Sheet Metal Rules

Overview#

A sheet metal rule is a named bundle of manufacturing settings that Fusion applies to a sheet metal component: material thickness, default bend radius, bend allowance method (K-factor), relief shapes at bends, and how corners are treated where two or three bends meet. Every sheet metal feature (flange, bend, corner) reads from the rule, and the flat pattern calculation uses it to compute how much each bend stretches the material.

Getting the rule right is the single most important step toward a part that fits when it comes back from the shop. If your K-factor and bend radius do not match your fabricator's tooling, your flat pattern will be the wrong size even if the 3D model looks perfect.

Where to find it#

• Design > Sheet Metal > Modify > Sheet Metal Rules opens the rules dialog (the rule reference page is titled "Sheet metal rule reference" in Autodesk's Fusion help). Rules are listed in the Sheet Metal Rules Library.
• When you create the first flange in a component that has no rule, the Flange dialog shows a Sheet metal rule dropdown. Choose one, or Fusion applies the default. You can change it later in the Browser by editing the rule on the component.
• Rules are stored in the document and in a library you can reuse across designs. Hover over an existing rule to reveal the New Rule icon (this workflow is described by a third-party vendor guide; the icon placement may differ in your build).

Step by step#

Create a rule that matches a vendor:

1. Get the vendor's data: material, thickness, minimum bend radius or die/tool radius, and their K-factor or bend deduction table. Many online cutting and bending services publish these (for example SendCutSend lists per-material values).
2. Open Sheet Metal Rules. Select an existing rule such as the default steel or aluminium and create a new rule from it (do not edit the default in place unless you intend to).
3. Fill in the Name (for example Steel_1.5mm_vendorX), an optional Description (material grade, finish or shop standard) and the Material label.
4. Set Thickness to the real thickness (use the actual measured gauge thickness, not the nominal gauge number).
5. Set the Bend radius (inside radius, measured from the inner sheet surface to the bend centre).
6. Under Unfold Method the Type is Linear (the only method listed in Autodesk's reference), and you enter the K-factor.
7. Set the Bend Relief shape (Round, Straight or Tear) with Remnant, Width and Depth, and the 2-Bend and 3-Bend Corner Relief options.
8. Set Units to match the vendor (millimetres or inches) before typing values. Per Autodesk's API reference, a rule's units are permanently associated with it and cannot be changed later.
9. Close the dialog, then in the Flange dialog pick the new rule. The component carries this rule from now on.

Options reference#

Per-feature Override rules toggles in the Flange dialog (Bend override, Bend relief override, 2-bend corner override, 3-bend corner override) let you change these settings for one feature without altering the rule.

Tips and pitfalls#

Tip: The K-factor is the most abused number in sheet metal. The theory: the neutral axis is at distance K x thickness from the inside face. Bend allowance = angle (radians) x (inside radius + K x thickness). Fusion's Linear unfold method uses exactly this idea. If the shop gives you a bend deduction rather than a K-factor, back-solve K from a test part, or ask for the value they use.

Tip: Build a physical test strip or ask your vendor for a sample. One real bent part of known flat length gives you the K-factor for that material and tooling combination.

Warning: A very small bend radius can cause problems. Autodesk support has pointed to a user whose exported DXF lacked bend lines because the rule had a bend radius of 0.01 mm; raising it to a sensible value (here, about thickness/4) restored the bend lines. Use a radius the real tooling can make.

Warning: Do not mix units. A rule has its own units, fixed when it is created, so make a separate rule per unit system and pick the one the vendor uses.

Warning: Different bend operations (air bending vs bottoming/coining) give different effective radii. Ask the shop which tooling they will use and match it.

Reading K-factor properly#

K is the ratio of the neutral-axis offset from the inside bend surface to the thickness. Its value depends on material, bend radius, thickness, tooling and bending method. As a sanity check, K tends toward 0.5 for large radii relative to thickness (the neutral axis sits mid-thickness), and decreases toward about 0.3 for tight radii. Do not apply published numbers blindly; treat them as starting points.

Back-solving K from a test part#

You cut a test blank 80.0 mm long from 2 mm aluminium and bend it 90 degrees with a 2 mm inside radius. After bending you measure the two legs on the outside faces and get 42.0 mm and 42.0 mm. For a 90 degree bend the outside setback is radius + thickness = 4.0 mm per leg. The flat length equals the leg lengths minus the two setbacks plus the bend allowance:

80.0 = 42.0 + 42.0 - 8.0 + BA, so BA = 4.0 mm.

Since BA = angle x (radius + K x thickness), K = (BA / 1.5708 - radius) / thickness = (4.0 / 1.5708 - 2) / 2 = (2.546 - 2) / 2 = 0.27.

Sanity check the result: K must fall between roughly 0 and 0.5. A value outside that range means a measurement was taken on the wrong datum (inside instead of outside faces, for example). One test part is a starting point; bend three and average, because a 0.2 mm measuring error on a single bend moves K by about 0.05. If the shop quotes a bend deduction BD instead, convert with BA = 2 x setback - BD, so a deduction of 3.6 mm on this part gives BA = 4.4 mm and K = (4.4 / 1.5708 - 2) / 2 = 0.40.

Choosing rule values: a starting table#

These are generic starting values to compare with your shop's own chart, not standards.

Using rules in a design#

• A component carries one rule at a time. If a design needs two thicknesses, use two components.
• You can still deviate on a single feature with the Override rules checkbox in the Flange dialog (and the Bend override for contour flanges).
• Changing the rule updates the whole component, so make rule changes early, then rebuild and check the flat pattern.
• Thickness in a rule created by Convert to Sheet Metal is detected from the face you pick and cannot be edited later.

Common failures and fixes#

Practice exercise#

Create two vendor-style rules and quantify the difference.

1. Create a rule Al_2mm_K033 for 2 mm aluminium: radius 2 mm, Linear K-factor 0.33, Bend Relief Round with width 2 mm and depth 4 mm, 2-bend corner Round size 4 mm, Minimum gap 0.5 mm.
2. Create a second rule Al_2mm_K050 with K-factor 0.50 and radius 3 mm; everything else the same.
3. Build the same 50 x 30 x 30 mm U-channel (contour flange, 100 mm long) with each rule, in two components.
4. Create flat patterns and record the flat widths. Hand check: for the first rule each 90 degree bend allowance is 1.5708 x (2 + 0.33 x 2) = 4.18 mm; for the second 1.5708 x (3 + 0.5 x 2) = 6.28 mm.
5. Note the difference per bend and total for two bends, and explain why the 3 mm radius also changes the outside setback.
6. Change one of the rule's relief shapes to Tear and see what the flat pattern shows at a relief location.

Expected result: flat widths that differ by a few millimetres in total between the two rules, matching your hand calculations to within about 0.1 mm, and a clear picture of why a vendor-matched rule matters.

Related#

• Sheet metal workflow
• Flange
• Bend and corner treatments
• Flat pattern and DXF export
• Design for manufacture