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.

Features that require material deformation, such as louvers or dimples, cannot be flattened. If these features are placed onto sheet metal faces using the Punch Tool command, they are accurately represented as 3D features on the flat pattern. Optionally, they can be represented using a selected sketch or with a center mark. Sketched and placed features can have unpredictable results, so use Punch Tool to add these shapes to your sheet metal part.

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 you create a model that 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 .

Note: In an assembly, double-click the sheet metal part in the browser to activate and double-click the flat pattern node. In this workflow, the sheet metal part opens in a new window with the flat pattern active. Save and Close to return to the assembly.

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.

How are 3D features displayed in flat patterns?

3D features added to the folded model using the Punch tool offer the most flexibility in flat patterns. These features may be displayed as:

• A 3D feature
• An alternative sketch representation
• A sketch with center mark
• A center mark only

Note: Punch features added to the flat pattern do not offer the above display options.

3D features that are placed in the folded model using iFeatures display as they were 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 are displayed on the flat pattern as they were modeled.

Note: Parts that are converted to sheet metal may have 3D features that cannot be formed using the uniform thickness of the sheet stock. These features display in the flat pattern as they were modeled.

Why are cut features shown as lines or arcs?

In some cases, cut features in a sheet metal part show only as lines or arcs in the flat pattern. Usually, this is because the feature was cut at an angle to the face on which it was applied, or because you added chamfers or rounds to the edges of the cut feature.

Can I edit the flat pattern?

While the flat pattern is displayed, Autodesk Inventor 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.

Note: Model features that may be easier to create while the model is in a flattened state should be added after an Unfold feature has been added to the model. If these features cross over a bend zone, they will deform as expected when the model is returned to the folded state using a Refold feature.

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).

Note: While nothing prevents you from adding punch features while the model is displayed flat, these features do not display when the model is folded nor can you take advantage of alternative representations in the flat or in drawings of the flat. Consider adding these features after an Unfold feature.

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. 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. The length, width and area will be available within Drawing Manager (and via the API) as Sheet Metal Properties listed as: FLAT PATTERN EXTENTS LENGTH, FLAT PATTERN EXTENTS WIDTH and FLAT PATTERN EXTENTS AREA. These properties update each time the flat pattern is updated or reoriented.

Note: Legacy sheet metal parts migrated to the R2010 release have these properties but they require a manual update.