11 Replies Latest reply on Feb 17, 2017 9:39 AM by Amit Katz

    Pump flow simulation

    Safet Seta

      Hello,

       

      I'm a mechanical engineering student and currently I'm working on my final project.

      For it I need to simulate the impact of different fluids on the pump, needed power

      for a given flow rate and RPM. I'm all new to this simulation thing, all the experiance

      I have is from the YouTube tutorials. So far I know how to set the boundary conditions,

      rotating regions. The problem starts here: When I put the BC's as enviromental pressure

      at inlet and outlet followed by a rotating region at 3000RPM I get a ''vortex crosses the..''

      warning message that I can't get rid of. I tried to extend the inlet and outlet pipe but to

      no avail and even refined the mesh. When inspecting the surface parameters of inlet and outlet

      lid for mass flow rate I get a different reading but in the report mass flow rate is listed as their subtraction

      (i.e. m.flow and inlet lid: 3.9205kg/s, outlet lid: -4.2329 kg/s(is the ''-'' a sight it's going out of the system?)

      and mass flow rate in report: 0.3123 kg/s) I'd wish to know how to avoid that message

      and how to correctly set up my boundary conditions.

       

      For my project the more important thing...

      When I set up an inlet mass/volume flow rate followed by an atmospheric pressure at the outlet

      I again get a different reading of the inlet/outlet surface mass flow rate reading, but this

      time without the warning during the calculation. I would like to know the best way to set the

      parameters for my pump, I want to know how to set the volume flow rate that the pump provides

      and not the flow rate of the fluid at the inlet pipe(or it's the same thing) and how does the

      option relative to rotating frame and absolute impact the results.

       

      The parameters I want to use for my analysis are:

      Pump flow rate: 100 m^3/h

      Angular velocity: 2500RPM

      Goals:

      1.Inspect the distribution of velocities/pressure/torque

      2. Calculate the needed pump power using the torque from each fluid simulated and angular velocity

       

      The main  question: How to set up the pump to surely get the correct results? (constant mass flow rate, suction pressure...)

       

      I'd be very thankful if any of you could provide me with the help needed to solve these problems so I can finish my project.

       

      The characteristic dimensions of the pump will be provided in the pdf below:

       

      http://i.imgur.com/X5qpHNh.png

       

      Thanks to everyone who finds time to read this and even more thanks to those willing to help out.

       

      Best regards

        • Re: Pump flow simulation
          Alex Clarke

          Right, so:

           

          First, your model setup. Because you're interested in power requirement at a given flow rate, you need to have mass/volume flow rate as one of your boundary conditions:

           

          Inlet boundary condition should be your mass or volume flow rate.

           

          Outlet boundary condition should be TOTAL pressure, set to 101325Pa (1Bar). This is a combination of static and dynamic pressure, remembering that when you have fluid exiting a fan/pump exhaust, some of the pressure must, by definition, be dynamic.

           

          The vortex crossing the pressure opening warning is just that, a warning. In your case, you would expect air to flow through the exhaust (Pressure opening) so I wouldn't worry about it. I get this warning on Centrifugal fan simulations all the time.

           

          The other problem you have is a little more fundamental; in an incompressible flow the volume flow rate at ALL points in the system will be constant. I suggest you do a little more background reading on fans, and in particular fan curves. This booklet is a personal favourite:

           

          http://www.trox-tlt.de/downloads/075547b0eb5193ae/346_elementary_fan_technology.pdf

           

          Below is a post I wrote to another student who was doing a Pelton Wheel simulation and looking to get the RPM required to provide certain flow conditions. The principle is the same, just liquid rather than gas:

           

          Set up your Pelton wheel model, and use a rotating region to encompass it. You'll need to use a transient study (Time-dependant).

          Set up a surface goal for torque and then select all of the faces that you want to evaluate the torque on (Then torque times rpm is power consumed).

           

          Set your discharge flow and head up as outlet and inlet boundary conditions, and set up surface goals for each of these. Set up your rotating region at a sensible speed (Just your best guess will do fine for now).

           

          Then you can do a  'goal optimisation' which falls under the parametric studies menu. Set up rpm as your goal to optimise (Target should be set as 'lowest' or something similar) and Solidworks will work out the lowest rpm at which the Pelton wheel can achieve the flow conditions.

           

          Personally I use lots of equation goals (Things like pump developed power (Pressure x flow rate), pump consumed power (Torque x RPM) and then efficiency and so on.) so that I can output the results to excel.

           

          Have a play with this and let me know how you get on, I do this with Centrifugal Fans all day long so can help.

           

           

          So there you have how to set up your fan consumed torque readout, you can do fan consumed power (Torque x RPM), fan developed power (Fan eye volume flow * Static pressure) and then calculate efficiency.

           

          What I haven't done is used the Parametric Study feature to vary fluid density, and in my version of Solidworks (2015) it does not seem to be selectable as a parameter to vary. Nevertheless, you can just copy the studies and change the fluid parameters every time, which shouldn't be too ardous.

           

          What might be a much better thing to do is to find the most efficient RPM at which to convey fluids of different densities. In which case, you would need to set up an equation goal for efficiency (Which we mentioned above) and use that for a goal optimisation with RPM as the variable. Then Solidworks varies the RPM until the most efficient point is reached. You can repeat these goal optimisations with each different fluid. (I'm actually doing something pretty similar myself at the moment!).

           

          Have a try and let me know how you get on.

           

          Hope this helps,

           

          Alex

            • Re: Pump flow simulation
              Safet Seta

              Thank you for your reply and willingness to help.

               

              I've set the BC's as you've said, inlet volume flow (50m^3/h) and outlet total pressure.

              rot.png

              flw.png

              prs.png

              The results are as follows:

              plot.png

              plot2.pngž

              They are more than weird... What causes this intense pressure  drop on the outlet(there might even be a negative pressure)? Why is there no suction pressure at the inlet of the pump?

               

              I tried the similar on an another pump model, I get now the contrary results... a huge inlet negative pressure where the inlet flow boundary condition is set...

              Untitled.png

               

              I clearly must be doing wrong in these basic things. With results like there any further steps in your explanation are a dangerous road for me to thread.

              Hope to hear from you again and I sincerely hope that these pictures will not be face palm material after you see them...

                • Re: Pump flow simulation
                  Alex Clarke

                  Initially that did seem a bit odd, but then I noticed that you don't seem to be running a Transient (Time Dependant) Study.

                  You'll notice that in your 5th screenshot, the air is actually bypassing the fan eye, which tells me that the flow boundary condition is driving the flow rather than the fan. This means that the rotating region clearly isn't working as expected, and it's probably because you have't given it time to spin up to speed.

                   

                  I also need you to check that, in your boundary conditions, the thermodynamic parameters are just at their default values. If in doubt, delete them and reinsert them as above.

                   

                  With Rotating Systems that are not axially symmetric, you need to do a Transient Study.

                   

                   

                  Here's how to set one up:

                   

                  In General Settings, select rotation; Local Region Sliding (Averaging isn't suitable here, since the volute/fancase is not axially symmetric):

                   

                  Forum 1.jpg

                   

                  Leave all the other General Settings as default.

                   

                  Then your Calculation Control options:

                   

                  For your finishing criteria, you can use Goals Convergence which looks at the change in the target values from iteration to iteration and stops the study when the change is below a certain percentage, which you can set. For fans, it's better to just set a number of iterations to allow the flow to fully develop. You need about 6 full rotations of the fan to get a nice fully developed flow, which requires a bit of trial and error to get right because Solidworks automatically varies the time step size depending on the cell count and rotation speed.

                   

                  Luckily for you, the fans I work on spin at about the same speed (325 rad/s) so I can just tell you to use 3000 iterations as a starting point.

                   

                  Forum 2.jpg

                   

                  Also make sure flow freezing is disabled in the Solving tab.

                   

                  Meshing!

                   

                  I don't know what your mesh looks like, and I don't think it is causing the problems that you are having above, but just to make sure you're on the right track, watch these:

                   

                  SOLIDWORKS Flow Simulation – Basic Meshing

                   

                  SOLIDWORKS Flow Simulation – Advanced Meshing

                   

                  I tend to have about 300,000 to 400,000 cells, where I have a local mesh refinement in the rotating region to get better mesh resolution across the fan.

                   

                  Solving:

                   

                  Patience is key, mine take about 16-24 hours to solve EACH! You can do a preview int eh solving window to see the pressure profiles to develop, which can be useful for spotting mistakes early on.

                   

                  Rotating Region:

                   

                  Don't just finish the rotating region at the outside diameter of the fan, it should finish halfway between the outer diameter of the fan and the closest part of the fancase (cutoff or tongue). When viewed from the top, the rotating region should finish at the outer faces of the fan.

                   

                  Results:

                   

                  Here's how I would expect a Pressure profile to look:

                   

                  Forum 3.jpg

                   

                  Have another go, and then if that doesn't work you can upload your model and I'll have a look.

                   

                  Have fun,

                   

                  Alex

                    • Re: Pump flow simulation
                      Safet Seta

                      I set the inlet to 100 m^3/h, outlet pressure to total pressure at 1 Bar and the rotating region to 3000RPM as sliding as you've shown to me. In the calculation options the fluid freezing was already disabled, and I've set the number of iterations to 3500. I've put the mesh to a level 2 refinement because currently I want to see close to real results before I head for the most accurate, so I wanted to save a bit of time.

                      About the rotating region, I've extended it as you've instructed and with it that was the results got better but still there are some things not clear to me. Here are the screens of the results:

                      rotating.png

                      flowtrajectories.pngcutplot.png

                      Now the insane pressure drop in the outlet pipe is gone, and I did not receive a vortex error at all. Considered the colors the results may appear correct, but judged by the numbers, not at all.The outlet pipe pressure is below atmospheric  Since the fluid is water and the rotation region is set to 3000RPM I expected the pressure to be way above. The flow trajectories feel a bit off too. My fails and lack of knowledge are sure a proof of me being a very beginner..

                      Are you able to open SW2016 files since you've said you have 2015. version? This pump was modeled in 2017. version, but the other pump I was experimenting on was 2016. I would like to send you  the prepared  files of it to you and if you have the will and time, could you set it up correctly, and I'll do the simulation my self, leave the laptop on for however much time needed. The fluids I want to simulate are water, plastic mass and slurry

                       

                      Thanks so much for all the help provided so far, I hope this post will be useful for other people too, but guess I'm kind of a slow learner.

                        • Re: Pump flow simulation
                          Alex Clarke

                          Hi Safet,

                           

                          Unfortunately I can't open 2017 or 2016 files on my 2015 version, but it looks like you're almost there to be honest. Flow Trajectories and pressure profile look about right to me.

                           

                          What type of pressure is the plot? Remember that it includes Static and Dynamic pressure. You can plot Dynamic Pressure separately to give you an idea of how much of the pressure is Dynamic and how much is Static.

                           

                          Personally I don't have much experience with water pumps, but it doesn't look like the Outlet Pressure pipe is below 1 bar (I wouldn't use atmospheric for fluids, it gets a bit confusing!).

                            • Re: Pump flow simulation
                              Safet Seta

                              Hi Alex,

                               

                              Well, I tried numerous combinations with the inlet flow and outlet atmospheric/total/static pressure putting values in the total pressure that  I'm likely to expect but to no avail. Thanks to you, I managed to get the suction pressure at the inlet and normal pressure distributing across the housing and outlet pipe in a sense that there are no vortexes or insane pressure drops.

                              In a centrifugal pump, be that for water or other material, it is expected to have high outlet pressure(i.e. 4-5-6 Bar) in order to be able to pump trough a pipeline system and overcome the friction losses.

                              All the tutorials and posts I could find were all explained as inlet and outlet pressure opening @ environmental pressure.

                              Don't think of me as ungrateful, but I don't feel any closer to solving this, since I've really tried everything I knew and everything you taught me, but nothing did give the expected results at the outlet. I've learned how to set up a time dependent study and rotating region dimension, and that is a great benefit.

                               

                              I thank you for your cooperation and all the help provided, and I know that you'd help if you knew, but it's not in your domain.

                                • Re: Pump flow simulation
                                  Amit Katz

                                  You will not see a high static pressure in your model, because you are discharging to atmosphere. If you had a piping system modeled in to provide the necessary backpressure then that would be a different story. But you don't really need that, because you can figure out what you're getting out of the pump by measuring the total pressure at the outlet.

                        • Re: Pump flow simulation
                          Amit Katz

                          Why set the outlet to total pressure? In this simulation you are modeling a fan venting to the atmosphere. By setting the total pressure to be equal to stagnant atmospheric pressure you force the high velocity air to have low (static) pressure at the outlet. This also doesn't make sense physically. A fan puts work into the air, it increases the energy in the air. The outlet air should have a higher total pressure than the stagnant atmospheric air that it breathed in.

                           

                          I would set the outlet BC to be environmental pressure, or set a static pressure BC of 1 atm.