When working in SOLIDWORKS to create sheet metal designs, we will often need to know three important values:
- The sheet metal wall thickness
- The sheet metal default bend radius
- The bend allowance/bend deduction of the sheet metal (specified in K-factor)
By configuring and utilizing a sheet metal gauge table, we can speed up the process of selecting the correct wall thickness (based on gauge value) and selecting the correct bend radius (based on available tooling).We can also automate the process of selecting the appropriate K-factor.
Sheet Metal Wall Thickness
We often see the specification for sheet metal wall thickness represented as a gauge value. Some examples are 10ga, 12ga or 16ga. But what do these gauge values translate to, in terms of sheet metal wall thickness? In order to answer this question, we often need to look up the values in a table.
Figure 1. An example of a reference table for looking up sheet metal thickness based on gauge size and material. Originally posted at www.unc.edu/~rowlett/units/scales/sheetmetal.html.
As we can see in Figure 1, the gauge value number will be translated to a specific wall thickness. This wall thickness will be different, depending on the material being used. These differences can be hard to keep track of, and mistakes can occur when looking up the value and manually typing this value into SOLIDWORKS.
Sheet Metal Bend Radius
The second important number when creating sheet metal designs is the bend radius value. The bend radius of a sheet metal design will be based on the wall thickness of the part and the tooling that is available in house.
Figure 2. A section view of a typical punch and die set used to create sheet metal bends.
Figure 2 shows us a typical punch and die set used to bend sheet metal. This punch and die set would be mounted in a press. The V-die would be mounted on the lower part of the press, and the punch would be mounted on the upper part of the press. The flat sheet metal would be positioned between the punch and the V-die, and the press would be forced closed, forming a bend in the sheet metal.
The punch and V-die will each have a radius at their peak, and these radii will cause a specific bend radius to be formed in the sheet metal. This technique (known as bottom bending) is just one of many methods available to create a bend radius in a sheet metal design.
Regardless of the bending method, a question that will often be asked by the designer is “What bend radius should I be using?” The answer to this question will be based on the thickness of the sheet metal and the available tooling being used in the bending process.
Bend Allowance/Bend Deduction
The third and final question that a SOLIDWORKS designer working with sheet metal will have is “How is the metal stretching/deforming in the bend region?” The phenomenon of sheet metal stretching in the bend region is often referred to as “bend deduction” or “bend allowance.” There are many techniques available to calculate what the “bend deduction” or “bend allowance” should be in these bend regions, but one of the most versatile is known as K-factor.
We could spend an entire blog describing the various options/techniques used in calculating the appropriate value to represent the stretching of sheet metal in bend regions. Instead, we will simplify this area of the blog by agreeing to work with a K-factor value of 0.5.
Sheet Metal Gauge Tables
A great tool available to SOLIDWORKS sheet metal users is the “Sheet Metal Gauge Table.” In this table, users can configure a Microsoft Excel spreadsheet to represent the appropriate sheet metal wall thickness, based on material and gauge values. Users can also specify the available default bend radius based on available tooling. Lastly, users can specify the appropriate K-factor to represent the stretch of the sheet metal in the bent corners.
For today’s example, we will create three sheet metal gauge tables representing the following materials and gauge values:
Figure 3. A table of different materials, gauge thicknesses and default radii.
In Figure 3, we can see a table that might be present in a sheet metal shop. Without a sheet metal gauge table in SOLIDWORKS, whenever we create a sheet metal model, we would have to reference this table and manually type the values into SOLIDWORKS.
We are now going to create three different tables in Excel, each one representing a different material.
The tables will need to be formatted in the following layout:
Figure 4. An Excel spreadsheet layout of a standard steel sheet metal gauge table.
Figure 5. An Excel spreadsheet layout of a galvanized steel sheet metal gauge table.
Figure 6. An Excel spreadsheet layout of an aluminum sheet metal gauge table.
In Figures 4, 5 and 6, we can see the appropriate Excel layout for a sheet metal gauge tablet utilized by the SOLIDWORKS software. Keep in mind that once you make one Excel spreadsheet, you can “save as” and change the values for the next material.
We will save all of these Excel spreadsheets into one folder. I will use a folder in my C drive.
Location of the sheet metal gauge tables in an Excel format.
Now that we have saved the Excel spreadsheets into one single folder, we need to point to this folder in the SOLIDWORKS software. We launch the SOLIDWORKS software, and choose OPTIONS>SYSTEM OPTIONS>FILE LOCATIONS. From the pull-down menu, we choose “Sheet Metal Gauge Tables” and then point to the appropriate folder.
Pointing SOLIDWORKS to the folder containing the sheet metal gauge tables.
Next we will utilize our sheet metal gauge tables in a new SOLIDWORKS sheet metal design.
Using Sheet Metal Gauge Tables in SOLIDWORKS
We have now created the sheet metal gauge tables in Excel in the appropriate format. We have saved the tables into a folder in Windows, and we have pointed SOLIDWORKS to this folder. We are now ready to use these sheet metal gauge tables. Our sheet metal design will use the following specifications: 10ga Aluminum U-Channel with the dimensions 1.5 x 6 x 10 inches long.
We will start by creating a simple sheet metal design with a three-line sketch.
Simple three-line sketch to test our sheet metal gauge tables.
Next we will choose the command Base Flange/Tab from the sheet metal toolbar.
Beginning the Base Flange/Tab command.
We will now input a depth of 10 inches for our sample sheet metal part.
We set direction 1 to utilize a blind depth of 10 inches.
At this point, we would have to answer our three questions from above:
- What is the wall thickness for 10ga aluminum?
- What should I use as a bend radius?
- What is the K-factor?
We have agreed that we will be using a K-factor of 0.5, so let’s focus on the other two questions.
Without a SOLIDWORKS sheet metal gauge table, the answers to these questions would require research—often time-consuming research. We would have to look up the values for wall thickness and radius and would have to enter them into SOLIDWORKS manually. With a sheet metal gauge table, the process is simplified to just a few clicks.
First, we choose the option to use a gauge table.
Choose the check mark to use a gauge table.
Next we use the pull-down menu to select the appropriate table. In our case, we will use the table for ALUMINUM-INCH.
Choose the appropriate sheet metal gauge table.
Next we simply need to choose the specified gauge of 10.
Figure 7. Choose the specified gauge value.
As we can see in Figure 7, we simply need to choose “10 Gauge,” and the appropriate wall thickness (“0.102 in”) is automatically selected. Of course, if we selected a different sheet metal gauge table for a different material (for example, galvanized steel), the wall thickness for “10 Gauge” would be a different value.
Lastly, we choose our desired default bend radius.
Figure 8. Selecting a bend radius from predefined choices.
In Figure 8, we can see that we only have three available choices for a default bend radius. These choices will be defined in our sheet metal gauge table based on available tooling and material wall thickness. This is a great time-saver because it ensures that the SOLIDWORKS designer will not inadvertently create a model with a bend radius that we cannot manufacture with available tooling.
We can now hit the green checkmark and move forward with our sheet metal design, confident that we are using the correct wall thickness and an appropriate bend radius.
By utilizing a SOLIDWORKS sheet metal gauge table, we can save time by eliminating the step of looking up sheet metal gauge values based on different materials. We can also ensure that an appropriate sheet metal bend radius is utilized in the design process and that this bend radius can be achieved in the manufacturing processes. This can also be a great time-saver and can help us get our products to market faster by eliminating the common mistake of using a bend radius that is unrealistic.
Remember that we can always add information to an existing SOLIDWORKS sheet metal gauge table (by editing the Excel spreadsheet), including new gauge sizes and new bend radius values. We can also take one sheet metal gauge table and “save as” to create a new gauge table for a new material.
About the Author
Tobias Richard is a SOLIDWORKS elite applications engineer from Philadelphia. He has been working with SOLIDWORKS software since 1998 and has been providing training, technical support and tips and tricks since 2001.