Flat Pattern and DXF Export

Overview#

The flat pattern is the unfolded outline of your sheet metal part, with bend lines. It is what the fabricator cuts. Fusion creates it from the formed model using the rule's thickness, bend radius and K-factor. You then export it as DXF (2D) for cutting services. A flat pattern is a separate environment tied to the part: it updates when the 3D model changes.

Where to find it#

• Design > Sheet Metal > Create > Create Flat Pattern. Fusion adds a Flat Pattern node to the Browser and shows the flat pattern.
• Export: right-click the flat pattern in the Browser, choose Activate, then click Export DXF on the toolbar (dialog title: Export Flat Pattern As DXF). Use this rather than a generic File > Export; the free personal-use licence can export a DXF from a flat pattern or sketch but not from the File menu, according to a vendor FAQ.
• Finish Flat Pattern (or Exit Flat) returns you to the folded model. In the Browser, the Activate Flat Pattern radio button switches between folded and flat views.

Step by step#

1. Check the sheet metal rule one more time (thickness, radius, K-factor) against your vendor.
2. Choose Create Flat Pattern.
3. Select the Stationary face, the face from which all flanges unfold. Pick the largest flat face on the part. The model needs at least one flat face, and the component must be a single body.
4. Click OK. Inspect the flat pattern. Use Measure to check the overall length and width against the sheet size.
5. If the Browser shows an Out-Of-Date icon on the flat pattern after an edit, activate it or right-click it and choose Update Flat Pattern.
6. With the flat pattern activated, click Export DXF on the toolbar.
7. In the dialog, pick the unit type (the design's active unit is the default), optionally tick Visible geometry > Center lines and Extent lines to include bend lines, and tick Convert splines to polylines (recommended, because polylines are more widely accepted; the tolerance sets the maximum deviation from the original spline). Click OK, choose a location and file name, and Save.
8. Open the DXF in a viewer or the vendor's upload page and check scale, units and bend lines.

Options reference#

Tips and pitfalls#

Tip: Vendors such as SendCutSend recommend using the dedicated flat pattern DXF export instead of generic File > Export; the generic route can change units, split curves into many segments, or drop details the vendor needs.

Warning: If bend lines are missing from the DXF, check the rule. One Autodesk support case traced missing bend lines to a bend radius of 0.01 mm in the rule; raising it to a realistic value fixed the output.

Warning: The flat length Fusion reports can differ from the shop's own bend allowance. A user measured about 0.014 inch difference on a single bend; across several bends this adds up. Verify with a test part or match the shop's K-factor.

Tip: Create the flat pattern as soon as the part starts to be bendable and check it regularly. Failure to flatten is easier to diagnose early.

Tip: The DXF is a 2D file; the shop will need bend direction, angle and material notes in the order, or a drawing. Many vendors read bend data from a STEP file instead; export both if needed. If you use a vendor's bending service, keep Fusion's default solid bend-line indicators.

Warning: Licence terms: DXF export of the flat pattern is available in the personal-use licence at the time of writing, but check your current licence; non-commercial use only applies there.

Reading the flat pattern for errors#

Open the flat pattern and check these before exporting.

1. Overall size. Compare the bounding box with the sheet or bed size. A 1,250 x 2,500 mm sheet and a 12 mm nesting margin leave roughly 1,226 x 2,476 mm usable; confirm with your vendor.
2. Bend lines. Count them. A part with five bends should show five bend centre lines. A missing line means the bend radius in the rule is too small to register (see below).
3. Reliefs and gaps. Corners show the relief shape you chose; check that none overlap holes.
4. Holes near bends. Holes within about 2.5 x thickness + radius of a bend will distort when formed. For 2 mm material and a 2 mm radius, that is about 7 mm.
5. Small features. Slots and tabs narrower than the thickness may not cut or bend. A 1 mm slot in 2 mm stainless is unreliable on laser.

Worked example: checking a flat length by hand#

A bracket in 2 mm aluminium has two legs, 40 mm and 30 mm (outside lengths), one 90 degree bend with a 2 mm inside radius and K-factor 0.4. Outside setback = radius + thickness = 4 mm for 90 degrees. Bend allowance = 1.5708 x (2 + 0.4 x 2) = 4.398 mm. Flat length = (40 - 4) + (30 - 4) + 4.398 = 66.40 mm. If Fusion shows 66.4 mm, the rule is behaving. If the vendor uses a K-factor of 0.33 instead, the allowance is 1.5708 x (2 + 0.66) = 4.178 mm, and the flat length is 66.18 mm. That 0.22 mm difference per bend is why you match the vendor's rule. A part with six bends could differ by over 1.3 mm.

DXF export: settings and preflight#

• Always use Export Flat Pattern as DXF from the active flat pattern.
• Tick Convert Splines to Polylines unless the vendor wants splines. Check the polyline tolerance; the default is usually acceptable.
• Reopen the DXF in a viewer. Verify units by measuring a known dimension, and verify that the layers are as the vendor expects.
• If a vendor's preflight demands all objects on one layer, merge layers in a graphics program, not in Fusion, because Fusion's export uses several layers.
• If the vendor does the bending, send the STEP file or drawing too, with bend angles and directions.

What to do when the export fails#

An Autodesk community report notes that some flat patterns fail to export with an unspecific error. Troubleshoot in this order:

1. Update the flat pattern (out-of-date patterns cause failures).
2. Check for zero-length edges or tiny slivers from corner reliefs; enlarge the corner relief or Minimum gap.
3. Simplify spline outlines, or enable Convert Splines to Polylines.
4. Delete the flat pattern and recreate it with a different stationary face.
5. As a last resort, project the flat pattern edges into a sketch and export that sketch as DXF.

Common failures and fixes#

Keeping the flat pattern in sync with the design#

The flat pattern is a feature tied to the model, so any change upstream can make it out of date. Three habits keep it reliable. Create it late enough that the part is bendable and early enough to catch problems, then check the Browser for the Out-Of-Date icon after edits. Do not place new sheet metal features after the flat pattern in the timeline without updating it, because the pattern shows the model state it was built from. And if the geometry has changed significantly, such as a new stationary face, delete the flat pattern and recreate it instead of updating, which avoids stale references.

For drawings, the flat pattern can be placed on a drawing sheet with bend notes, so the shop receives a DXF for cutting and a drawing for bending. Keep the rule name in the file name (for example bracket_1.5mm_steel_rev02.dxf) so a later reader can tell which K-factor and radius the pattern assumed. When a vendor returns parts that are slightly off, change the rule's K-factor to match their measured bend allowance, regenerate the pattern and compare; most of the time a correction of 0.02 to 0.05 in K brings the next batch into tolerance.

Practice exercise#

Create, verify and export a flat pattern with a hand check.

1. Make a 2 mm aluminium rule with a 2 mm inside radius and K-factor 0.4. Build an L-bracket with legs of 40 mm and 30 mm (outside lengths) and a 10 mm wide base, using edge flanges.
2. Add two 5 mm holes 15 mm from the bend on the 40 mm leg.
3. Create Flat Pattern, picking the largest flat face as the stationary face. Measure the length. Compare with the hand calculation of 66.40 mm.
4. Change the K-factor to 0.33 and update the flat pattern. Record the new length and compare with 66.18 mm.
5. Export the DXF with Convert Splines to Polylines ticked, and open it in a free viewer. Measure the overall length and confirm that there is one bend line and two holes.
6. Move one hole to 4 mm from the bend and see whether it falls within the distortion zone (about 7 mm). Move it back.

Expected result: a flat length close to 66.4 mm that changes by a couple of tenths of a millimetre when K changes, and a DXF with an outline, two circles and one bend line. Note any difference between the viewer's measurement and Fusion's.

Related#

• Unfold and refold
• Sheet metal rules
• Design for manufacture