I am having trouble going from a 3-D sheet metal drawing with the correct dimensions to a 2-D flat. I have hand calculated the bend deductions for the metal that I am needing to bend. In This case Stainless Steel. When doing hand calculations the parts outer diameter (OD) is 6.5 inches. This part has 4 bends in it, after doing the bend deductions the OD for the sheet metal should be 6.06 inches, because the metal stretches as you bend it. Which I am not getting when flattening my 3-D part. When I flatten the part the OD is 6.079 inches and should be 6.06 inches. Is there anyway to change the bend deduction settings in Solid Edge St8 to give me the correct dimensions? Or am I doing something wrong? I am trying to draw the 3-D parts in 2-D, and send them to our machinist to punch the parts out. Also the more bends I have on my part the the more the error in my calculated number and the number Solid Edge is giving me increases.
You'll need to look at your mateial definition [shortcut = double click on the material identifier in pathfinder], more specifically, the neutral factor on the "Gage Properties" tab. This is a variable that needs tuning to match the tooling, degree of bend, thickness, etc....
Design Manager Streetscape Limited
Solid Edge ST10 [MP2] Classic [x2 seats]
Also note that you can create custom Gae tables!!!
I dont do this so you will need to read up on this in SE help: https://docs.plm.automation.siemens.com/tdoc/se/107/help/#uid:material6d
or, I believe that @12GAGE would be a good reference for you maybe.
Thank you very much for your reply. I have been messing around with different numbers and gage sizes for the material and am still unable to get the same cut length as the number that I hand calculated. The material in this case I am working on is Aluminum 5050. The hand calculation that I am doing is for bend deduction and the formula I am using is: total inches of part(Outer Diameter including all flange lengths) – Kfactor* number of bends. The total part including flanges is 6.5 inches and from our bend deduction chart the K factor is 0.095, and the number of bends is 4. This make it so my cut size should be 6.12 inches. When I flatten the 3-D part it is giving me a cut length of 6.033 when I set the neutral factor to be equal to the k factor. Is the neutral factor and my k factor supposed to be the same number? What exactly is the neutral factor? When first opening the part the neutral factor is 0.33. and that gives me a cut length of 6.126 which is close to the cut length that I calculated but is 6 thousandths off.
I hope the way I explained my problem makes sense. If I am not making any sense I can try to explain it another way. Thank you very much for taking your time to try and help me out with this!
Also when doing the same part with 16 GA SS 304 as the material (just for comparison) and redoing the hand calculation using the material thickness the cut length should be 6.06 inches. But when using the .33 neutral factor when i open up the material properties it gives me a cut length of 6.144. In this case when I set the neutral factor to .11 which is the k factor I have from my chart for 16 GA SS the cut length is 6.061 which is only one thousandth off. In the SS case when I set the neutral factor to the k factor from my chart the number is close to my calculated number, but in the Aluminum case the number is closer to my calculated number when the neutral number is not equal to the k factor. So I think it has someting to do with my neutral number but am not exactly sure what the neutral number is.
N-factors, K-factors, etc, depends very high on sheet metall material, bend radius and sheet thickness.
Since You mentioned the correctioon values, You used for manually calculating, it could be, that You have used the old DIN tables therefore.
Assuming, that You have the same bend radius as the sheet thickness is, the DIN N-factor was exactly 0.325
SE always used the rounded value of 0.33
Maybe this small change will bring Your flat to the right result.
But I'm not sure if this will be correct for Aluminium?
Maybe You have an image of the situation, the radius and thickness, so we can make our own test to find out the right values.
The first picture is the 3-D part using Aluminum with thickness .063, second is the flat with the .33 neutral factor giving me a cut length of 6.126.
the third is 3-D part using SS with thickness .060, and the fourth is the flat with the neutral factor .11 giving me a cut length of 6.061
The Aluminum cut length that i calculated is 6.12 and the SS cut length is 6.06.
Al neutral factor .33 give me cut length of 6.126 and SS neutral factor of .11 gives me 6.061
Does this mean that the neutral factor for Al should be .33 and for SS .11?
using a Neutral factor of 0,122 with the thickness of 0.60
results in an exactly flat length of 6.060
a n-factor of 0.313 with thickness 0.063 will bring You the 6.120 for the flat length
The n-factor defines where, within the thickness the neutral zone will be.
0.313 means the neutral zone is at 31.3% from the inside of the material
Nothing more or less!
The material nam eitself has no influence to that.
Depending on Your experience, Your machines, the material behaviour itself, bend radius and thickness, this value let You define the flat length for Your sheet metall parts
There are other methods to calculate this values, so called PZL (plastic zone length)
There You either can use the DIN formular or the bend zone length itself, depending again from thickness, raidus and angle