155.49 gr. vs 153.24 gr.) is very small –about 1.5 percent. However, we have customers who create some electronics components using precious metals. A very small weight variation can make a significant cost difference.

Why would the folded and flatten sheet metal vary in weight in SOLIDWORKS?

In “real life” parts don’t have 2 weights. However, SOLIDWORKS is a modeler and things are represented a bit differently. When a material is bent, the bent area gets deformed and stretched. The stretch varies according to the material, the bend radius, bend angle, etc. To account for that stretch, SOLIDWORKS applies “Bend Allowances.” These bend allowances are only applied to the flatten state. This simulates the “stretching” that occurs during the real bending of the part. Hence, in general, the surface area –and weight — of a flatten body is slightly less than the same body in its folded state.

As you can see in (Fig. 6), the surface area of the folded body is 118,406 versus 116,710 square millimeters. This produces the weight variance between the twos states.

Which weight is the real weight?

Most of the sheet metal designs created with SOLIDWORKS are created feature by feature. Once the part is completed, you can unsuppress the flat pattern and get to the flatten state. This is why the flat pattern feature is at the end of the feature tree. However, most real sheet metal parts are started from a flatten body. Hence the “real” weight of a sheet metal body is on the flatten body.

Be aware though, that the above answer may not always be right due to the modeling capabilities SOLIDWORKS provides. For example, you have the capability to create features only in the flat pattern. These features exist only in the flatten state and produce a larger discrepancy between the folded and flat pattern weight

In other cases, we can get the opposite situation, features created in the folded state like PEMS, gussets or form tools can be removed from the SOLIDWORKS flat pattern. It is always good to assess your specific situation in order to consider which one is the most approximate weight.

#### 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".