Use a flat pattern, which is the shape of the sheet metal part before it is formed, to create drawings for manufacturing.
Flat patterns show bend lines, bend zones, punch locations, and the shape of the entire part with all bends flattened and bend factors considered.
Create Flat Pattern creates a flat pattern within the sheet metal part feature browser. A set of flat pattern edit commands are active while the model is displayed in the flat pattern state, including:
Although you cannot create a sheet metal part using Inventor LT, you can generate and document a sheet metal flat pattern. When you open a sheet metal part, the Sheet Metal tab on the ribbon provides access to the command to create a flat pattern.
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 of the flat pattern views in associated drawings.
Create Flat Pattern calculates the material and layout required to flatten a 3D sheet metal model.
The part browser displays a Flat Pattern node, and the flattened state of the model displays when this node is active. After you create a flat pattern, you can switch between the folded part state and the flat pattern state.
When you edit the 3D model, the flat pattern updates automatically. If a model revision results in an invalid flat pattern, a dialog box indicates any error conditions that exist in the flat pattern. You can accept and continue working, although the error warnings persist until the error conditions are eliminated.
You cannot flatten features that require material deformation, such as louvers or dimples. If you place these features onto sheet metal faces using the Punch Tool command, they are represented as 3D features on the flat pattern. They can also be represented using a selected sketch or with a centermark. Sketched and placed features can have unpredictable results, so use Punch Tool to add these shapes to your sheet metal part.
If you cannot unfold a model (for example, flange features that overlap in the flat pattern), a warning dialog box indicates intersecting features. You can Edit or Cancel the dialog box, or you can Accept the intersecting errors. If you accept, the flat pattern is developed with intersecting features. Subsequent feature creation in the folded model displays the dialog box until you edit the features that intersect in the flattened state.
Physical iProperties (including but not limited to: mass and volume) calculate differently depending upon the folded or flat state of the model. Any alternative punch representations present in your flat pattern impacts physical iProperties as does the last calculated model state (folded or flat with any edits in the flat).
You can export a flat pattern to an SAT file, or an AutoCAD DWG or DXF file. Full layer support (color, line type, and lineweight) is provided for flat patterns saved in DWG or DXF formats.
When you create a flat pattern, you can use the A-Side Definition command on the ribbon to mark any face in a sheet metal part as Up. The A-side face highlights to indicate the punch direction. If no A-side face is present when you create the flat pattern, the software creates the A side, and adds a browser entry
You can delete the A side it as long as no flat pattern exists. Changing the orientation of the flat pattern reflects on the A side that highlights when you select the browser node. If a change causes the compute of the A side to fail, you can right-click the A-side browser node and pick a new A side, which results in a new A-side browser node.
Use options on the context menu to highlight the A side, and adjust the orientation, punch representation, and bend angle measuring. If you click the command Show A-Side, you place all A-side faces into the preselection set of the document.
Sometimes various member files of a sheet metal iPart require unique orientations of their flat pattern. Save uniquely named flat pattern orientations to specify the orientation in the iPart table.
These display options are not available for punch features added to a flat pattern. 3D features that are placed in a folded model using iFeatures display as they are modeled. If these features remove material (for example, a cut), the flat pattern correctly represents the flattened sheet stock. If these features add material, the features display on the flat pattern as they are modeled
Using commands on the ribbon, Sheet Metal tab, you can add features to your flat pattern that assist with manufacturing. When you add features while the model is displayed as a flat pattern, they do not become part of the part model. When the model returns to the Folded Model state, these features do not display in the part feature history tree .
The Drawing Manager uses the flat pattern to create the flat pattern view. If you delete the flat pattern, that view is lost.
When creating drawings of flat patterns, remember that bend and punch notes that indicate a direction are relative to the flat pattern view shown in the model. Up is toward you relative to the shown (or named) view and Down is away from you relative to the shown (or named) view.
Physical iProperties (including but not limited to: mass and volume) calculate differently depending upon the folded or flat state of the model. Any alternative punch representations present in your flat pattern impacts physical iProperties as does the last calculated model state (folded or flat with any edits in the flat).
Flat patterns require a certain amount of material on the flat sheet stock. This material foot print varies in length and width depending on the orientation of the flat pattern. These properties update each time the flat pattern is updated or reoriented.
In Inventor, the length, width, and area are available in Drawing Manager (and using the API) as Sheet Metal Properties listed as: FLAT PATTERN EXTENTS LENGTH, FLAT PATTERN EXTENTS WIDTH, and FLAT PATTERN EXTENTS AREA.