sheetmetal, flat patterns, bend allowances

We are having a heck of a time getting flat patterns to come out correct. It seems like everyone in the shop has some kind of different formula to achievee a correct part. When the guy does the programming thru metalsoft manually, we have few patterns. But when we use a flat pattern from solidworks (created by sheetmetal, flanges, etc.) everything comes out way off. It isnt even close to what it should be. We tried the tables right out of the machinest manual for the material and size. BAD PARTS. We tried punching in the numbers the guys in the shop use. BAD PARTS. We tried using what the Metalsoft programmer uses. BAD PARTS. We need to get this flat pattern to the point where we dont have to go thru the extra steps of another person redrawing it in a nother program. Any ideas where we are failing. I had a part today with 13 90 degree bends. It came out over 1" off from the machine???? Thanks for all the help anyone can give. Jake Barron

Reply to
Loading thread data ...

o.k., good ol' bob z. has no actual sheet metal experience, but your post has bob z. troubled. very troubled. is/was there any consistency between all of the parts coming off of the machine that were designed to the different formulae? for example, if you created the part in swx using the machinery's handbook and then created the same part using the shop dude's criteria, did these two finished off-the-machine parts have the same error? bob z. knows this sounds a little obvious, but it sounds like the problem really needs to be simplified. ya know? take out some of the variables. pick a formula and stick with it till you get it to work. bob z. would probably pick the formula that the shop dudes use. why? ya gotta be friendly with them guys!

o.k., bob z.'s post sure didn't help you in anyway, but maybe... maybe... it'll help somebody.

bob z. p.s. curse this dreaded alcohol addiction!

Reply to
bob zee

what method bend table, k-factor, bend allowance or bend deduction are you using to calculate the flat?

bend table & bend deduction work well, results are very predictable. bend tables are nothing more than a list of bend deductions for varing radii & material thicknesses. the table will interpolate for angles other than 90. hth

Reply to
kenneth b

Do you mean few "problems' ? Or he just doesnt get much work done?

I've done my flat patterns both (and more) ways; including using MetalSoft (Fabriwin)

I soon discovered that to allow my Solidworks Flats to come out the way they they were being done manually, I had to change my K-Factor to .28.

Why? Because a .28 K Factor, using a bend radius equal to the stock thickness, returns the same valuse as the Bend Radius on 90 degree bends! Somehow they thought/think that doing a second equation of adding a fudge factor to the pseudo-bend allowance was saving time.

Example: .125 stock. .125 Bend radius, 90 degree bend, .28 K Factor = .125 bend allowance

If this is what's being done on your shop floor, and there is no chance of convincing them to do it correctly, then update your models accordingly :/

Another thing you may want to check is that the correct SIDE of the base face is checked. Inside vs outside allowance can make all the difference.

Thirdly, I dont use the OLE in Fabriwin to import a Flat Pattern from an open SolidWorks model.... 'things' happen to it. I export my flats from a SWX drawing.. either to DXF, or directly to metalSoft .prt format.

MetalSoft uses a low precision internally... and while 6 decimal places may seem fine in sheet metal, thats also only 6 decimal places using 'Pi' and any trig... Round off errors show up often in arcs and non-orthagonal lines.

Reply to

I use the OLE in fabriwin all the time, sometimes I have had problems with lines that were smaller than .001 modeling errors. I have also had problems with parts that have both new and old sheetmetal features. It supressed everything between the new flatpatern feature and the old features. I remedy this by making a mirrored part since the mirror of a flatpattern is just cutting from the other side. I tried to submit that to their development team and they always say it will be fixed in the next release but it never happens. SW has a much better system of getting releases fixed beleive it or not than any other software I have dealt with.

We always use close to .5 K factor but in our shop they say if it is within .25" it is good. So I never know how close it actually is.


Reply to
Corey Scheich

All we do here is sheet metal for pizza ovens. Stainless steel 20 thru 12 gage. Darn tough stuff to work with. The material properties vary from middle of the sheet to one edge, etc. We had to 'discover' the inside radii and K factors based on our tools. For instance we use K = .41 and inside radii = 1/16" for our Safan (dang nice machine) press brake loaded with Wilson Euro tooling (also nice) for the 18 gage stock. It took a little trial and error to get this, and we usually can hold +/- 0.015" or better. Operator, machine setup, and technique probably has more to do with holding close tolerances. There are a million variables besides the software. Solidworks has been a real time saver for me, and its sheetmetal capabilities was the primary reason I bought it to begin with.


Reply to
Gary Wolfe

You need to have your sheetmetal guys do some 90 degree test bends to determine what the bend deduction of the material is that you are working with. For example, where I used to work, #4 SS 16 Ga. had a bend deduction of .110. We determined this number by bending up some test pieces and finding out how much the material stretched. This number will change depending on material, dies and even the brake. So a 1"x1" L-shaped part needs to have a flat length of 1.89. You subtract .110 for every bend in the part.

So we simply put that .110 into a bend table and the parts came out nails. We had different bend tables for each different material. We only had one brake, so we didn't have to account for different tools. The use of a bend table allows SolidWorks to calculate angle other than 90 degrees

Reply to
Jeff Chambliss

WE DO A LOT OF SHEET METAL WORK! And have only recently discovered that the bend radius has nothing to do with the top tooling, but the bottom v block! If you send me your email address, I will send you our formulas for 1mm to

4mm sheets. this ensures that the notching is also correct when using the bend deduction option.

Reply to

PolyTech Forum website is not affiliated with any of the manufacturers or service providers discussed here. All logos and trade names are the property of their respective owners.