Sheet metal design is an extension of the part modeling environment.
You can use unique template files to create sheet metal parts with predefined attributes, including material, bend relief, bend radius, corner relief, gap values, punch representations, and unfolding rules. Sheet metal-specific commands streamline work on both the folded and unfolded model. Flat patterns rich with manufacturing information can be created and documented on drawings containing tables of holes, punches, and bends. You can export flat patterns to industry standard formats for CNC manufacturing.
When you use sheet metal parts in assembly models, sheet metal fasteners are available through the Bolted Connection Component Generator, or through Content Center.
Methods to create sheet metal part
- Create a sheet metal part using the sheet metal template. The template uses your settings for material thickness, bend radius, and corner relief. You use sketch commands to create a profile for a base face or an initial contour flange. Then you exit the sketch and create your sheet metal feature, and add any additional sheet metal features required to complete your part.
- Create a regular part with a uniform thickness, and then convert it to a sheet metal part. Specifying a part as sheet metal displays the Sheet Metal tab, and adds sheet metal-specific parameters to the parameters list.
Conversely, you can convert sheet metal part to a standard part. Doing so closes the sheet metal tab, and restores the standard part modeling commands and environment. Conversion of a sheet metal part to a standard part automatically deletes the sheet metal flat pattern. Any time you delete a flat pattern in a sheet metal part, you also delete all flat pattern views in associated drawings.
Note: When using this technique, ensure that the modeled sheet thickness agrees with the material thickness parameter setting. After converting a part to sheet metal, we recommend that you replace any dimension and parameter values that control the sheet metal thickness with the Thickness parameter. For example, in an extruded feature use Thickness as the extrusion value with the Distance extent method. The Thickness parameter updates the part thickness when you change the Sheet Metal Rule, or when you override the Thickness manually in the Sheet Metal Defaults dialog box. - To create a sheet metal part to fit a specific set of conditions, construct a series of surfaces, stitch them together later, and then thicken them.
Sheet metal parts vs. regular parts
A sheet metal part starts out as a flat piece of metal with a consistent thickness. For manufacturing purposes, details like bend radii and relief sizes are usually the same throughout the part. You enter the values for these details, and then the software applies them as you design. For example, when you create a flange the bend is added automatically.
It is necessary to convert the folded model back to a flat pattern for manufacturing purposes. Then you can switch between the folded view of the model and the flattened view by double-clicking the Folded Model or Flat Pattern browser node.
You can add features to the flat pattern for clean-up purposes. These operations are typically performed to support shop-specific manufacturing practices. Features added to the flat pattern using the commands on the Flat Pattern tab do not display when you view the model in the folded state.