SolidWorks Sheet Metal has a lot of useful and time saving features. One benefit is the ability to create a flat pattern of a complex sheet metal shape. This tutorial will cover setting up the sheet metal properties, as well as using “Edge Flange” and “Sketched Bend” features.
Turn on the “Sheet Metal” tab if it does not appear. To do this, right click any of the tabs and select sheet metal.
Sheet Metal Properties
Select Base Flange/Tab to begin a sketch of the sheet metal part. Unlike most features, a closed sketch is not required. A base flange sketch can be a single line, resulting in a flat sheet. Alternatively, the entire shape can be made in a single sketch, refer to the screenshot at the end of the tutorial for an example.
In the Base Flange property manager, there are many options. There is an option to use the material sheet metal parameters, these parameters can only be applied to custom materials.
The next section relates to direction, the end condition options are the same as those for an extrude. Refer to the tutorial on “How to extrude at an angle in SolidWorks?” for a detailed explanation of the different types of end conditions. Similar to extrude, the directions cannot be selected and are normal to the sketch plane.
Gauge & Bend Tables
The “Sheet Metal Parameters” and “Bend Allowance” sections can either be filled out manually or linked to tables. SolidWorks provides some tables, they can be found in the directory “C:\Program Files\SOLIDWORKS Corp\SOLIDWORKS\lang\english”, in folders called “Sheet Metal Gauge Tables” or “Sheetmetal Bend Tables”. Their locations can be confirmed from “File Locations” of the system options, under “Sheet Metal Bend” and “Table Sheet Metal Gauge Table”.
Alternatively, the sheet metal parameters can be set manually, input a thickness and bend radius. Ensure that the bend radius is not less than that of the material thickness.
The Gauge table can be selected directly from the drop down list. To select a specific bend table, set “Bend Allowance Type” to “Base Bend Table”, and then select one from the drop down below.
Unless the bend allowance is known, leave it set as default. For more accurate flat patterns, confirm the bend allowance with the fabricator.
To change the parameters, right click on “Sheet Metal” from the Design Tree and select “Edit Feature”.
Select base flange/tab from the CommandManager and sketch a midpoint line 200mm long constrained to the origin. Exit the sketch and set the base flange properties as shown below.
In preparation for the sketched bend, create a sketch of a line 75mm away from the 50mm edge. Then select “Sketched Bend” from the CommandManager and click on the line from the sketch.
Use the sketched bend parameter shown below. Assume the part is limited to a maximum height of 75mm, select the “Material Inside” bend position.
Alternatively select the bend position appropriate for the design. The other bend types are:
- Bend Centerline
- Material Outside
- Bend Outside
This changes the location of the bend; as a result this affects the length of the flange.
For the purposes of showing the automatic bend relief, a partial “Edge Flange” will be added to the edge that is approximately 124mm long. In this case, the “Bend Outside” flange position is the only one that will not show a bend relief.
Use the “Edit Flange Profile” button to dimension the flange position. See the dimensions and settings below:
Leave the height of the flange as unconstrained; the length is controlled by the flange length.
There are three new options for the flange length, they are:
- Outer Virtual Sharp – The dimension of the flange is measured from the virtual sharp, this is the projected intersection of the outer edges of the bend.
- Inner Virtual Sharp – From the virtual sharp or intersection of the inner edges of the bend.
- Tangent Bend – Measured from a line that is tangent to the bend and perpendicular to the edge of the flange. This option is only available for bends greater than or equal to 90°.
The result is an 80mm flange with an automatic bend relief. The shape of the relief depends on the setting selected when creating the base flange.
The sketch used for the base flange/tab can be more complex, see the screenshot below for an example. The sharp corners of the sketch are automatically converted to bends, and the part can be flattened.