Bend Allowance first created 25/06/06 - last modified 25/06/06 Page Author: Ty Harness
Work in Progress............
Write more on specific software parameters.
A common question often asked about the sheet metal software is how much material should be allowed for the bend.

The answer really depends on how you are going to use the pattern, the material, and also the chosen machine tool (M/T) to form the bends.

How are you using the pattern?

Some people just use the software for rolled,extruded or cast sections. For example, using a paper template to wrap around the outside of a circular hollow section (CHS) pipe. In which case the outside diameter dimensions are entered into the software because the paper has a negligible thickness. Figure 1 shows paper templates being used to 'mark-out' pipes by centre dotting through the paper templates. It's then possible to flame cut and grind back to the centre dotting.

text here
Figure 1 - Using paper templates wrapped around the outside of the pipe.


We are mainly talking about sheet materials of constant thickness like steel, copper, aluminum,brass and plastic sheet. The ductility and malleability dictate how tight a bend can be produced without the material being fractured or becoming excessively weakened. You can cut and bend some poly carbonate sheets like Lexan(TM) but acrylics like Perspex(TM) can only be folded by heating the fold line.

Rolled materials such as steel elongates the grain in the rolling direction. It's always advisable to fold at 90 degrees to the grain direction. Some materials (even Steel) when folded along the grain direction will split along the outside of the bend. Of course it's not possible or economical to always fold 90 degrees to the grain direction. If the folded product is a structural element then it's important that the manufacturing and structural engineers check the material suitability either from the manufacturer's data or by testing the material because a particular folding sequence may be detrimental to the ultimate strength.

Something for the designer to consider are sheet coatings like tin and zinc which may also dictate how tight a bend can be produced without damaging the coating. Finishes applied after folding like nickel, chrome and even plastic powder coating do not like sharp corners as there's a tendency to fill up the internal corner with an excess of the coating material and produce a thin, weak point on the external edge allowing the coating to split away.

Working with sheet materials

For the Ty Harness Sheet Metal software the dimensions should be entered with neutral plane dimensions. Unfortunately there is no function in the software to compensate for any material extensibility. Hence, the pattern generated is an inextensible developable surface. Paper is a good example of an inextensible material; however, for materials with thickness the neutral plane is a plane that neither stretches or shrinks. In general, for thin sheet the neutral plane can be considered the centre line of the sheet particularly if the radius of bend is large compared to the thickness.

If you know little about the machine tool or how the material behaves when bending (particularly thick material 3mm up) you will need to make some experiments with (say)some material off-cuts. Figure 2 shows a simple 90 degree bend with an equal leg length - a typical every day job for every sheet metal shop. The Draughtsman usually specifies outside or inside dimensions rather than neutral dimensions and rarely makes any compensation for bend allowance. The bend allowance and cutting list is often left to the sheet metal worker and the reason for this is every M/T is different and an experienced operator will be best placed to know all the machine's idiosyncrasies.

A sheet metal worker shall gauge the importance of the work and dimensions to deduce the accuracy needed for assembly work. For routine or average quality work the bend allowance can be found by deducting the thickness of material from the outside dimensions i.e. just summing the internal dimensions. Equation 1 shows the flat sheet should be cut to 94mm and the bend line marked at 47mm (the centre).

text here
Figure 2 - 50x50x3 folded angle

$(50-3) + (50-3) = 47 + 47 = 94 [mm] $ .......... Equation 1.

Some work requires a greater accuracy but more information needs to be known about the bend radius. You must therefore understand your M/T and its tooling. To be truly accurate you will need to do some simple tests to determine the bend radius for different tooling and also for different materials. A tight bend may be detrimental to some materials and some grades of steel. Even bending with or against the grain may produce different results.

Box and Pan (or leaf)folders can produce a very tight bend where the inside radius tends to be the same as the tooling blade radius. The hand operated Edwards folder shown in figure 3 is used only for light gauge material up to 2 mm thick and the blade tip radius is approximately 2 mm. We use the same tooling for all jobs and hence even 0.8mm to 2mm thick sheet all have a 2mm inside radius. If the swing beam distance is too close you can't fold to 90 deg without squishing the material and over straining the folder or if the swing beam is too slack then the fold looks dreadful. A very good tip given to me is can fold a sacrificial piece of aluminum around the blade so that you can increase the inner radius of the folded piece. This can be critical for coated materials. It also means you don't have rush out and buy more tooling.

text here text here text here
Figure 3a - Edwards box and pan folder. b) Typical folder geometry. c)Tip for adjusting inner radius

Press brakes are often used in the air bending configuration, as shown in figure 4b, where the blade tip radius is not that influential on the formed bend's inner radius. Conventionally, the Vee block opening is 8 to 10 times the thickness of the material to produce good quality folds. It's a compromise because you have to use the same 'vee' over a range of different materials and thicknesses. Figure 4a shows a multi purpose V block although you can buy or have made a huge array of specialist tooling. Please see [xx] for more details. If the blade tip radius is too sharp it will cut or deform the surface which will produce a sharp bend but complicate the bend allowance calculation considerably. Most machines have a chart on the side telling you the best operating parameters and tooling configurations.

text here text here
Figure 4 - A typical 'vee' block bottom tool. b) Kingsland 300 Tonne Press Brake.

So for the 50x50x3 folded angle example I would use the 30mm 'vee' opening on the above Kingsland press brake and from experience this would tend to produce an inner radius of twice the thickness of material. Incidently, draughtsmen used to specify the inner radius to twice the thickness of material because it was a standard defined by the Air Ministry [xx].

Therefore knowing this extra information we can take another look at a more accurate calculation.

text here
Figure 5 - 50x50x3 folded angle

Figure 5 shows the same bend as figure 2. Note I assume a neutral axis (central to the sheet) has a radius of 7.5mm in equation 2 and PI/2 is 90 degrees in radians.

$(50-1.5-7.5) + (50-1.5-7.5) + 7.5*(pi/2)= 93.781 [mm] $ to 3 decimal places ...........Equation 2

So that you can see equation 1 produces a result, in general, accurate enough for most work.

Some sheet metal shops introduce a k factor (or a bend deduction factor) into the equation to compensate for machine tooling and material factors which do not necessarily produce an inner bend radius of twice the material thickness and where the neutral line can not be assumed to be centre of the sheet. From figure 2 where we assumed the neutral axis was central then the bend radius, rb is :

$ r_b = r_i + t*0.5 = 6+3/2 = 7.5 $ ............. Equation 3

where ri is the inside radius, t the material thickness and the 0.5 factor is often called the k factor.

The k factor can only really be found by experimentation for each sheet metal shop and for each M/T. The sheet metal shop could cut down some accurate strips of (say) 100mm long in 3mm thick mild steel. The press brake backstop is set to 50mm and a 90 deg bend is folded. Using (say) internal radius gauges then the inner radius can be determined by measurement and the external legs could be measured with a vernier caliper. Let's say we found an inner radius of 5.5mm and leg lengths of 53.4mm.

53.4 + 53.4 = 106.8 If we were trying to produce figure 2 the 50x50x3 folded angle then we can see the created angle is 6.8 too long. The difference between what you get and what you want is the bend allowance B - Hence we could now guillotine another strip at 100-6.8 = 93.2mm. To find the k factor use equation xx:

$ 6.8 = 5.5 + 3*k $ and therefore

$k = (6.8-5.5)/3 = k = 0.4333 $

For bends on that machine using the same material, tooling and bend angle then you can use the calculated value of k to achieve a more accurate bend.

If k is less than 0.5 you might ask yourself why have we lost some material and if k is greater than 0.5 then we've gained some material. The local thickness of the sheet has been deformed either stretched or compressed. The ideal of a inextensible ruled surface is no longer true. Too much thinning or thickening may be detrimental to the strength and, or appearance of the product.

What happens when the bend is greater than 90 degrees? Can we use the previous calculated k factor? The answer is unfortunately no because the bend is more likely to neck down even further because the strain is greater edging nearer to failure. Finally, we could say for every phi radians bend the bending allowance equation is:

$B = r_b*phi = (r_i+t*k)*phi[rad]$ ................ Equation 4

If you don't understand radians then the conversion from radian to degrees

$B = (r_i+t*k)*gamma[deg]*(pi/180) $ ................ Equation 5

More information on radians and there conversion to degrees can be found here:

Quick N.,J. [1] recommends that if the inside radius is less than 3t then k = 0.4 and if the radius is greater than 3t then k = 0.5. Wikipeidia[5] states between 0.3 - 0.5

In conclusion then knowing the exact bend allowance is not a straight forward calculation and some experimentation may be required. If your making (say) one off piece of duct work then you can get away with not worrying too much about bend allowance where you can soon stretch or shrink the flange a millimetre either way[4]; however, if you are mass producing a product then it's essential a prototype is built to resolve the bending allowance and all the issues before production.

(1) Quick, N.,J., Kempe's Engineers Year-Book, Morgan-Grampion Book Publishing Co. Ltd., 96th, London: (1996), Vol. 1 pD3/63.
(2) Townsend, W.,S.,, The Development of Sheet Metal Detail Fittings, Pitman, 2nd, London: (1938), pp xx-xx.
(3) Benson, S.,D.,, Press Brake Technology A guide to precision sheet metal bending, Pitman, 2nd, London: (1938), pp 53-66.
(4) Budzik, Sheet Metal Technology, ??, ??, ??: (19??), pp?? .


More Information on the web

ASCII to MathML used in this page: ASCIItoMathML homepage