A flat pattern is a 3D sheet metal model in a flattened state.
Although you cannot create a sheet metal part, 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.
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.
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.
Export of flat patterns
You can export a flat pattern to an SAT file, or an AutoCAD DWG or DXF file. Full layer support (color, line type, and line weight) is provided for flat patterns saved in DWG or DXF formats.
Orientation of flat pattern
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 right-click 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.
Edits to flat pattern
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 .
Drawings of flat patterns
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 do so 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 pattern extents
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.