7 Replies Latest reply on Jan 7, 2016 4:59 PM by Boyko Tchavdarov

    Propeller efficiency, best way to get fan performance curve?

    Robert Hohmann

      Can someone evaluate my project? I calculated volume flow at both ends of the pipe so i can do parapetric study with pressure drop. At calculated volume flow i should get pressure drop close to 0 but after 55 travels i still get 11268 Pa. Normaly i would do 20 parametric points with volume flow from 0,01 m^3/s to calculated volume flow from first study. Is this a way to calculate propeller efficiency? I want to use it later as a fan in a tank, so i can evaluate different angles of a blade and choose best mixing option.

        • Re: Propeller efficiency, best way to get fan performance curve?
          Amit Katz

          Your project seems to be incomplete. There are missing files which make it impossible to solve. Did you use "Pack and Go"?


          From what I did get though, I can see your project setup. One reason for your higher than expected pressure drop probably has to do with the walls of the test section. You specified a rotor condition, but they still have friction (even with zero roughness) and will have an effect on the pressure required to move the fluid.

          • Re: Propeller efficiency, best way to get fan performance curve?
            Boyko Tchavdarov

            I could be of good help but I am with SW2014 and cannot open your model.
            I hope you can get a complete answer  but if not or the job is urgent for you please provide snapshots with model details.

              • Re: Propeller efficiency, best way to get fan performance curve?
                Robert Hohmann

                Hi Boyko,

                here are some screenshots, if you need more options to see let me know. I added 3 screenshots from other propeller with bad results as well. Is there a way to save my project with backwards capability?

                  • Re: Propeller efficiency, best way to get fan performance curve?
                    Boyko Tchavdarov

                    Here are my recommendations from what have seen in the snapshots:

                    1) You have mentioned a fan but the fluid is water (?) - The expected " zero" pressure drop with water will be less "zero" than if it is air. Furthermore, the run-out (zero pressure drop) and the shut-off (zero flow rate) operating point are not possible to predict with the mixing-plane (averaging) local rotating region, You need to use sliding mesh for better accuracy at operating point away from the Best Efficiency Point (BEP).


                    2) For convergence  criteria use the following Goals  the following in priority order by highest accuracy:
                        - forces on the rotor
                        - pressure drop

                       - efficiency (you need an Equation that links flow-rate, pressure-drop (head), rotational-speed and Z-torque component to calculate Efficiency - check the Engineering Tool Box for the correct formula in mixed units if you use such)

                       - while you can track the mass imbalance in % (inflow - outflow)/inflow, the goal converged first and we need to run at least 2-5 more travels to converge the last two goals above (more travels for the first goal)


                    3) Mesh resolution is important. It looks like you have chosen a good one but if you sand me snapshots of the mesh, I can tell you more precisely.

                      • Re: Propeller efficiency, best way to get fan performance curve?
                        Robert Hohmann

                        1) Fluid is water because propeller (fan) will operate in tank filled with water (or milk). I thought that sliding mesh is usually used in non symetrical flow? My first calculation is set up to know what volume flow is at the inlet (propeller pushing water towards outlet). Next i'm doing parametric study with starting point like 0,01 m^3/s and ending point which i got from previous calculation, and calculating how pressure drop change to the point of supposedly even volume flow (because in parametric study on inlet i'm using volume from calculated first study so inlet flow and propeller pushing water should be equal, so pressure drop should be 0?). I should get propeller (fan) curve which i would like to use in a tank filled with water as a boundry condition. Should i use air instead to get propeller performance curve?

                        2) I think i could misguide a little with topic. I want to get propeller curve from volume flow and pressure drop (look at images that i attached)

                        Let Your Fans Do the Work in Flow Simulation - A Night School Preview



                        3) I attached pics with meshing, should i use new option that solidworks 2016 provides? (Equidistant Refinemnt) And if so, can you guide me with some proper settings?

                          • Re: Propeller efficiency, best way to get fan performance curve?
                            Boyko Tchavdarov

                            "Fans" term is used when the propeller (rotor) works in open air space while "blowers" (create air flow at low pressure ) and "compressors" (create much higher pressure) - work  in a duct (volute). This difference makes the best design different. When rotor works in a liquid fluid it is a "pump" (creates pressure/head ), "turbine" (creates torque), or " mixer" when the rotor works in a tank. All the above different turbo machinery has very different performance curves and using a fan curve to guide you in mixer analysis wont help at all.  Is your application a "mixer" or a "pump"?


                            Regarding the mesh. Flow Simulation has better convergence rate and ends in better accuracy if more uniform mesh is used. If you are with SW2016 then

                            apply the "Uniform mesh" (it is a new option, I guess)  that create a uniform mesh around the rotor. This new option is designed to assure equidistant  uniform mesh around a body with minimum effort. If you are not with SW2016 then you can create a volume around the rotor and  use it for Local Mesh Refinement in the CFD model unchecking the body in the Component Control list to disable it (the body will be invisible for the flow and will serve only for the mesh and eventually for post-processing, automatic solution based mesh refinement,  or transfer data for initial data of another model). Also, keep in mind that you need minimum 3-fluid cells on both side of the local Rotating region (needed when the stator geometry is not a cylinder everywhere) for better accuracy. I have mentioned sliding mesh for operating points away from the BEP, assuming that your stator is not a cylinder and has a few stationary vanes (blockages) as the rotor does. The stronger is the rotor-stator interaction the larger is the difference in the convergence and in the value of the results between the steady-sate averaging (mixing-plane) model and the unsteady sliding mesh.


                            If you have one-mean direction of the flow (as in your pipe) then assure longer distance downstream for the axial rotor and much shorter upstream (in other words move the rotor upstream in your benchmark model)


                            Another thing to remember is tat for incompressible fluid (liquids)  Flow Simulation works better with (velocity@inlet) and (environment_pressure@outlet)  b.cs. rather than with any other combination of those, however depending on your objectives and analyst you may need to have a known pressure at inlet ( for example if you turn on the cavitation for internal flow model). In that case use pressure / environment_pressure as inlet /outlet conditions  is preferable.


                            Hope the above helps to set up your analysis. Let me know if you have further questions,