8 Replies Latest reply on Jun 15, 2017 9:20 AM by Bill McEachern

    CFD not matching real world testing on a flow bench

    Jeff Soucek

      Hi All,

          Been learning and experimenting with CFD flow mostly as a hobby and a learning experience.  I have access to some nice equipment to validate the results.  Unfortunately the results in Flow simulation are not matching.  I cant seem to figure out why as it is a simple experiment.

       

      Let me explain my results and set-up.

       

      I have and actual 3d file of a velocity stack that was turned and CNC machined.  It was then put on a flow bench and the results came back as 312CFM at 10" depression

       

      18986698_1529552517068612_673037754_o.jpg

       

      19022774_1529598743730656_740191160_o.jpg

       

      You can see the results above on the flowcom screen

       

      I set up a model in Solidworks to represent this test to compare the results

       

      Below you can see my model.  The "balloon" is cross sectioned to see the velocity stack mounted to the square plate with a 4" pipe below it just like the actual test.  Even though the actual 4" pipe is only a 6" long I modeled it at 12" to get as much detail as possible

       

      18949041_10211269845835033_1502526126_o.png

       

      I set up my simulation with the Inside surface of the "balloon" to be environmental pressure opening of 14.6959473 lbf/in^2

       

      Screenshot 2017-06-07 22.46.42.png

       

      I then set the outlet surface "lid" ( bottom of the 4" pipe) to 14.334676481726 which converts to 10" wc

       

      In my model I set the initial mesh to automatic level 3 with advance narrow channel realignment

      I then applied a local mesh to the velocity stack and plate surfaces with custom settings of the following

       

      Screenshot 2017-06-07 22.56.38.jpg

       

      Screenshot 2017-06-07 22.55.54.jpg

       

      Screenshot 2017-06-07 22.55.08.jpg

       

      I then applied a second local initial mesh over the velocity stack and gave it automatic setting level 6 and picked the solidbody and chose disable solid component.  this can be seen in the picture above as a mushroom looking body

       

      One more note, I set my calculation control options to the following:

       

      Screenshot 2017-06-07 22.58.52.png

       

       

       

      Below you can see my mesh and the results

       

      Screenshot 2017-06-07 23.02.17.png

       

      Only problem is my results are considerably higher at 346.9 cfm vs 312 on the flow bench -  see below:

       

      18947276_10211269449065114_764525433_o.jpg

      This is more than 10% off.

       

      So does anyone see what I am doing wrong? Or do I simply have to tweak to get it to match?  If I have to tweak it to match, what is the best approach?

      My goal is to validate using this simple set-up then move to my cylinder head porting so that I know the changes I am making are valid

       

      This is a picture of the head I want to test, print a FDM rapid proto then flow test to compare again.  Eventually I will 5axis port machine the head for my personal track bike

       

      18986328_10211265576848311_666970146_o.jpg

      Sorry about so many pics but I felt it helps explain where I am at.

       

      Any input would be appreciated as I am now stuck and do not know what to do next.

       

      Thanks for any help you can provide

        • Re: CFD not matching real world testing on a flow bench
          Siavash Khajehhasani

          Hi Jeff,

          Gear work.

          Couple of concerns here:

          1) Do you have sufficient mesh close to wall boundaries.

          2) Are you sure if your solution is grid independent?

          3) Do you have further insight into the boundary conditions (eg. inlet turbulent flow: turbulent intensity, k, e, etc - which I guess not)

          4) assuming flow is turbulent, is is fully developed at the inlet (in experimental setup and numerical)

          5) It always worth to ask: is there any possibility that the experimental data are not 100% correct? In fact there is always some errors involved in experimental tests (mostly minor).

            • Re: CFD not matching real world testing on a flow bench
              Jeff Soucek

              Hi Siavash,

                  Thank you for the reply, please let me comment on your questions below, Please click on the pictures for an enlarged view

               

              1) Do you have sufficient mesh close to wall boundaries. - I have set up 2 local mesh and turned up the curvature.  I have also changed the global settings in the calculation control to #2  I am running close to 9g ram so my cell count is pretty high, here is a close up of the mesh, you can see my initial mesh settings in the first post

               

              Screenshot 2017-06-08 07.18.08.png

               

              2) Are you sure if your solution is grid independent? I dont understand what this means can you explain more? Are you saying that the mesh is small enough as not to affect the results?

               

              3) Do you have further insight into the boundary conditions (eg. inlet turbulent flow: turbulent intensity, k, e, etc - which I guess not) I simply left these to the default settings as I do not have this with the experimental data

               

              4) assuming flow is turbulent, is is fully developed at the inlet (in experimental setup and numerical) for the experimental data The flow bench runs for a 3 minute run and averages the results.  For the numerical data it converges at 777 iterations, about 6 hours run time on 4 cores, my settings below:

               

              Screenshot 2017-06-08 07.20.13.pngScreenshot 2017-06-08 07.20.22(2).png

               

               

              5) It always worth to ask: is there any possibility that the experimental data are not 100% correct? In fact there is always some errors involved in experimental tests (mostly minor).  It is hard to say, the flow bench used is the newest technology and it is calibrated with a plate with specific hole sizes and standards.  The data from this bench is consistent with another flow bench I also tested on

               

              100_7060_zpss4jxyxzp.jpg

               

              Once again thank you for any input

                • Re: CFD not matching real world testing on a flow bench
                  Siavash Khajehhasani

                  Hello Jeff,

                  As shown in the 3rd photo, I think you are using adaptive mesh which is great. Two consideration here: you can switch to periodic method (for details please refer to SW Flow Sim technical reference document), also I do not see sufficient refinement in high gradient regions (you can increase the refinement level). One more note here, I suggest to reduce that value of 8,650,000 to something reasonable as you do not want to end up with such huge amount of cells.

                  About the grid independence: you you correct; you should run your simulation couple of times with various mesh refinement level, until to a point you can conclude that more refinement does not have a major effect on the results and deviation between two last mesh resolution become minor.

                  About the turbulence parameters: what I found from your reply was that you are just using the default settings; for sure there is no experimental data available for your case. However, I'd suggest to use more reasonable values other that the defaults from the software. The simplest one is the turbulent length scale (can be set in initial settings) which can be defined according to hydraulic diameter of the dominant entrance flow.

                  - Siavash

              • Re: CFD not matching real world testing on a flow bench
                Bill Dempsey

                Hey Jeff

                I too play around with SF benches.  Have a SF600 myself.  I am not fully up to speed on Flow yet but what you are doing is one of the primary reasons why I bought Flow.  All that said, did you cal the bench with those plates at 10" or at 28"?  And did you cal with your stack adapter that I see bolted on?  My bench has cal plates that are to be cal'd with SF's adapter.  I cal at 25" and then recheck at 28".   

                Just trying to make sure you're eliminating a bad cal on the bench.  Some day I hope to be proficient enough on the tool to give you a better answer!!

                Bill

                • Re: CFD not matching real world testing on a flow bench
                  Amit Katz

                  Hi Jeff

                   

                  I don't have any experience with test benches, but looking at your setup it seems as if you are using pressure taps to estimate flow rates. I would take the actual pressure data from your experiment (not the calculated flow rate) and model those exact same taps in your CFD model, at the same locations and orientation. Compare those measurements first and see how they stack up, it may help you pinpoint where the difference between reality and your model lies.

                   

                  And by the way, 10% difference is not bad at all for a first pass.

                  • Re: CFD not matching real world testing on a flow bench
                    Mark Keown

                    Nice work.  I will put my 2 cents in.

                    I think you should: