Ok, so I've had this problem for a long time, and have been using work a around to get the correct values. However, I figure the time is now to post the question and see if I can get an answer. Why do bend deductions in Solidworks not give you the proper flat length? Bend deductions in theory relate to the amount of stretch on every corner. A bend deduction is the amount of material you must subtract from the flat pattern in able to obtain your desired part. Thus, if you put a bend deduction of 3/16" for every bend, then Solidworks should subtract that amount from every bend when constructing your flat pattern. However this is not the case. My flat patterns are always wrong compared to what it SHOULD be and I can't figure it out. Now it would be acceptable to be off by a 1/16" or so but sometimes it is off by an inch which is totally unacceptable. It appears that if the bend deduction is double the thickness of the material then I can obtain the correct flat pattern length. However if I am bending 12 ga steel with a bend deduction of 3/16" I obtain totally wrong flat length dimensions. This has me wondering how Solidworks actually uses Bend Deduction to calculate flat patterns. It should be as simple as adding up all your bent dimensions and then subtracting the number of bends multiplied by the bend deduction to get a flat pattern. I don't think I am doing anything wrong, but maybe I am. My Solidworks VAR told me to try using decimals instead of fractions, which is a rubbish solution to a real problem. Does anyone else have similar problems when creating sheet metal parts? We bend all of our stuff in house so I need correct flat pattern lengths. Please help me, I am desperate for an answer.

Thanks you.

Kevin Bartok

Here are 2 sample parts with a thickness of 0.100" and a bend deduction of 0.1875" and a radius of 0.0625". The first file has the correct flat pattern length and it utilizes all OD (outside) dimensions. (5OD + 5OD + 5OD) - (2 x 0.1875) = 14.625" which is correct in theory. Now the second file has one ID (inside dimension) and 2 OD dimensions. This file has given me a flat length of 14.825". Now the way we calculate our flat patterns is OD to OD subtract one full bend deduction, OD to ID subtract a half of a bend deduction and ID to ID subtract no bend deduction. With this theory my flat length should be as follows (5ID + 5OD + 5OD) - (2 x 0.9375) = 14.8125". Now the 14.825" flat pattern is telling me that Solidworks utilises this formula (5ID + 0.200" + 5OD + 5OD) - (2 x 0.1875). So it adds the thickness of the material for ID bends and then subtracts the bend deduction to get the flat pattern length. Is this actually correct or is our theory wrong? Maybe some of the more experienced sheet metal designers can comment on this. When I use the solidworks flat pattern, the guys on the shop floor tell me my dimensions are too long or too short.

Also, there actually does seem to be a glitch when using fractions as opposed to decimals. When I first did the part using a 3/16" bend deduction and then changed my units to decimals, my bend deductions changed to .1719 which is 11/64" not 3/16". Maybe this needs to be reported?

## Attachments

The problem in your theory is that you are not using it correctly.

The rule of thumb is based on the material thickness.

You're material thickness is 0.100" and your deduction per 90 degrees 0.1875" (should be twice the material thickness = 0.200)

Once you start getting away from the material thickness (because this is just a rule of thumb and not very accurate) and the deduction per 90 degree bend of 0.1875 could be more accurate your trick of OD/ID doesn't work anymore.

Just do the math by hand on a 1/4" THK channel with a bend deduction of 1/2" per 90 degrees.

We know that a 5"OD would mean a 4.5"ID on a 1/4" channel bottom so both channels are the exact same in the sample

Sample OD to OD: 5OD x 5OD x 5OD out of 1/4" material ----> flat pattern 5OD + 5OD + 5OD - 2 x 1/2" = 14"

Sample OD to ID: 5OD x 4.5ID x 5OD out of 1/4" material ----> flat pattern 5OD + 4.5OD + 5OD - 1 x 1/2" = 14"

So I would just go with your bend deduction of 0.1875 if that works better but than you can only use OD's

Bending Allowance

BA = 2(R + T) tan (alpha/2) - (.01743R + .0078T)Alpha

Where:

T= Material Thickness

R = Inside Bending Radius (This depend on tool, material and process, for approximations you can use 0.85 x T)

Alpha = Bend Angle in degrees

BA is developed at the neutral axis of the material by the angle "Alpha". Neutral axis (or neutral fiber for normal steel is at 0.44-0.45 of thickness from inside bending radius).

K-Factor = Position of neutral axis in relation to inside bending radius as percentage of material thickness (for normal steel process on a press brake use 0.45)

This are "approximated" values, for exact values you will need to know the exact bending radius and exact position of the neutral axis which as mentioned depend on the tooling, material and process.

We bend everything in house too and never have this problem.

It all depends on what you fill in in your bend deduction table.

We use K-factors and if the flat pattern does not come out right it means your bend deduction table isn't right.

You fill in the bend deduction table solidworks does not do this for you because it is different on every machine.

If you do a search in the Solidworks help file for "Sheet Metal Gauge/Bend Table" it explains how to set up the table.

Here is also a link that explains some things http://www.sheetmetalguy.com/tips_bend_table.htm

Good Luck.

Check the settings in

Tools > Options > Document Properties > Units?Is the

Fractionscolumn set to16?Is the

Morecolumn option set toRound to Nearest Fraction?