Sheet Metal Flat Patterns for Multi-Bend Parts

An L-bracket has one bend, and a small error barely matters. A hat section has four, a box has four plus corners, and a small error in each one adds up to a part that does not fit. You can already work out bend allowance, setback and bend deduction for a simple part. The next step is to handle real prints: mixed dimensions, several bends, holes in the flat, and tolerances that have to survive every bend.

What You Will Be Able to Do

• Convert a print with mixed inside and outside dimensions to one basis.
• Work out your real bend deduction and K-factor from a test bend.
• Lay out a multi-bend part and locate every bend line.
• Lay out a box, including corner notches.
• Add a closed hem to a blank, and move holes from the print to the flat.
• Estimate tolerance stack-up before you cut.

A Quick Reminder

The flat length is the sum of the outside dimensions, minus one bend deduction (BD) for each bend. For a 90 degree bend, setback (SB) is the inside radius (R) plus the thickness (T), and BD = 2 x SB - BA, where BA is the bend allowance.

Everything here builds on those three lines, so make sure they feel easy before you go on.

Put the Print on One Basis

Designers dimension what matters to them, so a print often mixes inside and outside dimensions. The formulas need outside dimensions. Convert everything before you do any math.

Worked Example: A Channel With Inside Dimensions

A channel in 16-gauge steel (0.060 inch) has an inside web of 3.000 inches and two legs of 1.000 inch, measured from the inside face. Your bend deduction is 0.116 inch.

• Outside web: 3.000 + 2 x 0.060 = 3.120 inches
• Outside leg: 1.000 + 0.060 = 1.060 inches, twice
• Sum: 3.120 + 1.060 + 1.060 = 5.240 inches
• Two bend deductions: 2 x 0.116 = 0.232 inch
• Flat length: 5.240 - 0.232 = 5.008 inches

Skip the conversion and you get 5.000 - 0.232 = 4.768 inches, which is 0.240 inch short. That is a scrapped part, and you may cut the whole batch before anyone notices.

Finding Your Real K-Factor

K-factor gives the location of the neutral axis. About 0.33 is the usual starting value for air bending mild steel. But K is not a fixed property of the metal. Published shop tables show it rising as the bend radius grows compared to the thickness, from about 0.33 for tight bends to around 0.40 or more for larger ones. Material hardness and tooling change it too. So when the job is tight, you measure.

Worked Example: Backing K Out of a Test Bend

You are bending 14-gauge steel (0.075 inch) on a 0.625 inch V-die. In air bending, the inside radius is about the die opening divided by 6, so R is about 0.104 inch.

1. Shear a strip of the real material to exactly 6.000 inches.
2. Bend it to 90 degrees on the real tooling.
3. Measure both outside legs: 3.076 and 3.074 inches.
4. Add them: 6.150 inches.
5. Your bend deduction is 6.150 - 6.000 = 0.150 inch.

If all your bends are 90 degrees, you can stop here and use 0.150. To get a K-factor for software or for other bend angles, keep going:

1. Setback: 0.104 + 0.075 = 0.179 inch
2. Bend allowance: 2 x 0.179 - 0.150 = 0.208 inch
3. K = (BA / 1.5708 - R) / T
4. K = (0.1324 - 0.104) / 0.075 = 0.38

The 1.5708 is pi divided by 2, which is the angle part of the bend allowance formula for 90 degrees. For this setup, K comes out to 0.38, not 0.33.

Does that small difference matter? A K of 0.33 would give a bend deduction of 0.156 inch, which is 0.006 inch too much. Over four bends, your blank comes out 0.024 inch short. On a part with a tolerance of plus or minus 0.015 inch, that is a reject.

Measure the real radius with a radius gauge if you can, because a wrong R gives a wrong K. Save the result in your shop bend chart along with the material, thickness and die. A measured number for your own tooling beats any table.

Worked Example: A Hat Section With Four Bends

A hat section has outside dimensions of 1.000, 1.500, 2.000, 1.500 and 1.000 inches, in the same 14-gauge steel. Use the measured BD of 0.150 inch.

Flat length:

• Sum of outside dimensions: 7.000 inches
• Four bend deductions: 4 x 0.150 = 0.600 inch
• Flat length: 6.400 inches

Bend lines. You also need to know where to bend. A bend line runs down the middle of the bend zone. That gives two simple rules:

• From a free edge to the first bend line: the outside leg minus half a BD.
• Between two bend lines: the outside dimension minus one full BD.

Check it. The last leg is 1.000 - 0.075 = 0.925 inch, and 5.475 + 0.925 = 6.400 inches. That matches the flat length, so the layout closes.

Always run that check. If the bend lines and the last leg do not add up to your flat length, you have made a mistake somewhere, and it is much cheaper to find it now.

Moving Holes From the Print to the Flat

A hole on a formed part is dimensioned along the formed surface, so its position in the flat is different. Work from the nearest bend line.

Say the top of the hat has a hole 1.000 inch from the outside corner at bend 2. From a mold line to the bend line is half a BD, so:

• Flat distance from bend line 2: 1.000 - 0.075 = 0.925 inch
• Flat position: 2.275 + 0.925 = 3.200 inches from the left edge

Since 3.200 is half of 6.400, that hole sits at the center of the blank, which is right for a hole centered on the top.

Keep holes out of the bend zone, because metal there stretches and a round hole turns oval. A common shop rule is to keep the edge of a hole at least 2 x T plus the bend radius from the bend. If a hole has to sit closer than that, make it after forming, or ask about a relief slot.

Worked Example: Laying Out a Box

You need an open box with outside dimensions of 10 by 6 inches and flanges 2 inches tall, in 18-gauge steel (0.048 inch). Use an inside radius of 0.0625 inch and K of 0.33.

Step 1: Bend deduction.

• BA = 1.5708 x (0.0625 + 0.33 x 0.048) = 0.123 inch
• SB = 0.0625 + 0.048 = 0.1105 inch
• BD = 2 x 0.1105 - 0.123 = 0.098 inch

Step 2: Blank size. Each direction has two bends.

• Length: 2 + 10 + 2 - 2 x 0.098 = 13.804 inches
• Width: 2 + 6 + 2 - 2 x 0.098 = 9.804 inches

Step 3: Bend lines.

• From each edge to the bend line: 2 - 0.049 = 1.951 inches
• Base between bend lines: 13.804 - 2 x 1.951 = 9.902 inches long, and 9.804 - 2 x 1.951 = 5.902 inches wide

Step 4: Corner notches. Cut a square notch at each corner, 1.951 inches on a side, so that the flanges can fold up without crashing into each other. Add a small relief where the two bend lines cross, so the corner does not tear.

Your corner joint changes the notch. A welded corner may want a small gap. A riveted or lapped corner needs a tab added to one flange. Decide on the corner before you cut, and test one if the job is new.

Step 5: Bend order. Bend the long sides first, then the short sides. Once two sides are up, a standard brake cannot reach the others, so use a box and pan brake with its removable fingers set to clear the flanges.

Adding a Closed Hem

A hem is a 180 degree fold, and the ordinary bend formulas do not apply to it. A published press brake rule says that the metal in a closed hem elongates by about 43 percent of its thickness, for material under about 0.080 inch thick. So you add the outside dimensions up to the fold, then subtract 0.43 x T.

Example: A panel in 20-gauge steel (0.036 inch) has a 2.000 inch flat section ending in a 0.500 inch closed hem.

• Sum: 2.000 + 0.500 = 2.500 inches
• Hem deduction: 0.43 x 0.036 = 0.0155 inch
• Flat length: 2.500 - 0.0155 = about 2.485 inches

That figure assumes ideal conditions, so make a sample hem and measure it. Shop charts or a test beat the rule.

Tolerance Stack-Up

Each bend adds its own small error. Stack-up is what you get when those errors add up across a part. Worst-case stack-up assumes they all go the same way.

Say each bend in the hat section holds plus or minus 0.010 inch. Four bends give a worst case of plus or minus 0.040 inch across the part. If the print holds the overall width to plus or minus 0.030 inch, the process cannot be relied on to hit it. Fix that before you run the job:

• Find out which dimension matters. Often it is one feature to another. Talk to the person who wrote the print.
• Gauge from a flat, cut edge. Gauging from a formed flange carries the last error into the next bend.
• Choose a bend order that protects the critical dimension. Bend the critical feature with the fewest steps between it and the gauge edge.
• Make a first article. Measure it fully before you run the batch.

Check Before You Cut

1. Is every dimension on one basis?
2. Did you use the real thickness, measured with a micrometer or calipers?
3. Do you know which die the brake will use?
4. Does the bend deduction come from your shop chart or a test?
5. Do your bend lines and final leg add up to the flat length?
6. Is there one bend deduction for every bend?
7. Are holes clear of the bend zones?
8. Is the grain direction right for the tightest bends?
9. Have you made one first article?

Common Mistakes

• Mixing inside and outside dimensions. The blank can be off by several thicknesses.
• Using 0.33 for every job. K changes with the radius and material.
• Forgetting to split the BD at a free edge. The first bend line lands in the wrong place.
• Skipping the layout check. A math error reaches the shear.
• Measuring holes on the print and marking them in the flat. They need the same conversion as bend lines.
• Cutting a corner notch before deciding on the corner joint. You may need a tab you already cut off.

Check Your Understanding

A channel in 0.060 inch sheet has an inside web of 4.000 inches and inside legs of 1.500 inches. Your bend deduction is 0.116 inch. What is the flat length?

The outside web is 4.120 inches and each outside leg is 1.560 inches, for a sum of 7.240 inches. Subtract 0.232 inch for the two bends, which gives 7.008 inches.

A test strip cut to 8.000 inches measures 4.110 and 4.112 inches after one 90 degree bend. What is your bend deduction?

The legs total 8.222 inches, so the bend deduction is 0.222 inch.

A part has five bends, each holding plus or minus 0.008 inch. What is the worst case across the part, and why does that matter?

Plus or minus 0.040 inch. If the print's overall tolerance is tighter than that, you need a different gauging plan or bend order.

A panel in 0.030 inch sheet has a 3.000 inch section and a 0.375 inch closed hem. About how long is the flat?

The sum is 3.375 inches. Subtract 0.43 x 0.030, or about 0.013 inch, to get about 3.362 inches. Check it with a sample hem.

Key Takeaways

• Convert every dimension to one basis before you start the math.
• K-factor is not a constant, so measure it for tight work.
• A free edge gets half a bend deduction, and the space between two bends gets a full one.
• Check that your bend lines and last leg add up to the flat length.
• Holes need the same conversion as bend lines, and they need to stay out of the bend zone.
• Errors stack up, so gauge from a cut edge and prove a first article.