5 Replies Latest reply on Apr 6, 2018 2:38 PM by Dennis Dohogne

    Sheet metal gauge / bend table for air bending

    Matt Zglobicki
    Matt Zglobicki Apr 5, 2018 3:52 PM

      We have a new press brake in our shop and I am trying to get SolidWorks sheet metal flat patterns to match the blank size from the brake controller (it has been very accurate). We are air bending and using consistent tooling per material thickness.

      I am trying to use a gauge table with bend allowance to create the proper flat pattern based on angle. I made a simple part with 1 bend and ran it through the brake software to get its blank size for various bend angles. I then back figured what the bend allowance should be in SolidWorks for the corresponding angle to give me the correct flat pattern dimension for this bend.  I know the radius changes with air bending based on the tooling used and angle bent, but as I mentioned we are using consistent tooling and I was hoping to make up for the radius with the bend allowance. For us having the correct flat pattern dimension is more important than radius on the part.

      The problem I am having is the table is not working the way I thought it would. I started with a sample table from SW and have filled in some bend allowances for each thickness per angle. The table gives correct flat pattern for the 90 degree bend and nothing else. Any other angle does not seem to be pulling the bend allowance from the table. With the part set at anything but 90, if I change the bend allowance for the corresponding angle in the table it does not change the flat pattern dimension. If I change the bend allowance for the 90 degree angle it changes the flat pattern for all angles. It is as if SolidWorks is using the bend allowance for 90 degrees and then maybe K factor form there. 

      I must be missing something, am I using the table wrong?  Has anyone else found a good way to have their SolidWorks flat patterns match what comes out of a brake controllers software, is there another way to do this?

       

      I have attached my table, any help would be much appreciated

       

      Matt

      • 441 Views
      • Tags:
        • Re: Sheet metal gauge / bend table for air bending
          Dennis Dohogne
          Dennis Dohogne Apr 5, 2018 4:16 PM (in response to Matt Zglobicki)

          Matt,

          I don't have access to a press brake any longer, but I developed the attached files at one company where we did A LOT of sheet metal.  We measured the actual material thicknesses (NEVER trust the published values or use the nominal gauge thickness - probably the single biggest mistake folks make) and measured the flats before bending and the coupon parts after bending.  Putting those measurements into the attached spreadsheet we calculated our K-factors.  For any new designs in SWX we just looked up the material gauge and inside bend radius and used the appropriate K-factor to generate the flat patterns.  We got amazing accuracy with this technique.  We were able to pre-punch holes on multi-bend parts and they lined up perfectly in assembly.  No more mate-drilling!!

           

          I have to admit that most of our bends were 90 degrees, but I would venture that if you make similar measurements you will get great results, even for other angles.

            • Re: Sheet metal gauge / bend table for air bending
              Matt Zglobicki
              Matt Zglobicki Apr 5, 2018 5:00 PM (in response to Dennis Dohogne)

              Thank you Dennis,

               

              Not sure if i am missing it somewhere, late in the day for me, but the formula seems to only work for 90 degree bends. We bend a lot of custom stuff between 40 and 150 and I think that would throw this formula off due to the different arc length at different angles based on radius. It seems like this is how this formula is working to come up with the K factor. Also our radius varies with every angle due to air bending and unfortunately I do not have a good way of accurately measuring the radius. Fortunately most of our stuff does not have any holes that need to line up! Thanks for the input, I will take another look at it in the morning.

                • Re: Sheet metal gauge / bend table for air bending
                  Dennis Dohogne
                  Dennis Dohogne Apr 6, 2018 8:08 AM (in response to Matt Zglobicki)

                  The K-factor is not a function of the bend angle at all.  The spreadsheet is setup to use measurements for parts bent at right angles because a) that is most common, and b) it is much easier to measure.  But if you do a good job of measuring and generating the K-factors using theis method I suggest you do a couple of things to build your confidence:

                  1. Design some simple right angle bent parts in SWX using the actual material thickness that you measure and the K-factors for the combination of thickness and IBR (Inside Bend Radius).  Cut the flat pattern to the dimension determined by SWX and bend it accordingly and see how well the finished part matches the designed part.  (They should be dead-on.)

                  2. Do the same thing for 40 and 150 degree bends - design them in SWX using the thickness and K-factor, cut the flats and bend them.  Measure them to compare to the designed part.

                   

                  Only then will you have confidence in the results.

                   

                  If you determine that these K-factors do not give you good enough results for your 40 and 150 degree bends then I can help you develop measurements and calculations for K-factors specific to these angles.  But first, do the work of measuring and filling out the spreadsheet and the two verification steps mentioned above.  You might have just done all you need to do to get the results you are after.

                    • Re: Sheet metal gauge / bend table for air bending
                      Matt Zglobicki
                      Matt Zglobicki Apr 6, 2018 2:08 PM (in response to Dennis Dohogne)

                      I tried this using the brake controller software to get the numbers for me as we have tested in the past and what it comes up with is good and ultimately I am really trying to mimic what it puts out. At 90 degrees with formula I got a K factor of .52 plugged into SolidWorks and blank size came out correct. After that things fell apart. At 55 degrees with the formula the K came out to 1.4 (can not be more than one). To get the flat pattern correct in SW it needs to be .88.

                      I guess part of my problem is I am not trying to increase accuracy, I am just trying to mimic the controller and give the designers an easy way to model and produce the same flat pattern as the controller (I can't believe i just typed that!). In all reality it would make out process much smoother if I can have a table that SW references, Bend allowance, Bend deduction or K factor that will allow SolidWorks to output the same Flat pattern as the controller comes up with for Blank size. Current practice is for the brake to create a program to produce the blank size, to give back to the sheer to get cut, to give back to the brake to be bent. I am looking to get rid of the back and forth. I figured I could do this with one of the tables, but they do not seem to be working. Dennis I appreciate your input, I just don't think it is going to work for what I need to achieve.

                       

                      I really would like to know why the tables in SolidWorks act the way they do, is there a bug, or am I doing something wrong. If the Bend allowance table worked the way I thought it would, I know I can make this work. It is just a matter of how many angles I need to put in. For any given angle it would pull a value to insert as the bend allowance, but for some reason it only appears to be using the bend allowance from the 90 degree angle and doing another calculation from there.

                       

                      again thank you for your responses.

                        • Re: Sheet metal gauge / bend table for air bending
                          Dennis Dohogne
                          Dennis Dohogne Apr 6, 2018 2:38 PM (in response to Matt Zglobicki)

                          Matt,

                          It sounds like you are trying to do some black-box reverse engineering.  I get that, but there are times when a different approach is warranted and I think this is one of them.  You are absolutely correct to say the K-factor must be less than one.  The fact that you got something greater than makes me want to see the data and calculations that got you there.

                           

                          If you were to make some measurements as laid out in my method and then do the two steps, regardless of what your controller is telling you, you will be able to answer the question of how well the K-factor works.  Period.  THEN we can compare to what your controller is telling you.

                           

                          For instance, let's say you are bending material that is .053" thick (the measured value of a 16 GA specimen for example, not .0598") and you are using tooling with a nose radius of 1/16".  Let's say that after making the measurements of the flat length before bending and the flange lengths after bending and plugging all that into the spreadsheet you get a K-factor of .42.  Now make three dsigns in SWX of 40*, 90*, and 150* bends using this thickness, IBR, and K-factor.  See what the flat pattern is in SWX and then go make the parts.  Note what the controller is telling you, but bend the parts to the angles and flange lengths of those SWX sample designs.  In all likelihood the flat patterns will be correct or wonderfully close.  The thing that I suspect that might be off is the setbacks, making one flange longer than it should be by the same amount the other one is short (for a single-bend verification part).

                           

                          The very first time I got into sheet metal I was calculating the flat pattern with my HP-41CV hand calculator with equations I'd gotten from Amada.  I solved a HUGE problem they had been living with for five years.  However, one of the biggest obstacles I had was in dealing with the press brake operator because he wanted to use his own numbers for adjusting the setback.  I had to insist that he use my numbers and had to stand there as he entered those values.  We had a part with two 45* air bends such that the two ends were parallel and offset from each other.  There were notches in each of these ends that formed pivot points.  The spec called for the distance between these to be 8.000".  The three pieces we made measured out to 8.002", 8.002", and 8.003".

                           

                          I suspect your controller is doing a decent job of estimating a flat pattern length, but not the setbacks, but without looking at your data it is only speculation.

                           

                          Trust me, I am only going to this much trouble because I have seen this method work time and time again.  If a person does their homework they have a set of numbers that will serve them very well.

                           

                          Make the measurements and the verification parts.  Tell us what information the controller is telling you for these parts and perhaps we can get you the correlation you are after.