AnsweredAssumed Answered

K-Factor for multiple bends

Question asked by Mike Knauss on Feb 2, 2012
Latest reply on Apr 24, 2012 by Lyndon Crossman

Like • Show 2 Likes2
Comment • 21

Hello,

I'm working on a series of sheet metal parts to come up with a K-Factor for various thicknesses of sheet metal, and various number of bends. We started with some sample pieces (6" x 6") in various thicknesses from 16GA to 3/8" Hot Roll. In each thickness, we made several samples, (single bends, double bends, etc.) and took measurements of the bent shapes, including the resultant bend radius. I then took these measurements and used them in a mathematical equation that I've found on-line for accurately defining a K-Factor for a single bend, but when the same K-Factor is used on a piece with multiple bends, the total length of the flat pattern does not equal the 6" that we started with on our sample piece. Below is the equation that I used to find a K-Factor for single-bend pieces for each gage size and had great success with the flat pattern equalling 6.000". A and B are the overall outside lengths of each leg and Total Flat Length is the 6" flat sample piece.

Bend Deduction = A +B – Total Flat Length

Outside Setback = (Tan(Bend Angle/2)) * (Thickness + Bend Radius)

Bend Allowance = (2 * Outside Setback) – Bend Deduction

K-factor = (-Bend Radius + (Bend Allowance / (π * Bend Angle / 180))) / Thickness

Here is the eqaution with my numbers(in inches) plugged in for 16 GA:

Bend Deduction = 3.054 + 3.056 - 6 = .110

Outside Setback = (Tan(90/2)) x (.060 + .060) = .120 (where (Tan(90/2) = Tan 45 = 1)

Bend Allowance = (2 x .120) - .110 = .130

K-Factor = (-.060 + (.130 / (3.14 x 90 / 180))) / .060 = 0.38 (where 3.14 x 90 / 180 = 1.57)

I followed this formula for each GA thickness and, with the resultant K-Factor, had a flat pattern of 6.000" each time. But when I tried using the same K-Factor of 0.38 for a 16 GA piece with two bends, with an overall outside width of 3.595 and two legs with overall outside lengths of 1.320/1.321, the flat pattern length grows to 6.016". To get the flat pattern to equal 6.000", I had to use a K-Factor of 0.295. Why is there a difference when going from one bend to 2 bends when starting with the same size flat pattern sample piece? I have yet to start working with pieces that have 3 or more bends, because I have been stumped at 2......

Thank you in advance for any input,

Mike Knauss

Bernie Daraz Feb 2, 2012 1:12 PM

Correct Answer

Mike,

I've been bending a long time and tried to better myself by better understanding what happens to minor changes in the bend setup, allow me to share some of that with you. While there are some on this forum that only need/desire to produce models that may be close to actual production models, I (and apparently you) need to produce accurate models for our shops. This also eliminates errors in programming.

That said, while K-factors exist, they are simply an approximation. You also cannot use a K for 16 gauge and 3/8" thick stock and expect the same results. Not that they couldn't be obtained though. This would depend on the talents (read patience) of your press brake operators and available tooling.

Air bending is one of the bending styles available, coining is another. Air bending does not generate a bend radius equal to the tool radius, except maybe for a small part of a 90 degree bend. Coining does however. Each bend style has a different K factor as does each material given similar material thickness and die width ratios. 10 gauge stainless has a different K than 10 gauge CRS.

As you have found your operator came in with a different result, no matter the reason. I found I had less to no further occurances of that nature when I specified a bend deduction. A brake operators job is to achieve the specified bend deduction. When he cannot, the programmer/designer has made a mistake. Of course we can sometimes cheat and achieve the bend deduction, but all that does is make the job harder and most often a request (should I say demand) to fix it for the next time.

No doubt for many materials and bend radii your operator can tell you what to use as a bend deduction, I would ask. When there is no information, a simple test bend in scrap of the same material, gauge and grain direction will give you an accurate bend deduction. I always do at least three samples. Measure the flat blank or test sample before the bend, then make the bend. Now measure the two flanges and subtract the sum from your original blank size. That is your stretch or bend deduction.

Don't get me started on how SW handles jogs or offsets! LOL!

Bernie

See the reply in context

No one else had this question

Outcomes

21 Replies

Jeff Cox Feb 2, 2012 12:40 PM
Mark Correct
Correct Answer
how are you checking the actual resultant bend radius? If you are air bending there is not an accurate way to check the radius on the inside of the bend. I did something similar to what you're doing and found that I had to check the radius on the outside of the bend and then subtract the thickness. When the press brake guys comes to my cubicle and say "this stretch out is wrong", we can usually back track and find out that he used the wrong punch tooling and thus has the wrong radius.

I like your thinking on this and the equation is the same as I would use. Another thing to consider with each additional bend your doubling any error in your method for one bend. Just a thought.

Jeff
Like • Show 0 Likes0
Actions
- Mike Knauss @ Jeff Cox on Feb 2, 2012 12:57 PM
  Mark Correct
  Correct Answer
  Jeff,
  
  We are, in fact air-bending with a hydraulic brake press. At first I tried to measure the radius with a shadow graph comparator and could easily see the distortion, or in this case, not a true radius. So I used simple radius gauges and, through what I like to call "precision guess-work" I recorded a rough radius measurement. With my flat patterns equalling 6.000" every time on every GA thickness, I assumed my radius measuring was pretty close. I thought of measuring the outside, as you had stated, but with the theory that, as the metal stretches, it thins out. This would result in a less-than-accurate measurement as well....
  
  Mike
  Like • Show 0 Likes0
  Actions
  - Anna Wood @ Mike Knauss on Feb 2, 2012 1:37 PM
    Mark Correct
    Correct Answer
    Mike,
    
    Here is a good site with info on bending metal. Reiterates much of what Bernie is saying.
    
    http://www.ciri.org.nz/bendworks/
    
    Cheers,
    
    Anna
    Like • Show 1 Like1
    Actions
    - Bernie Daraz @ Anna Wood on Feb 2, 2012 1:55 PM
      Mark Correct
      Correct Answer
      Anna,
      
      Thanks! I have seen BendWorks and I have a copy for reference. I have seen degreed engineers use it incorrectly too. I have been using the test bend method since the early 1970's. My experience is actual and I'm lucky to say I still have all 10 fingers. I also have close to 30 stitches for various injuries on the shop floor though. I'm still lucky!
      
      Bernie
      Like • Show 0 Likes0
      Actions
      - Anna Wood @ Bernie Daraz on Feb 2, 2012 2:07 PM
        Mark Correct
        Correct Answer
        We use bend deductions derived from actual tests of the material and brake press tools we have. Testing is the only way to go for getting good bend deduction info.
        
        Cheers,
        
        Anna
        Like • Show 0 Likes0
        Actions
      - John Stoltzfus @ Bernie Daraz on Feb 2, 2012 2:10 PM
        Mark Correct
        Correct Answer
        Good afternoon Bernie,
        
        Thanks for all the good stuff, I just wish I could get our people to look at it the same way, Oh the only thing they do is subtract material thickness if the're lucky...........sigh
        
        A lot of times people think that it is easier to manufacture something if you open up all the tolerances, 1/4" bolt..eh 5/16" hole that'll be good enough, I know for a fact it is harder, tighten up your tolerances and the easier it is for assembly, where most of the poor tolerance time is wasted.
        
        Now let's talk battle scars, one finger, two fingers, three fingers.... hey I got all of mine too
        
        Later,
        
        John
        Like • Show 0 Likes0
        Actions
        Bernie Daraz @ John Stoltzfus on Feb 2, 2012 2:34 PM
        Mark Correct
        Correct Answer
        Hey John,
        
        You got that right! At one time it was 1.5 times the material thickness, so I understand where that came from. Then accuracy came into play. Mind you I do electronic chassis primarily, accuracy is important if you want all the PC cards and jacks properly aligned with their mounting features.
        
        Someday I'll find the drawing that I had to make one time for a customer, it was a retrofit. It had 13 bends in one axis. You think that could have been made without accurate bend deductions and knowing exactly what can be achieved on my shop floor?
        
        My favorite argument to those that think it's not that important, one day it will be. What's your experience amount to then? Try to tell an inspector from a customer that it's close enough after he's already rejected your job.
        
        The surfers have 'hang ten'. We don't have a good one do we?
        
        Bernie
        Like • Show 0 Likes0
        Actions
        Bernie Daraz @ John Stoltzfus on Feb 3, 2012 8:47 AM
        Mark Correct
        Correct Answer
        John,
        
        Good morning!
        
        I found that part, it was 12 bends not 13 as I remembered it. We got this job as their other vendor could not deliver on time, we originally lost job the job as our quote was higher. I had this job in the old programming system as I no longer have access to Pro-E. I exported the DXF flat and then added the sketched bends in SW. Man! Was that fun!
        
        This was a retrofit to an existing chassis and the top and bottom mounting holes had to match the existing rack mount chassis and cover. I started on Thursday and we delivered the 100 piece order on Monday, we got a rush premium on the job as well! My boss left me alone on this, leaving me with the comment: Now we'll see if you're worth what I pay you! I loved the challenge!
        
        This had to be done with known bend deductions. We had the original chart that was created at Westinghouse I believe in the early 60's. I had redone the chart to incorporate our new style of bending after we aquired the Amada brakes. It was .06 aluminum, no test bends. We ran all 100 plus 16 extras as that was what the blank yield allowed.
        
        I want some more challenges! But now I'm just doing the 3D end of it and trying to get the best and most usable models to my vendors.
        Bernie
        
        Like • Show 1 Like1
        Actions
        John Stoltzfus @ Bernie Daraz on Feb 3, 2012 10:11 AM
        Mark Correct
        Correct Answer
        Good morning Bernie,
        
        That had to be a good part to work on.
        
        The hardest part that I remember in sheet metal was a huge oven hood, I wish I still had the files. The issue for me was I did it in 2001 using 1998 Plus SW, so forget the features we use today, right..
        
        At that time I did part time design work for a company that made oven hoods for homes and restaurants, this one was for an expensive private home and all the trim above every door and window throughout the entire house had a 4" rise and a 4" protrusion and a 4" or so flat spot at each end and they wanted the same thing with the hood. The hood was 8'-00" long and at least 4'-00" wide and I had to create a flat pattern layout so they could get everything laser cut. Normally in a hood like that there are quite a few features, like holes, openings, grease filter trays and outlets etc, oh it was also out of 304 Brushed finish SS, so absolutely "No" mistakes.
        
        Again doing it now would be much easier, because of the SW sheet metal and modeling features. Sheet Metal Loft would have been awesome.
        
        Fortunately once I figured out the process it worked out ok; What I needed to do is use line segments instead of a smooth rolled surface, ended up being a real good job for the guys, so all went well,
        
        Later,
        
        John
        Like • Show 0 Likes0
        Actions
        Bernie Daraz @ John Stoltzfus on Feb 3, 2012 10:52 AM
        Mark Correct
        Correct Answer
        John,
        
        Good morning!
        
        Yeah, we used to do all those kinds of g-jobs at most of the jobs I had. The hoods and backsplashes were fun. Funny though that you mentioned a hood. My brother in law was a member of this yacht club and he asked me to make a hood, .090 stainless. So here I am after hours calculating the bend positions to input into the Amada brake, three times just to be sure. My boss walks by to say good night so I break right there.
        
        I recalc the numbers yet again after he leaves and bend the hood. It doesn't match the sides to be welded on! I recalc the numbers and realize that the glow from the overhead lights blanked a portion of one of the characters on my calculator, I was off a whole inch! I bent at 9" instead of 8"! I had to buy another 3x8 sheet of the material from my boss to remake the hood!
        
        Yeah, I lost on that cash one! TGIF and Go Giant's!
        Bernie
        Like • Show 0 Likes0
        Actions
Bernie Daraz Feb 2, 2012 1:12 PM
Unmark Correct
Correct Answer
Mike,

I've been bending a long time and tried to better myself by better understanding what happens to minor changes in the bend setup, allow me to share some of that with you. While there are some on this forum that only need/desire to produce models that may be close to actual production models, I (and apparently you) need to produce accurate models for our shops. This also eliminates errors in programming.

That said, while K-factors exist, they are simply an approximation. You also cannot use a K for 16 gauge and 3/8" thick stock and expect the same results. Not that they couldn't be obtained though. This would depend on the talents (read patience) of your press brake operators and available tooling.

Air bending is one of the bending styles available, coining is another. Air bending does not generate a bend radius equal to the tool radius, except maybe for a small part of a 90 degree bend. Coining does however. Each bend style has a different K factor as does each material given similar material thickness and die width ratios. 10 gauge stainless has a different K than 10 gauge CRS.

As you have found your operator came in with a different result, no matter the reason. I found I had less to no further occurances of that nature when I specified a bend deduction. A brake operators job is to achieve the specified bend deduction. When he cannot, the programmer/designer has made a mistake. Of course we can sometimes cheat and achieve the bend deduction, but all that does is make the job harder and most often a request (should I say demand) to fix it for the next time.

No doubt for many materials and bend radii your operator can tell you what to use as a bend deduction, I would ask. When there is no information, a simple test bend in scrap of the same material, gauge and grain direction will give you an accurate bend deduction. I always do at least three samples. Measure the flat blank or test sample before the bend, then make the bend. Now measure the two flanges and subtract the sum from your original blank size. That is your stretch or bend deduction.

Don't get me started on how SW handles jogs or offsets! LOL!

Bernie
Like • Show 0 Likes0
Actions
Bernie Daraz Feb 2, 2012 1:35 PM
Mark Correct
Correct Answer
Mike,

Perhaps you may find the attached Excel sheet useful. This sheet details accurate (for us) bend deductions for a variety of material gauges and radius. These are calculated using an approximate .424 K factor, you can change that if you note the RED number below the sheet itself. This factor was used for reference only.

It would be easy to add radii and material thicknesses to the sheet if you understand the way Excel works. This sheet has been very accurate over the years with only minor modifications to the K as required by the bending styles at the shops I have worked at. Material thicknesses run across row 5, bend radius along column A.

This sheet may not be accurate for your use as the bending styles may differ, so therefore, USE AT YOUR OWN RISK. So test, verify, test and verify.

Bernie
Attachments
- BEND1.XLS29.0 KB
Like • Show 0 Likes0
Actions
- Mike Knauss @ Bernie Daraz on Feb 2, 2012 2:49 PM
  Mark Correct
  Correct Answer
  Bernie,
  
  It sounds like my testing that I have been doing follows along with your post above (Feb. 12, 2012 11:12 AM). Through our testing we have come up with a K-Factor for each GA thickness using the above stated formula.
  
  16 GA: 0.38                              1/8": 0.399
  14 GA: 0.435                             3/16": 0.362
  12 GA: 0.456                             1/4": 0.371
  10 GA: 0.427                             5/16": 0.389
  07 GA: 0.38
  
  These K's have proven to be accurate with single bend pieces using our determined bend radii and flange lengths, but does not follow through when more than one been is introduced to the part. I will look over your Excel sheet and see if this information can be of use to our manufacturing/engineering processes.
  
  Thanks to all the others, as well, for your input on this topic.
  
  Mike
  Like • Show 0 Likes0
  Actions
  - Bernie Daraz @ Mike Knauss on Feb 2, 2012 3:43 PM
    Mark Correct
    Correct Answer
    Mike,
    
    Sounds and looks good! What does your press brake guy refer to, a bend deduction or a K factor? That's where I would be looking. The interesting thing is that tke K factor as you show it for 16 guage is good for you, I believe we're referring to an air bend too.
    
    We more than ever coined to get bend angle consistancy in our 500 piece and more runs. A lot of it was 20 gauge galvaneal. I did run into an issue once though more recently. Our bend deduction for 16 gauge CRS was .086 for a normal bend and a part less than 24" of bend length. Our programmer dutifully used a normal bend deduction (.086) on this 81" long bend.
    
    Even with a 110 ton press brake we wouldn't have been able to achieve that bend deduction. It came out closer to .103. Noting that you air bend you would have been closer anyway. Good that there was enough tolerance on the print to have the part come out close.
    
    Even a standard practice has variables.
    
    Bernie
    Like • Show 0 Likes0
    Actions
    - Mike Knauss @ Bernie Daraz on Feb 2, 2012 4:05 PM
      Mark Correct
      Correct Answer
      Thanks for your replies, Bernie. I will utilize this information to further my knowledge of this. We mostly refer to the K-Factor, but some of the old-school fabricators will shy away from it. They like to just take the overall bend dimensions and subtract material thickness where necessary to get a flat pattern size. Although this is generally close, it doesn't magically fill in the K-Factor in our Solidworks software.....
      
      Thanks, again,
      
      Mike
      Like • Show 0 Likes0
      Actions
- Bernie Daraz @ Bernie Daraz on Feb 4, 2012 9:16 AM
  Mark Correct
  Correct Answer
  Hello all!
  
  I was contacted by an alert viewer of this post who didn't want to be named, I'll respect that and Thank You! The spreadsheet I posted above was actually supposed to be called "Bend Deductions for 90 Degree Bends". To me, an allowance is something you add and a deduction is something you subtract. I have corrected that sheet and it is attached. ( "_Bend Deductions" ) Also please note that the K factor as used is added to 1. It just made the calculation formulas easier to use when I did that sheet back many years in Lotus 123.
  
  I have also attached another spreadsheet that allows you to calculate your angular bend deductions and allowances. Over the years I have seen prints dimensioned in a variety of ways. Some dimension the angular bends to the centerline of the radius specified and some to the outside and or inside tangent or apex. This spreadsheet gives you both of those numbers to aid in your layouts and calculations. ( "_K Bends Calc" ) If you know your K factors this one is easy to use, if not just use .42 for air bends or .33 for coin bends to get started. If you vary that number slightly you'll see that there isn't much difference in the result.
  
  You'll note that this sheet also presents additional results when possible. There have been many times when an angle bend was shown on a print, the complimentary angle was also needed. This was most common when an angular joggle or offset of more than 8 times the material thickness was specified. That was a suggestion by Roger Hill and his name was added to show his contribution.
  
  The allowance figures presented are added to the calculations when used with inside tangent or dimensions to the centerline. The deductions are used with outside or outside apex (outside set back) dimensions and are then subtracted.
  
  Of course with posts and spreadsheets like this you must verify the accuracy with your own use and TEST, TEST, TEST. Neither of these spreadhseets should be used for joggles or offsets bends or hems.
  
  Let me know how they work for you!
  
  Bernie
  Attachments
  - _K Bends Calc.xls25.5 KB
  - _Bend Deductions.XLS29.5 KB
  Like • Show 1 Like1
  Actions
  - Lyndon Crossman @ Bernie Daraz on Apr 24, 2012 2:43 PM
    Mark Correct
    Correct Answer
    I am currently trying to improve the accuracy of our flat patterns. We do air bending.
    We also have a program called AutoPOL which produces extremely accurate flat patterns based on bend samples.
    We generate our flat drawings and dxf's in Solidworks so need to make them match AutoPol.
    
    The problem I am trying to solve is have solidworks set the radius and k-factor for each bend. Currently Solidwork's bendtables don't correctly model the air bending process.
    
    The bend radius and k-factor varies by bend angle. Currently bend tables allow different k-factors by bend angle but keep the radius the same.
    
    As for calculating inner radius of sample pieces.
    Here is an accurate method:
    I don't know the formula but if your good at trig you should be able to figure it out.
    Some Data I have generated
    
    I am thinking about writing an add in where the user selects die opening and then add in sets each bends radius and k-factor automatically unless someone has already done that!
    Like • Show 1 Like1
    Actions
    - Bernie Daraz @ Lyndon Crossman on Apr 24, 2012 3:11 PM
      Mark Correct
      Correct Answer
      Lyndon,
      
      To me bend allowances and bend deductions are two ways to express the same things. They are obviously very different in application.
      
      You've found the point where it doesn't match the obvious. Or should I call it, what you expect it to do. Understanding those variables is key to coming up with the closest and most accurate flat for your guys (or girls!). The other part of the process is being close enough so that your guys can get it in tolerance.
      
      Don't take me to task for the 'close enough' comment. I have been doing this stuff for 40 years and know how to get things right. Put it on the floor with a lack of understanding on your part or the brake guys is a recipe for disaster.
      
      I've said it before and I'll say it again, you'll never learn everything about precision sheet metal until you learn how to bend.
      
      Of course you have to know how to measure all those dimensions (accurately) to verify them too. My last place the CAD guys drew in sharp (no radius) bends for all bends, even those over 90 degrees. The bend allowance would never be right. You could still get the jobs done, but they were only close and they took longer.
      
      The closer you are with the actual bend allowances makes the job easier to bend. DUH!
      
      Getting back to what you've posted, I'm guessing that you have limited actual bending experience. Please take no insult here, I do not mean to insult you! I've worked at a few shops and at each one I've had to adapt my bending style to achieve their bend allowances. It made me better no matter that hassle.
      
      Your first picture is the real indicator of the issue, what is the actual resulting radius regardless of the tool. In all reality, for a short bend (2 to 3 inches) in light guage you'll likely achieve an allowance that is at the smaller end of the scale. Working a much longer bend will cause the opposite. Yes, I've programmed jobs with different bend deductions for different length bends on the same part.
      
      Just because the bend deduction for 16 gauge steel is .092 does not mean you'll achieve that for a 10 foot long bend. Then of course you may have to deal with the occasional, "I had that setup in the brake so I used it, I didn't know it would do that".
      
      I would guess your guys have their own charts and suggestions. When we first started CNC punching and variables were allowed in the programs I asked the guys on the floor. All your charts are nice and more than likely very accurate. Just change the material from aluminum to stainless, CRS or copper. All sorts of small variations will come into play.
      
      The hardest part here is to show the guy on the floor with 10 years or more experience that your chart says this is what he should get. I always send prints with the bend allowances I designed (and expect) the parts with. If they know that and they MUST change a setup you're ahead of the game.
      
      Be ready to accomodate yourself to some realities.
      Like • Show 0 Likes0
      Actions
      - Lyndon Crossman @ Bernie Daraz on Apr 24, 2012 4:11 PM
        Mark Correct
        Correct Answer
        Bernie,
        Thanks for the comments.
        
        As you stated the closer one is to the actual bend allowances the job is easier to bend.
        
        We design, fabricate and assemble. Overtime I have become familiar with the process from Solidworks through to assembly.
        
        My current goal is to reduce the rework time due to modeling errors.
        
        I know that flat pattern accuracies less than 0.010" can be achieved because I have seen it using Autopol. We use it to program our brakes offline.
        http://www.autopol.com/products/bendsimulator/introduction/introduction.asp?sidebar=intro_bs
        
        Unfortunately the algorithm used by autopol is proprietary.
        We have considered just setting Bend radi to material thickness and not using solidworks to generate flat patterns but then we would need to generate flat drawings outside of solidworks which kind of goes against the solidworks benefits of relational modelling.
        
        I want to try and achieve flat pattern accuracies from Solidworks of +/-0.010 inches.
        The question is what is best way to achieve this?
        
        I am aware of following bend allowance calculation methods for solidworks.
        We currently use following format. Which works well for parts with only 90deg bends.
        For thick materials (>12GA) with bend angles <>90 flat pattern error increases the further you get from 90.
        Like • Show 0 Likes0
        Actions
        Bernie Daraz @ Lyndon Crossman on Apr 24, 2012 4:31 PM
        Mark Correct
        Correct Answer
        Lyndon,
        
        I have heard of this practice but never was involved in its implementation. I'm stuck for time so my response will be shorter this time. It's possible that my response will reflect the lack of knowledge of its implementation too.
        
        I find it odd that the AutoPOL software will accept models and then apply its own bend calculations, isn't it too late in the process? SolidWorks bend tables are at best averages, they may or may not work for you. I have modified my own tables using my own bend deductions.
        
        I am aware that Amada brakes use their own method or calculations to set up brakes, the allowances can be determined from the displays of the backgage position and the flange length entered with some easy math.
        
        Sorry I don't have more time to devote to this right now. Perhaps tomorrow.
        Like • Show 0 Likes0
        Actions
        Lyndon Crossman @ Bernie Daraz on Apr 24, 2012 4:58 PM
        Mark Correct
        Correct Answer
        The AutoPol software can export a dxf file. This flat pattern dxf is then as accurate as you have calibrated the autopol flattening algorithm.
        The algorithm is calibrated by bending two samples using two different die widths. You then take a bunch of measurements plug in the numbers and now AutoPol knows your particular material's bending properties.
        
        Basically the accuracy is determined by accuracy of you measuring the bend samples.
        
        I think you have summed up Solidworks bend tables well with "are at best averages" comment.
        
        In the ideal world the sheet metal designer would simply set the material and the bending process governing parameter. For air bending that would be Die Width.
        
        I was hoping someone may have already created an add in that improves upon solidworks bend tables.
        
        regards,
        Lyndon
        Like • Show 0 Likes0
        Actions

Incoming Links

Re: Bend Allowance Table

K-Factor for multiple bends

Outcomes

Attachments

Attachments

Related Content

Recommended Content

Incoming Links