Create flat pattern in sheet metal

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 is displayed when this node is active. The flat pattern updates automatically when you edit the 3D model. Edits can be made to the flat pattern that simplify subsequent manufacturing operations. However, these edits are not visible when the model returns to the folded state.

The flat pattern is typically created normal to your initially sketched face feature; however there may be times when you must adjust the orientation. Select Edit Flat Pattern Definition from the context menu when the Flat Pattern node is selected to modify orientation, punch representation and bend angle measuring options.

The Drawing Manager uses the flat pattern for the flat pattern view. The flat pattern must be created in the part before you can place a flat pattern view in the drawing. If you delete the flat pattern, the drawing also loses the flat pattern view.

Note: If a model cannot be unfolded (for example, the created flange features overlap in the flat pattern), the flat pattern request generates a warning dialog box indicating 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 which intersect in the flattened state.

How is the flat pattern displayed?

After you create the flat pattern, you can switch between the folded part state and the flat pattern state.

To view an existing flat pattern:

Double-click the flat pattern node in the browser or
On the ribbon, click Sheet Metal tab Flat Pattern panel Go to Flat Pattern .

To view the folded model:

Double-click the folded model node in the browser or
On the ribbon, click Flat Pattern tab Folded Part panel Go to Folded Part .

If you revise the model, the flat pattern updates automatically. If a model revision results in an invalid flat pattern, a dialog box is displayed. Error conditions that exist in the flat pattern can be accepted so you can continue working. The error warnings persist until the error conditions are eliminated.

What happens if the flat pattern is oriented incorrectly?

Flat patterns may not always be generated in the best orientation for your manufacturing purposes. To reorient an existing flat pattern, select the flat pattern node context menu while the flat pattern is displayed and select Edit Flat Pattern Definition. A dialog box is displayed so you can select edges to make horizontal or vertical, and you can also flip the entire sheet over as required.

You may determine that various member files of a sheet metal iPart is best served by using unique orientations of their flat pattern. By saving uniquely named flat pattern orientations you are able to specify the orientation in the iPart table.

Note: Take care when creating drawings of flat patterns. Bend and punch notes which indicate a direction do so relative to the defaulted front side view that is placed during view creation. This view is based upon the front face seen in the flat pattern state of the model.

Can I edit the flat pattern?

While the flat pattern is displayed, Autodesk Inventor LT provides a Flat Pattern tab with panels of commands that can be used on the flat pattern. You can add features to your flat pattern that assist with manufacturing. Features added while the model is displayed as a flat pattern do not become part of the part model and are not displayed in the part feature history tree when the model returns to the Folded Model 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 impact physical iProperties, as does the last calculated model state (folded or flat with any edits in the flat).

How are flat patterns used in drawing views?

The Drawing Manager uses the flat pattern to create the flat pattern view. If you delete the flat pattern, that view is lost.

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).

Note: Take care when creating drawings of flat patterns. Bend and punch notes which indicate a direction do so relative to the defaulted front view that is placed during view creation. This view is based upon the front face seen in the flat pattern state of the model.

Can I export a flat pattern?

Flat patterns can be exported to a SAT file, or an AutoCAD DWG or DXF file. Any of these file types can be opened by some modelers, including Autodesk Inventor LT. With the flat pattern displayed, open the Flat Pattern node context menu and select Save Copy As. Full layer support (color, line type, and line weight) is provided for flat patterns saved in DWG or DXF formats.

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.