K-Factors: Let's Share Info 2

[DennisD]

I have recently seen several references to sheet metal flat patterns, in particular, flat pattern calculations. The common techniques for calculating "accurate" flat patterns involve using bend deduction tables or the K-factor. Very often what people use is some general data that may or may not be close enough.

Since we design parts for others to fabricate our procedure is to detail the finished part that we want, including the bend radius, and hold the fabricator responsible for achieving that part. We do, however, provide a dimensioned flat pattern "For Reference Only". We clearly mark this flat pattern sheet as such and we reiterate the material, thickness, bend radii, and the K-factor we used to calculate the flat. Often a fabricator will make their adjustments to our flat pattern. (We also make the flat pattern as a sanity check on our part design.)

Our preference for calculating flat patterns is to use the K-factor. It is dimensionless so metric/inch is not an issue (as it can be with the bend deduction tables). We have had several folks conduct some cursory research and (not surprisingly) come up with different results. The Machinery's Handbook has good information but it is too general for our satisfaction.

We have learned this much:
1. K-factors are a function of inside bend radius and material thickness.
2. K-factors are also a function of material type.

Since our press brakes (in-house and at our other vendors) have a set of standard bend tools and since the available materials come in standardized thickensses, we have set up a simple table in Excel. The rows list the standard bend radii, the columns list the standard thicknesses for the materials (aluminum, cold-rolled, stainless, etc.). The table is populated with the appropriate K-factor.

We are currently using a table populated with values that one of our production engineers came up with based on his interpretation of his research. His data is in some dispute but nobody else either has done the homework or has the 'nads to stand up to this guy.#-) I identified a procedure whereby a set of parts would be measuremed before and after a set of various bends were made to verify the K-factor data, but you can only lead a horse to water. (We are in different departments and I have no authority over him. That's my excuse and I'm stickin' to it!)

I am asking two things with this post:

1. For those of you using K-factors, especially those of you having to actually make the parts, what are you using for the K-factors? How have you developed/verified this data?

2. Which of you clever I API programmers can make a routine that will read the material from the part file property and the bend radius from the sheetmetal information and stuff the K-factor with the appropriate value from the table? 100 points to the first person to come up with this!!

- - -Dennis D.

 

[MadMango]

In my line of work, our end product is about 80% sheet metal manufactured. Working closely with our sheet metal department, we have zeroed our K-factor down to .430 for our manufacturing needs. This K-factor is used in conjunction with known inside bend radii for specific materials and material thicknesses.

This usually results in parts that fall within a +/- .010 tolerance. I know this is huge, but for what we do, it is an adequate balance between usable parts and rejected parts.

The method we used to come to this K-factor was to model several C, U and W shaped strips of our most commonly used materials, and for each run, change only the bend dies used. Once the finished parts were completed, we compared them to our models and if the dimensions were incorrect, we would adjust the K-factor. After about 4-5 runs our enigneering department and our manufacturing department settled on the .430 K-factor.

Our department has two Amada punches, one 3k laser and about 7 breaks of varing tonnage. We work on material from 6061-T6 aluminum to AISI 304 stainless, ranging anywhere from 20ga to as thick as 3/8 plate. "The attempt and not the deed confounds us."

 

[Stoker]

If you are marking any mechanical drawing "for reference only" I think the question needs to be asked - do your vendors actually use the flat pattern information? I suggest you talk to them and find out. Especially if they are importing the SWX models directly I strongly suspect the answer is no.

As for the API part, I think that it can be done, but the benefits of coding it in the way you have described are limited. For example, since you have to choose the thickness and bend radius when creating the sheet metal feature anyway, what is the real benefit to selecting the
k-factor via the API? It will probably take more time to create the sheet metal feature and then run a second command to update the k-factor than it would to key in the
value directly. Also remember that although a VBA macro could be made to look up the appropriate value, it will not update automatically if the thickness or bend radius is changed. You will have to run the macro every time a change is made to the sheet metal definition. It would take an add-in to watch for changes to the sheet metal definition and update the k-factor automatically.

If you are not fabricating the parts in your shop, I question the need for you to get a perfect flat pattern. Your vendors may have several different brakes. You probably deal with more than one vendor as well. The only time I have found it really necessary to have an accurate bend deduction is when you have a cutout that goes across a bend and you need to accurately control the position of both edges. Other than this particular case I think its better to give the fabricator the freedom to determine the appropriate value.

 

[DennisD]

MadMango and Stoker,

Thanks for your input. You are correct that it is up to the fabricator to make an appropriate flat. We only hold them responsible for the formed part.

We have a need for sheet metal parts with tighter tolerances than the customary +/-.010" and often with multiple bends. We have also found that it CAN be done. I can relate about a part that had two 45 degree air bends and we still hit an 8.000" dimension with a range of only .0025"!! We were ony able to do it by calculating an accurate flat pattern. Months of iteration and voodoo attempts had previously failed. It was only when we contacted Amada and got their flat pattern calculations that we were able to accomplish this. It made a believer out me that there was more science than art to bending metal than we all had thought.

Though we provide the flat "For Reference Only", it behooves us to give the fabricator the best information possible. We give the vendors all the freedom in the world, but know that we can give them a lot of help as well. Most of our S/M vendors do not have SWX and therefore do not have the luxury of automatically generating an accurate flat pattern from the formed part. Also, we have parts that are made by a vendor one day and in-house the next. For the in-house operation WE are then completely responsible for the finished part, which requires an accurate flat. Our in-house fabrication is not much more than a bunch of button-pushers at the press brakes.

As far as the API goes, we currently have a spreadsheet with our K-factors for the various materials/thickness and bend radii. We must open it to look up the appropriate K-factor. While this works it would be nice to automate it. After all, if the SWX bend table spreadsheet were used the bend allowance information would be automatically obtained based on the bend radius and thickness. This technique even interpolates between values. By the way, this would equate to widely varying K-factors, however it doesn't take into account different materials.

An example of the range of K-factors we currently use:
(Note IBR=Inside Bend Radius, t=thickness, K=K-factor, units for IBR and t are inches)
for Aluminum:
IBR=.031, t=.020, K=.3743
IBR=.031, t=.063, K=.2497
IBR=.120, t=.020, K=.5212
IBR=.120, t=.063, K=.3967
for Cold Rolled Steel:
IBR=.031, t=.060, K=.2550
IBR=.120, t=.060, K=.4020

I think the case is sound for this type of K-factor information. I would just like to see someone's data that has been debugged. As far as the automation goes, I don't care if it is API, VB, or whatever. I just thought someone would be able to apply some previously developed technique that reads certain SWX information, i.e., material (property), thickness and bend radius, and look up the appropriate K-factor and poke it into the right spot. I wish I knew how to do customization like that.

How about it guys (and gals)? We're looking to improve operations.

Thanks in advance,

- - -Dennis D.

 

[RannyMeier]

There are API notifications available that pre-notify the user program when the user edits the definition of a selected feature. Therefore if a k-factor add-in is running the sheet metal k-factor will update automatically whenever the thickness or bend radius is changed. There is little overhead used by this monitoring process (it will be un-noticeable).

 

[Psycool]

For DennisD,

You said your company has a spreadsheet with K-Factors for the various metal sizes/thicknesses, right? Do you think you could e-mail me that list? I know it's asking a lot, but I've been trying all day to get an Excel sheet to serve as a bend table.

GregB@FTBSon.com

-Thanks. "I am the Alpha and the Omega" ~Xenogears

 

[DennisD]

Greg,

We found the basis for this information in the Machinery’s Handbook. I have the 23rd edition and it’s not in there. This came from the 26th edition. If I had the 26th edition in my possession I’d be able to give you more detail, such as page numbers, etc.

The values in this spreadsheet were selected because of the standard stock thicknesses we use. Notice that the K-Factors have quite a range, especially between materials. For instance, with an inside bend radius of .030” and an aluminum thickness of .063” the K-Factor is .404, yet for cold rolled steel with a thickness of .060” the K-Factor is .467.

I originally posted because we have other data from one of our engineer’s class notes that indicated an even larger range of values. I was looking for someone, such as a precision sheet metal fabricator, to provide a set of values that have been proven. I tried to arrange an in-house study to verify either the engineer’s class notes or the Machinery’s Handbook, but have not gotten the cooperation necessary to implement it. In the meantime we are using the Machinery’s Handbook derived values.

Please, if you have access to a precision sheet metal fabricator that has confirmed bend calculation data in any form; K-Factor, Bend Deduction or Bend Allowance, have them share that information with us.

Thanks,

- - -Dennis

K-Factors for Aluminum, Cold Rolled Steel and Stainless
ALUMINUM
Thickness
Radius 0.032 0.063 0.100 0.125
0.030 0.398 0.404 0.406 0.407
0.060 0.394 0.402 0.381 0.407
0.090 0.391 0.401 0.380 0.406
0.120 0.391 0.401 0.380 0.406
0.188 0.392 0.401 0.380 0.406

COLD ROLLED AND STAINLESS
Material & Thickness
Radius 0.029 SS 0.048 CRS 0.060 CRS 0.078 SS 0.093 CRS
0.030 0.483 0.438 0.467 0.449 0.459
0.060 0.479 0.433 0.463 0.446 0.457
0.090 0.475 0.433 0.463 0.446 0.456
0.120 0.475 0.433 0.463 0.446 0.456
0.188 0.454 0.420 0.453 0.438 0.450

* from Machinery's Handbook 26th edition.

 

[YJeepster]

You must also take into consideration the size of the bottom Die "V" you are using. (IE. Alum. 0.063 thick (14ga) with a 0.030" rad will have a one k-factor using a 0.236" V and another if using a 0.472" V

Does the handbook tell you the size of the opening they are using to get these numbers?

Also there is a slight differance between CRS and SS

My $0.02

Cheers,

 

[bcolley]

In my opinion you just can't count on using k-factors for high precision sheet metal. Well, I'm sure you can but for solidworks using the bend deduction table is so much easier and much more accurate. For coin bending we have a set take-off for each material thickness, I entered that in at a .010 radius and then I used a formula to calculate all of the other bend deductions for a variety of thicknesses and radii. I have 3 tables: alum., s/s, and crs. I'm interested in following this topic because with all of the experimenting I have done I have not been able to use k-factor because it is not as precise as I want.

 

[Htaed]

I've wriiten a program for figuring BA and press brake set back. The formulas used in it are taken from over 10 years experience in the metal fabrication industry. It is used in the plant I work for and the engineers there found it very useful. If anyone is interested in it please let me know. I'd be happy to share.

htaed@comcast.net

 

[jeanpaul]

Take a look at:

http://www.massey.ac.nz/~odiegel/bendworks/

It is a little pgm with K factor

 

[SWVB101]

Dennis,
I have the eletronic version (pdf) of the 26th Edition...

I believe it is on pgs. 1308-1310

Chapter: Manufacturing Processes
Section: Punches, Dies, and Press Work

Thanks,
--Josh--