Hello,
I am working with high strength steel grade S700MC and I would like to know if somebody here work with it and which parameters you use in SW for it. I think the K factor should be between 0.4 and 0.5 but difficult to have something accurate with our trial a 0.05 change a lot in fact.
Or press brake software use the same rule for unfold S355 and S700MC for me that is wrong but I need your help for find out.
Hope that make sense.
Thanks,
Hi Arnaud,
One way i have used to find the k-factor is to physically bend a few sample pieces and calculate it from there.
SheetMetal.Me – K-Factor
This link might help you out.
Note this will be the k-factor for the material on the specific press brake, it could be slightly different on other machines?
Hope this helps,
Hi Duncan,
Thanks for your help. With the tooling I have for check, my K factor can vary approx +-0.5 and that seems to be a lot. My average on 4 pressing + 3 measures by pressing is 0.4013 but that looks small compare to the other value I can see on internet for hard steel (I can't find any value for high strength steel). On fine plate that is not a problem but on thicker plate that can be. The trials was with 5mm S700MC top tool radius 12mm and vie 50mm.
I also created my sketch to be more accurate than just a 90 deg bend 
Someone working with high strength steel can maybe help sharing his value ?
Thanks,
Hi Arnaud,
The k-factor depends on material and bend tooling. Even identical materials can have significant differences in bending results depending on the mill certificate. Meaning sometimes you need to make a test strip for each batch of raw material. Especially if you require close tolerance bending. So the simple answer is that you have to get your own data from trial bend test if you want accurate values.
Some High strength alloy tend to stretch less that's why your k-factor will be lower. But that also depends on the material thickness, bend radius, bending die, bend process even break press size & ration of bend strip width to brake press max. span.
Elmar
We always test bent samples to get really accurate bend deductions, I never use a K factor really. I would like to offer a piece of advice though, on these materials I have found that it is better to fabricate the all from the same side. That is, top top is always up. You many really have to look at the material to see this. On some thinner materials with a bend radius 3-4 or greater we have always used a backup piece.
Further to Elmar's comments, grain direction may also be a factor in bending, particularly for strength.
At the end of the day, it all comes down to design intent. How accurate do you need the k-factor to be? can the design be changed to be less reliant on the accuracy of the bend? personally i don't put a lot of accuracy into sheet metal as it can and does change part to part.
Also you're working with high strength steel, so i'm guessing this is more of a structural application. how many bends are you working with?
One last point is to be careful what you read on the internet. go with your test pieces, they are going to be most accurate to your material/tooling.
Thanks all for your comments.
With fine material thickness I am agree the accuracy of the K factor is not a big problem. But on some critical application that should be. In fact, with high strength steel you need to have the minimum gap between two parts for welding otherwise the weld is weak. I manly working with multi bend part for move the weld in low stress area. Bellow some examples :
Also the K-factor with thicker plate change quick a lot the flat pattern length. Bellow example wit 0.3 vs 0.5 I have 6.3mm difference :
When you design a part you design the part with the tool radius or the true radius of the part after pressing ? Which tooling do you use for check the inner bend radius of your part for calculated an accurate K-factor?
Arnaud Henry Lefort, here are some comments and calculation tools for K-factors.
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.
Arnaud Henry Lefort wrote:
When you design a part you design the part with the tool radius or the true radius of the part after pressing ? Which tooling do you use for check the inner bend radius of your part for calculated an accurate K-factor?
We always used the nose radius of the tool. Bernie Daraz has also pointed out the width of the V-die plays an important role in these values. For the work I did we had standardized on the V-dies so they did not change, but if you have different widths then you need to consider that as well.
Hi Arnaud,
These look like boom components. You also have various bend angles. That makes things a little trickier. There is a good DIN 6935 Standard "COLD BENDING OF FLAT STEEL PRODUCTS" that can be incorporated with sheet metal gauge tables. The attached file explains the principle idea. It's in german but the formulas are international anyways. The standard will list the v-values used in the formula (see snap shot..I hope posting half a snapshot is okay with the document owners). But even this will not save you from making test strips but it handles all ranges of bend angles.
I have done sheet metal like yours before without going to the extreme and still be able to hold tight tolerances. A good press brake operator and proper part design will handle some of the tolerance variations due to material stretch. It also depends on how you dimension your bend lines.
We use scribe marks but proper care needs to be taken to avoid bend cracking.
I keep forgetting to ask what are the tolerances?
If you're close now that's great. On the next run measure everything accurately, then bend and measure again. I can't tell you how important this part is.
Every time you run this job again, do it again. I mentioned material top and bottom before but I forgot grain grain direction. The bends will be different.
Thanks for your answer. Sorry but I can't fine the PDF and Excel attached ?
Yes on my trial I started assuming the material thickness is perfect but in fact not. With S355 it is worse compare (4.9 / 4.92 mm for 5mm nominal thickness) and not to bad for high strenx steel (5.01 / 5.02 for 5mm nominal).
When we bend a 5mm with 6mm top tool radius and 50 mm V the true part bend radius approx 7mm but it is extremely difficult to check it. The bend radius doesn't seem to be perfect. It looks to start bigger approx the top tool radius on the middle and finish bigger again.
We would like to achieve something like +-1mm on material from 3 to 10mm. That seem to be achievable ?
I need to check the grain direction as well.
Hi Arnaud,
Grain direction has certainly an influence when bending. It also affects overall strength of your final piece. If and how you need to consider grain direction in your fabrication process depends on many factors. There is simply no set rule that you need to bend across the grain.
It means you need to be aware of it in case your design and fabrication process are really affected by it. The following link sheds some light on grain direction and minimum bend radius. Bending Basics: The fundamentals of heavy bending - The Fabricator
As a tip. Dimension symmetric parts from center line. If the press brake operator was to use your drawing dimensions, it would almost certainn that he will be out of tolerance.
Do you think grain direction impact the K-factor or only the minimum bend radius ?
For the bend radius I always follow the guideline from our supplier and use the bigger minimum bend radius between along the rolling and transverse the rolling.
Our press brake operator didn't use the drawing how it is, dimensions are for inspection. Trouble is our press brake operator mostly use the bend lines generate by our press brake software from a SAT file of the final part but event if we change the material our press brake software generate the same DXF and bend line than S355 steel so I am trying to find out why.
Hi Arnaud,
Grain direction does affect your k-factor. As it does affect spring back, forming force and component strength. The question is not if it affects it, the question is, is it significant to your application. You seem to use 3rd party flat block layout software and don't seem to use the flat block created in SW. You will need to look into how your software operates. Maybe you should talk to your press brake manufacturer or the software supplier. They will be able to tell you what parameters affect the correct stretch out.
I think this discussion revolves around in an endless loop. My suggestion is that you take some of the advice in this post and apply it. If your tolerances are critical and if material is crucial in your design along with all the associated costs, then you should have no problem to spend some time and money on testing. Ultimately only testing will prove that your assumptions are correct or not. For that you need to start somewhere. Take a stab at it and compare the results with your theory. If it works out okay, great. If you find deviations then you will have to make adjustments and so forth. Try to nail down the critical parameters and make sure you check your test pieces before and and after bending. That is critical or you will not be able to tell what sources actually contribute to your variations.
Good luck,
Elmar
Arnaud Henry Lefort wrote:
Thanks for your answer. Sorry but I can't fine the PDF and Excel attached ?
You have to log into the forum to see and download the files. You cannot access them from the e-mail notifications you get.
Arnaud Henry Lefort wrote:
We would like to achieve something like +-1mm on material from 3 to 10mm. That seem to be achievable ?
I need to check the grain direction as well.
This is absolutely achievable provided you do the following:
1. MEASURE and follow the procedure I outlined in the pdf and spreadsheet. (This is actually very easy to do, but too few people want to be bothered with making an actual measurement or two.)
2. Use the tooling nose radius as the inside bend radius and the computed K-factor in SWX.
3. Use the SWX flat pattern and its bend line locations in the press brake. (Press brake operators are notorious for adding their own adjustments based on their experience. INSIST on using the values that SWX generates for the backstop to bend line setting.)
4. Verify all this by making a simple strip (measure the length and thickness prior to bending) and doing a simple 90 degree bend. Measure the bend lengths. Check it in the calculations. You will be impressed if you did everything correctly.
Yes, grain direction affects the springback as Elmar Klammer states. so pay attention to the grain direction in your test coupons and your actual product. The difference due to grain direction is typically small, but it is there. Why not get as much accuracy as you can?
Hi Dennis,
Since you asked the question: Why not get as much accuracy as you can?
The simple answer: Cost.
You want as much accuracy as you need! Big difference.
Not trying to be a smart ass...but it makes a huge difference. Look at anything that is worth taking into account. Leave the rest.
I once worked with a data miner who said "I love data. The more the better" It wasn't surprising that his work provided little transferable insight. Why make yourself do more work then necessary. Mother Nature doesn't do it and I believe for very good reason.
Elmar
Dennis Dohogne wrote:
Arnaud Henry Lefort wrote:
Thanks for your answer. Sorry but I can't fine the PDF and Excel attached ?
You have to log into the forum to see and download the files. You cannot access them from the e-mail notifications you get.
Also, you can't see attachments from inside your inbox. You need to click on the header to open the thread individually to see the attachments.
Elmar Klammer wrote:
Hi Dennis,
Since you asked the question: Why not get as much accuracy as you can?
The simple answer: Cost.
You want as much accuracy as you need! Big difference.
I agree 100%. I was sloppy with my wording but was simply supporting your statement that grain direction does make a difference, though it is a small one compared to other things. If it is an important difference, i.e., the extra precision warrants the little bit of extra effort to get it, then it should be duly considered.
If someone is making some test strips and measuring them in order to determine the k-factors then it is a very small effort to include a few extra test strips and measurements done with a cross-grain direction.
Morning All,
Just for let you know I solved my issue with one part. The correct K factor for 3mm plate and 5mm top tool radius is 0.37 for us.
Thanks,
Yes Bernie only bend test samples with the same material and used tooling will get you spot on.
I learned this from u and now all our nerby competition wants to know how the hell we can produce part that have 10 bends and overall accuracy is like a human hair.
K factor so called rule of thumb is the biggest mistake that can be done. If i care about my work, I get my samples bend untill I am 100% sure it will produce part with tolerances 0.0mm.
I never use KFactors or deductions from somebody else. No way ever. Thats like asking my baby to get brest milk from my neighbour!!!
Fred Vraj wrote:
Yes Bernie only bend test samples with the same material and used tooling will get you spot on.
I learned this from u and now all our nerby competition wants to know how the hell we can produce part that have 10 bends and overall accuracy is like a human hair.
K factor so called rule of thumb is the biggest mistake that can be done. If i care about my work, I get my samples bend untill I am 100% sure it will produce part with tolerances 0.0mm.
I never use KFactors or deductions from somebody else. No way ever. Thats like asking my baby to get brest milk from my neighbour!!!
how do you generate the correct flat pattern without accurate K factors or deductions in the CAD?
And yes, I understand the issues listed above such as bending changes with grain, etc. but you need a good average K factor to spit out the flat.
I dont design without Kfactor or Bd. I test small offcuts and this gives my absolutelly spot on BD that I use in solidworks special test models. Those will give me Kfactor.
My Kfactors are 100% acurate for our tool.
dear andry,
i work with S550MC high strength low alloy steel with 760mpa UTS and 550mpa YS.
can you guide me with the K-factor for Press brake bending - Air bending.
Morning All,
Just for let you know I solved my issue with one part. The correct K factor for 3mm plate and 5mm top tool radius is 0.37 for us.
Thanks,