calculate the k-factor
What is the formula
SheetMetal.Me – K-Factor
In general it is 0.5 X Thickness
But it depends on material, machine and experience.
In my progressive die world, there are too many variables to have an in general answer.
If the inside corner radii is 5x material thickness or more 0.5 x thickness works well.
If the inside corner radii is less or more than 5x material thickness (and how much less )
Type of raw material
Type of bend (wipe, V-Bend, Z-Bend, Roller Rocker, Curl, Etc.)
Amount of pinch used
Amount of coin used
Yes and that is where the experience counts
The K facor is an adimensional "factor"...
You could calculate the Bend deduction (BD) or the bend allowence (BA)...
For 90° bend almost always the BD is 2x Thinkness... ( in my experience)
The K factor most use is .447 for steel low carbon.
You can found more information in machinery Handbook.
I hope I did not say any madness...
K Factor changes depending on the top die radius in accordance with the bottom die width. As a bender I know this for a fact. I have bent many jobs sharp to .008 radius with 4 times the material thickness die width and approximated a .38-.4 K Factor and open dies such as 6-8 times the die width and greater and most often end up with .50 K-Factor. Bending styles also affect this as well. If you are coining you could get a .33 K Factor.
In my 40 plus years I have never seen a K Factor below .33 or above .50. If you do there is something wrong with the measurements or your math. Lower than .3 most likely resulted in a cracked bend in aluminum.
In all the job shops I have worked or consulted at they always had a bend deduction chart that clearly displayed the allowances used. If one wasn't available test bends were performed to accurately determine that allowance or bend deduction. Job tracking sheets or tickets had the bend instructions showing the bend radius if not sharp (.0 to .008) and the deduction/allowance used to program the job. If you as a bender were not able to achieve that allowance the job most likely was rerun with a new bend allowance if it couldn't be saved through clever bending or just bending the job using all of the tolerances available.
If your inside bend radius (IBR) is >= 1.5 * material thickness (t) we have found a K-factor of .44 works very well, i.e., we get a flat pattern and bend locations that yield very good formed parts. For a ratio of IBR/t less than 1.5 the K-factor starts to change rather quickly and it behooves one to make some measurements from sample bends.
K-factors can be very accurate, assuming you use good data. The biggest mistake I have seen is assuming values for material thicknesses and bend radii instead of measuring them. DO NOT use the published values for material thickness, you must physically measure the sheet thicknesses as a few thousandths of an inch can make a big difference.
The attached pdf explains K-factors and how to calculate them and the attached spreadsheet makes the calcs easy. We went so far as to measure coupons made from scrap and bent with each gauge and bend radius combination, and then we created a table of K-factors specifically for our shop.
K-Factor Development.xls 38.0 KB Preview
K-Factor Development.PDF 49.1 KB Preview
Selimcim Tekyazın sitesinde bir excel var. Oradan hesaplayabilirsin
Thank you for sharing your real world K factors.
I didn't see what type or material, or the hardness of the material, in the spread sheet. Was the chart just there as a example and we need to fill in based on our real world testing?
In all my involvement with manufacturing I've always been in search of the universal answer. I'm still looking because I haven't found it! What that means is "what works for one sheet metal shop doesn't necessarily hold true for another", so yes, you need to make your own measurements. I was simply sharing what I have learned (by digging for the information) and the tool (spreadsheet) I put together to calculate the k-factors based on our data.
I guarantee, actually I offer a double-your-money-back-guarantee, that if you make these measurements of a) your sheet thicknesses, b) your bend radii, c) coupon lengths, d) bent flange lengths, and use the spreadsheet to calculate the k-factors, and use those values in your SWX designs you will be very happy with how well the actual parts match the design. Very happy. But you have to do the groundwork and make the measurements and test bends. It is actually a small investment of time compared to the value of the results.
Coupons??? We don't need no stinking coupons. Just bend the laser cut sheet to the print and we will make it work. Tongue was seriously in my cheek for that one.
also include if the shop is ambitious enough to change and use the proper die of they decide one size fits all.
Not to argue of course but to add to this discussion in a helpful way if I may. I ran the Excel file and I found it to be accurate but not when I compared the results to a neutral line formula that I have. We joke that a K factor of less than .3 results in two pieces or a broken part at bending. I am referring to press brake bending. I did add a column to your file so I could determine the actual bend deduction.
So for the first item in your Excel file the K Factor of .11 appears to be incorrect while the others are more in line with what I have experienced in my 40 plus years in the trade. I have added a picture of a many years old Excel file and the Excel file itself as a reference. Then again this refers only to bend deductions. This chart uses a formula that was developed by Westinghouse more than a few years ago.
That is followed by an Excel file I created to have these values adjustable. Of course I will add that this data has been used for many years and on many, many jobs. Your results may vary. (Legal Disclaimer! LOL!) Another recognizable difference in our charts would be that I have material thickness ascending.
While I think it is fine to have designers model parts in SW with a K Factor be assured we will edit the file as necessary to achieve the results required. I model my parts with actual allowances and bend deductions because I know the ones I have work. We actually bend with sharp bend tooling to virtually any radius tooling. That of course depends on the material and grain direction.
Good stuff and valid points. Yes, very tight IBR vs. part thickness is asking for trouble. When I worked on military aircraft we weren't even allowed to use an IBR that was less than 1.5 * thickness.
The file I posted was developed for our internal sheet metal shop for the company I worked for at the time. Now whenever I send out sheet metal I leave it to the vendor to achieve the finished part. I do show a flat pattern with some dimensions, but it is clearly labeled "For Reference Only - Vendor is Responsible for Fully Formed and Finished Article". I also send the vendor my SWX part in some form whether it be a native *.sldprt format or Parasolid or whatever they can use. That way they can make the flat pattern using whatever parameters work for their shop.
At one of the shops I worked at we did tons of work for Pitney Bowes. They would supply us with Pro-E drawings with the same flat pattern you speak of. I imported the .DXF file version of that flat into AutoCAD and 'stretched or shrunk' their flats as required to match up with our bend allowances but used the majority of the flat 'as is'.
As discussed by Forum Members there are lot of parameters on which your K factor depends.
In my earlier work we used to Generate K-factor/Bending allowance by following this method.
1.Cut a blank of 100x100 using Laser or TPP (same process will be used for manufacturing of our product)
2.Bend the blank in "L" profile.
3.Measure the dimensions of bends and subtract thickness and 100mm will get me most accurate bending allowance.
4.This Bending allowance can be used in solidworks directly or calculate K-factor using Bending allowance in solidworks.
This is time consuming process.Once you generate a table of values.you will get most accurate flat patterns
For anyone looking for just a general formula, here is what I have. Note: you will need a couple of pieces of information, which will vary by material, gauge, and tool geometry:
BD (bend deduction): (Distance from outer apex of bend to edge of bend) - (distance from bend line in flat pattern to edge of material)
IR (inside bend radius): might be difficult to measure, but a good approximation is 5/32 x bottom die width, for air bending. (make sure you are using consistent length units)
A (bend angle): The amount the bend is angled up from the flat pattern state. If you are setting this up experimentally, 90 degrees is the most natural choice. NOTE: This can actually be easy to get confused, because an acute bend is GREATER than 90 degrees, whereas a bend less than 90 will form a more shallow, obtuse angle.
K = ((360*(Tan(A/2)*(IR+T) - BD) / A * PI) - IR)) / T
Where A = bend angle in degrees
IR = inside bend radius
T = material thickness
BD = Bend deduction
PI = 3.14159.... (etc.)
For A = 90 degrees, this equations simplifies to:
K = ((4*(IR+T) - BD) / PI) - IR) / T
The above can be derived from understanding the physical relationship between K and the bend region.
In the bend region, the inside of the bend compresses and contracts in length, while the outside stretches and expands in length slightly. The surface within the material that separates these regions of contraction and expansion can be thought of as a "neutral surface", in the sense that it neither expands nor contracts. This surface will be the same length in the formed state as it is in the flattened state.
K is the ratio of the depth of that neutral surface to the total material thickness. So a K of 0.5 means that the "neutral surface" occurs exactly half way through the material. Knowing the flattened length of the part (and thus, the length of the neutral surface) relative to the formed geometry, we can calculate the K factor, as in the equations above.
a lot of really good comments on a complicated thing to get to work right, here is a bend table that I have used in the past with great success
we used to have similar table for our design team.
works like a charm.
hi. I've had our shop bend sample pieces of every thickness we have. Now I'm trying to decide if using K-factor or bend deduction is going to get us better flat lengths. I'm inputting physical dimensions into a spreadsheet, and k-factor is varying from .25 up to .5. But a sheet metal gauge table in SW only allows for one k-factor for the whole range of thicknesses, doesn't it? So would you recommend that I try bend deductions instead?
Joseph Sensenig, Bravo! You are doing the right thing by bending samples and computing the k-factor. Be sure to measure and use the actual material thickness, not the published values, in your calculations.
SolidWorks can use a different k-factor for each bend if you want. I only do a little bit of sheet metal anymore so I don't have the gauge tables setup to use a k-factor. We just kept the information handy and looked it up as we needed it. Our k-factor information gave us such accurate results that we were able to compete with much more expensive shops.
Ok, I'll check into how to incorporate different values on one sheet. Thanks.!
To me it doesn't matter what you use but it has to be accurate and repeatable. I have always used bend deductions and allowances, never k-factor really. I understand how it works and how it is accurate for the most part but if I had a chart that has been basically the same for more than 40 years that is what I'll go by. You did the right thing by test bending to those pieces and I have to ask did you record what top and bottom die they used? That's why all of our shop travelers had those listed as well as the bend deduction you were to achieve, if you didn't get that was there something wrong? Did the bender use a different top or bottom die that was listed? These are factors that are pretty much absolute, though benders that came from a different place may have a different idea on how they used to bend a similar job, that was there, this is here.
I used to bend a lot, then more so lately I became interested in the design end so I familiarized myself with SW. My last 10 years were with AutoCAD and SW, more SW than AutoCAD. You can 'rough' a job with k-factors and it's likely to come out well but if you want to really produce accurate parts I would suggest you use deductions and allowances as they apply. If you want your SW flats to go direct to your programming system I would again suggest deductions.
Getting back to the travelers, would any of your guys understand what the k-factor means and how it relates to their setup of any job?
At one of my last places three of the four programmers never even bent a single job, I was the other one. Consistency is that important.
Bernie brings up an excellent point about the dies.
When I got to the place I worked we had a royal mess with our tooling and drawings. My predecessor did not have any inside bend radius specifications on the drawings! All our sheet metal was made in our own place so we had responsibility for design AND production. His rule of thumb was "The bend radius is the same as the material thickness." My jaw dropped. I told him to hold out his thumb and I put mine next to his. "Sam, are our thumbs the same?", I asked him. "No" was his response. "Neither are our rules of thumb" I told him. Besides, we had six or seven nose radii tools and about twelve different stock thicknesses AND the radii and thickness values weren't even the same. I was hired to replace him. After evaluating the situation I was able to justify the mothballing of all the press brake tooling and replacing it with new tools consisting only of 1/16" and 1/4" nose radius with only one size of V-blocks for each and color coded to match. We did the coupon measurements and generated our own k-factors, but we did not have the variation of tooling Bernie mentions; we had one set of tooling for a given radius. Yes, tooling certainly plays a role in the flat pattern and therefore must be considered when looking up the k-factor or bend deduction. Our tooling effects were buried within our nose radius differences.
Bend deduction and k-factor can be computed from the same empirical data and will therefore yield identical results. It becomes six of one, half a dozen of the other and comes down to what is most convenient to use for your situation.
Material type, actual thickness, and tooling are the most important factors in determining k-factor/bend deduction. To a lesser extent grain direction also plays a role, but most people find the difference is not worth the effort to distinguish. We did a quick study and determined the k-factor for one condition we .44 and for the same condition with a perpendicular grain direction the k-factor was .425. For most of our sheet metal this resulted in flat pattern differences of less than .001". It all depends on your needs whether or not to go to that level of detail.
The big lesson here is you really must develop your own data for your own situation. The great news, Joseph Sensenig, is that you are doing just that. Congratulations! You have just separated yourself from the great mass of people that haven't done this. You will see very good results and be glad you went to the effort to generate the valuable data.
One tip I'd like to suggest is that you periodically recheck the stock material thicknesses. Sometimes mills make slight changes and sometimes your purchasing department will buy from someone else. Nobody tells you about this, but thickness changes will have a pretty significant effect on the flat pattern. When we discovered this we were able to make appropriate adjustments and keep our excellent results without having to add more money to the product.
Thanks for your input, Bernie and Dennis. it is helpful.
Yes, Bernie, the shop did record which top and bottom dies they used for each thickness of sheet metal. I look forward to getting my new gauge table set up.
Retrieving data ...