Sheet metal parts are different from regular parts
Sheet metal design lends itself to optimization. Sheet metal has a consistent thickness. For manufacturing purposes, details like bend radii and relief sizes are usually the same throughout the part. In a sheet metal part, you enter the values for these details and then the software applies them as you are designing. For example, when you create a flange you do not need to add the bend manually.
Another way that sheet metal design differs from part modeling is the flat pattern. Because a sheet part starts out as a flat piece of metal, it is necessary to convert the folded model into a flat pattern for manufacturing purposes. After the flat pattern is created, 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.
Features can be added 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 available on the Flat Pattern tab do not display when the model is viewed in the folded state.
Decide how to create sheet metal parts
You can create sheet metal parts in several ways:
- Start a new part. Select the sheet metal template. The template uses your settings for material thickness, bend radius, and corner relief. Use sketch commands to create a profile for a base face or an initial contour flange. Exit sketch and create your sheet metal feature. Add additional sheet metal features as required to complete your part. It is the most common method of creating sheet metal parts.
- Optionally, you can create a regular part, and then convert it. The part is converted to a sheet metal part and the sheet metal command palette is displayed. Conversely, a sheet metal part may also be converted to a standard part. Doing so closes the sheet metal command palette and restores the standard part modeling commands and environment.
Note - when using this technique it is important to 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 from the Sheet Metal Defaults dialog box.
- Alternatively, constructing a series of surfaces which are stitched together later and then thickened is the most straight forward way to obtain a sheet metal part to fit a specific set of conditions.
Specifying a part as sheet metal makes the Sheet Metal tab available and adds sheet metal-specific parameters to the parameters list.
Create stamped features in a sheet metal part
Sheet metal features that are created using specialized punch tools can be modeled and saved using iFeatures and later placed using the Punch Tool command. For example, you can use the Revolve command to create a dimple and save it as a Sheet Metal Punch iFeature.
Features created with feature modeling commands are not flattened, but the outline appears on the flat pattern. When you detail the flat pattern in a drawing, you can dimension to the outline of the feature. Optionally, these features can be represented on the flat pattern (and drawings) with a punch center point or by using an alternative (possibly simplified) sketch.
Use the Punch Tool command to place multiple occurrences of a punch in one step. Create iFeatures to represent the punch shapes. When placed on a sheet metal part, the iFeatures are shown as 3D in the flat pattern.
An iFeature used as a punch must have a single unconsumed center (sketch) point in the placement sketch. The Punch command uses the center point to position the punch. The placement sketch must be on the top or bottom sheet metal face.
Use industry standard materials
Use the Sheet Metal Defaults command to select materials, sheet thickness, corner, and bend reliefs and unfolding rules that differ for the rules in the active style.
Sheet Metal Styles are fully supported by the Style and Standard Editor and can be stored locally within a part or template or shared by using a shared Style Library.
Use the Parameters command to change parameter names and values
Changes in the Parameter dialog box affect only the active sheet metal part.
- On the ribbon, click .
- In the Parameters dialog box, click a cell under Parameter Name, Unit, Equation, or Value and then modify the current model parameters.
- Click a cell under Comment to add instructions or other custom text.
- Click Add to create your own parameters.
- Click Link to locate and specify an external spreadsheet that defines parameters.
Plan how to show features in flat patterns
Creating a flat pattern of a rolled part
By selecting a rolled face before creating a flat pattern, you can flatten a part which may not have any flat faces.
Features with elliptical or spline profile geometry
Contour Flange, Contour Roll, and Lofted Flange features may contain elliptical or spline segments within the defining profiles. These geometries rely on a Spline Factor Value (as will the length of any non-cylindrical or conical bends) when the feature is flattened. The Spline Factor Value is defined within the Sheet Metal Unfold rule. This value defaults to 0.5. Adjust the value up or down to more closely represent your manufacturing requirements.