Sheetmetal Blank Size Calculating

Hi all,

I’ve just commenced working with a fabrication company. We receive a lot of sheetmetal requests from customers and while I have some experience of basic sheetmetal design on SolidWorks I am not up to speed with fabricating it and all the nitty grityy things to consider.

I received a set of drawings from a customer recently and need to calculate my blank size (total flat pattern size) which I believe is based on the outside dimensions minus the material thickness. I can’t seem to find a standard formula to verify this.

In the attached image for example (apologies for poor quality) would I need to do the following:
• Subtract 1.5mm from the top horizontal 25mm dimension
• Do I subtract thickness again from 110mm?
• I believe for the 46mm dimension I subtract 2/9 of thickness from 46mm
• Not sure about the 39.38 or the 23.38
Perhaps one could point me in the direction of a good Youtube video?

Are you familiar with terms like K-Factor, Bend Allowance, and Bend Deduction? These are the things I would look into and learn about and everything should fall into place. I use Alibre Design (CAD) for sheet metal design. You specify materiel thickness and K-Factor (a lookup value for known materials and bending processes) and it calculates the rest. The software can flatten the finished part and you have the dimensions of the sheet metal before bending. I think Solidworks does the same. Else you can calculate it all by hand. Searching the net for sheet metal design k factor gives lots of good info like this Calculating Bend Allowance, Bend Deduction, and K-Factor

As for your specific questions I have no idea where you are getting the 1.5mm from. Read through the link I posted and I think you should arrive at the solution to your question.

Understanding K-factor, bend allowance and bend deduction is important but in the real world it's still a good idea to do a
couple test bends with the same material you're going to be using. Materials can vary from batch to batch and seeing
how an actual sample bends up can save you a lot of wasted time and material...

Thanks, yes I've read about them but wasn't sure if I needed them for the blank size. 1.5mm is the thickness (forgot to mention that).

PM2.5 said:

Hi all,

I’ve just commenced working with a fabrication company. We receive a lot of sheetmetal requests from customers and while I have some experience of basic sheetmetal design on SolidWorks I am not up to speed with fabricating it and all the nitty grityy things to consider.

I received a set of drawings from a customer recently and need to calculate my blank size (total flat pattern size) which I believe is based on the outside dimensions minus the material thickness. I can’t seem to find a standard formula to verify this.

In the attached image for example (apologies for poor quality) would I need to do the following:
• Subtract 1.5mm from the top horizontal 25mm dimension
• Do I subtract thickness again from 110mm?
• I believe for the 46mm dimension I subtract 2/9 of thickness from 46mm
• Not sure about the 39.38 or the 23.38
Perhaps one could point me in the direction of a good Youtube video?

Click to expand...

OP I have been doing Sheet Metal layout for 30 years and I have something I hand off to new Engineers designing Sheet Metal parts that might help you out to understand Bend Deduction, Bend Allowance and Neutral Axis. K Factor is nice for quoting purposes we have found it is not accurate enough for our Tolerances we strive to hold. We are a precision fabrication shop.

Not sure they type of work you do or tolerances you can hold (target) or the type of Bending Equipment/Tooling you use. But these formulas will get you very close. Then you can develop your K Factors based on theoretical using the formulas and compare to the reality of inspected parts and adjust accordingly.

I know enough about Solidworks to be dangerous and leave that in the capable hands of my younger crew in Engineering. I get all the old school Transition Parts that Solidworks has a hard time with unless you design the part as a "casting" outside of the Sheet Metal module. The current part I am work on is a .060 316L Stainless Header Collector for an Offshore Racing Boat. Merging (4) 2.500 dia tubes into a 4.500 dia over 7 inches inside a Water Jacket...I love my job...LOL...

Send me a PM with an email address and I'll reply with the formulas. They are in a PDF format and I cannot attach them to this board. Email is so much easier than a message board.

I was the supervisor for the shearing and bending department of a steel supplier before I started my own business.

The rule of thumb I always do is you never have to remove thickness for bends up to 45*. A 45* will basically be the same inside and outside.

It also depends on the kind of punch and dies your using, if using the standard 8x bending rule or custom.

If critical, just do a sample bend, it is always the safest route

Sent from my 2PS64 using Tapatalk

Blank size is determined by many things. The most important factor is Voo Doo. Science can get you very close. Grain direction and thickness tolerances can kick your butt a bit. Bottom bending and coining really have their uses, but air bending gets you all of the funky angles in between.
I have a Delem control on my Brake and trust that more than Solidworks. But the Delem control has tables based on the Trumps punches and dies I am going to use. Almost all air bending. True that the tables never over bend the material, and part sizes are what I need.
Google Solidworks sheet metal stuff. What I got from that is that I need to take a few days with a lot of sheet metal parts to get the tables as accurate as possible foe SW to give accurate blank sizes for the laser.

After farting around with inaccurate bends for several years (being a shop with engineers and non sheet metal machinists) I finally took the bull by the horns and actually measured bends in every thickness of steel and aluminum we normally use and with every reasonable combination of punch and die. This involved bending 4" long parts into an L and measuring the inside bend radius with a radius gauge and the length of each resulting leg with a height gauge. These numbers with the thickness let one calculate k-factors and then make Excel tables for Solidworks that you access from the sheet metal functions. This allows us to bend with a tolerance of around .01" per bend which is good enough. This is on an Atek B412 12 ton bender with a CNC backguage from Atek. I recommend this approach if you have CAD software. It will take a couple of hours and the payoff will be for years. For reference we have 1" and 3/8" opening dies. We use the smaller one for most bends up to 16ga and the larger for 14 and 12 ga. Solidworks lets you have different dies so we have settings for the larger die on thinner material if you want to do a longer bend or larger radius bend for example.

OP here you go...let me know if this makes sense. We are job shop feeding 24 Press Brakes 20 hours a day.

I have attached a "Form Sketch" that I would send to our Press Brake Dept. The key is to use a uniform dimensioning technique. We lay everything out based on Outside Apex, no exceptions!!!. Ref dims shown on the sketch are what we call "Caliper" readings to help the Set-up or Operator dial in the back gauge.

When you use Outside Apex Dims is it much easier for the Set-up/Operator to us a Bend Deduction Chart based on Material Thickness, Inside Bend Radii and Angle to program the Back Gauge (Bend Line = Apex Dim - .5 the Bend Deduction). As rcoope pointed out real data developed over time will get you these Bend Deductions you can set-up in Tables.

Hope this helps.

You sure went to a lot of effort there - I am really grateful for that. I will have to spend some time going over it. In the meantime I dug out a table that has recommended die, internal radius & kfactors for different thickness materials so the same approach was applied. I just need to go and start plugging these values into formulas and figure out how it works I guess. Thanks again.

If you look around on the Trumpf website you will find a free Android app with die openings for different materials and thicknesses. Tonnage, min flange lengths, and a lot of other calculations. Metric and English too.

If you are sending out parts as RFQs, DONT LAYOUT THE PART FLAT. This was a pet peeves of mine when I was a full time sheet metal mechanic for ten years. All shops use diff die and punch nose radii, so your flat layout literally means nothing to any given shop. Send them the isometrics, and any good mechanic will bang out the numbers in a split second. I can't tell you how many times clients have sent flat drawings with incorrect deductions that messed up mounting hole locations.

E.F. Thumann said:

If you are sending out parts as RFQs, DONT LAYOUT THE PART FLAT. This was a pet peeves of mine when I was a full time sheet metal mechanic for ten years. All shops use diff die and punch nose radii, so your flat layout literally means nothing to any given shop. Send them the isometrics, and any good mechanic will bang out the numbers in a split second. I can't tell you how many times clients have sent flat drawings with incorrect deductions that messed up mounting hole locations.

Click to expand...

Our rule of thumb is: All flat supplied by the customer are for reference only.

While I understand your concern I find that when I have 25 quotes to get done in a short period of time having the flat make it much faster on complex parts. In a quick second I know the Blank Size, again it is not the real Blank Size we would use but it is close enough for a quote.

I can count the number of Bends, the number of holes and the number of punches if ran in the turret or take the width x 2 + the length x 2 x a multiplier to get the linear inches of Laser and build the quote from there.

Some of the Frames we quote are weldments made from 150+ pieces of Sheet Metal. Having supplied Flats for ref sure speeds up the process. And when the hit rate on quotes is less than 50%, sometimes as low as 30% I would rather invest as little time as possible in the quote. Once we land the job and have a PO in hand we will invest the time to "finite" the Model to make it manufacturable and produce the correct flat the Shop can run to.

Based on the customers dimensioning technique on the print/part shown below, I would have invested more time in calculating the Flat than completing the whole quote.

To the OP:
I'm not a sheetmetal guy with 25 years experience every day, but I have found that the fundamental formulas that are published in Machinery's Handbook ("Press Work" section) are quite adequate to get you very close to ideal blank sizes. I have run a press brake bending plastics and metals, and done a lot of prototyping and small qty work on a finger brake, and I have found the calculations to be fairly accurate. There are many other sources for this info in the golden age of the internet....

As others have noted, test bending, using the setup and material of interest, is usually the most reliable way to determine exactly what you want to know.

This thread is old, but wanted to put this here in case it's helpful for anyone who finds this. This article goes over some blank size engineering using LS-DYNA for the automotive industry. Blank Size Engineering in Dynaform | ETA, Inc.

To figure the bend allowance around a bend in forming sheet-metal.

Sin of 1 degree X arc X (inside radius + 1/3 stock thickness) = Developed Length around the Bend.

Just took a look at how the piece part dwg. is dimensioned in your example. It leaves something to be desired. Should be Dimensioned to the Center of the Radii and provide Inside Radius of the part. It's a guess as to the true dimensions of the part.

Roger