Weekly Whole Hog SolidWorks Tip & Trick: Using the “Insert Bends ...

There are many times in SolidWorks that a user would like to take existing geometry and convert it to something that could be formed as a sheet metal part. This type of conversion is common when working with fixtures, but also comes up in places such as coverings, panels and mounting brackets within assemblies. While a long-time user can move between different modeling styles in SolidWorks, some CAD operators feel more comfortable sticking with the regular geometry creation tools that they have become accustomed to already. This weeks tip describes how to transition your solid models to sheet metal models in SolidWorks using the INSERT BENDS command. Depending on how the CAD user starts the sheet metal conversion process, there is an important rule to keep in mind for all sheet metal part creation: UNIFORM THICKNESS - The unifying rule to sheet metal conversion is that the part must have uniform thickness. This applies to both thin-walled parts and parts that have radius’ applied at the corners. The best method of preventing problems during conversion is to use a shell feature to control the overall wall thickness of the model. TIP - Don’t worry about radius values on the corners of your solid part at this point. SolidWorks will add the appropriate bend radius where needed upon conversion of the solid. Our example of a solid part being converted to sheet metal will be a thin-solid that might be used as a fixture for some component in an assembly. The model is shown to the right without any radius applied to the corners and with a wall thickness of 0.105″ identified during the thin-extrusion feature definition. Most users would argue that creating geometry of this nature is without mention, which is true. The definition of the part is simple, as is the abillity to place it correctly in an assembly to locate a component. Adding the sometimes intimidating complexity of sheet metal to the mix however can make this type of model seem like a great challenge for a new user. To ‘magically’ make this part into something that a shop could form, the “Insert Bends” command can be used. This tool is found on the “Sheet Metal” Command Manager toolbar. If you don’t see the Sheet Metal tab, it is simply turned off, and can be activated by right-clicking on any of the existing tabs and selecting it from the pop-up list. Once the toolbar is shown, the “Insert Bends” command is shown below. With Insert Bends selected, SolidWorks asks for a few simple inputs from the operator: Fixed Face - One of the faces of the model must remain stationary. This face will determine the orientation of the part when it is flattened, which really is of no consequence to the operator at this time. Bend Radius - This is the inside radius dimension of your bends. You can enter any value, but Whole Hog would suggest that you talk with a fabricator (or do some online research) to see what some standard bend radius values are. Typically the bend radius is a function of the material type, the thickness of your material and the orientation of the metal grain. Bend Allowance - The manner in which you predict a part to stretch is defined by the bend allowance calculation. SolidWorks offers this calculation to be done by k-factor, bend table, bend deduction, bend allowance and bend calculation. Depending on your fab shop and the dimensional accuracy of your part, you should check with the shop to see what appropriate value to use. A generally safe value for most sheet metal design is a k-factor of 0.45. Auto Relief - This is the way that SolidWorks will treat the corners of your sheet metal part. Tear is a fairly common setting, although rectangular relief is seen on many products as well. Rip Parameters - The final selection box is to define whether any edges will be ripped when converting to sheet metal. This is a way of making a complex shape ‘unfold’ into a single flat piece that can be cut from sheet material. Our simple example does not have any rip edges, but the user can define them if necessary. We will explore rips in a future post on sheet metal conversions. With the bend information defined for this part , SolidWorks will automatically apply the bends and the additional length seen in the flat pattern from the bend allowance from our k-factor.