6 Replies Latest reply on Apr 26, 2011 10:33 AM by Chris Michalski

    Flow simulation in a venturi-type gas mixer?

    Jeff Anderson

      I am working on a project where I am trying to simulate flow through a venturi mixer.  We have a device that works, but need to improve its performance.  But I can't get Flow Simulation to correctly model it.  I am performing an internal flow simulation.  I am using Solidworks 2011 and Flow Simulation 2011.   The part consists of an orifice where a 50PSI  oxygen gas source is the inlet.  So I set the inlet pressure to Total Pressure 50 lbsft/in2.  It has a large inlet at the bottom of the part that is an atmospheric air inlet.  I left the atmospheric air inlet at default atmospheric pressure.  There is also a mixed gas outlet boundary condition that is set to atmospheric air.  I have tried changing a bunch of parameters including temperature of the inlet gas.  I have set the atmospheric boundary conditions to static pressure or atmospheric pressure. I have changed boundary conditions from laminar to turbulent and vice versa.

      Here are the problems that I have encountered.

      When I measure the flow of the the gas through the orifice in real life I reach a flow of 11.5 Liters/min.  In the simulation I only reach a flow of around 5.5 LPM exiting the orifice.  This also shows up in my total exit flow appearing much lower.  (I could set the flow rate coming out of the orifice, but that doesn't allow me to simulate the effects of changing the orifice, which I would like to do.)

      I am also trying to simulate the volume fraction of oxygen.  Essentially, I want to know what mix ratio I am getting.  It also does not match my actual device.

      I first tried to simulate the flow without an exit tube on it.  In our real-life application we have a series of tubes that the gas passes through after it exits our device.  I have simulated the flow with just one of the pieces of that tubing.  It gave me some terrible results.  It shows the gas mixture starting within the device where I have a oxygen concentration that gradually increase back to 100%.  I can't figure out where this extra oxygen is coming from.  From what I know, gas doesn't just unmix itself.  Here is an image of that simulation. (Coincidently, I performed a similar test to this where the long outlet tube seen below was smooth on the inside instead of corrugated like the actual tube). I can't believe that corrugation would really effect as much as the model is showing.  I have tried reducing the mesh, but then it has trouble modeling the gas exiting the orifice.  I tried simulating it with a localized mesh at the orifice and it also didn't work.

      OptiVenturi test with 2 ft section of tubing.jpg

      I have tried to break down each flow part separately to try to find the problem.

      I noticed in one of the forum threads, that another user was running a flow simulation similar to this except with water.  I turns out he had to do an external flow simulation.  Is that my problem? Has anyone else run a simulation similar to this who could help?

        • Re: Flow simulation in a venturi-type gas mixer?
          Chris Michalski

          Jeff -


          first off, to get close to the actual measured conditions: you say you set total pressure to 50lb/in2 but if you have 50PSI you are likely reading gage pressure compared to the atmospheric conditions.  You'd need to add the 14.7PSI of atmosphere so everything is in absolute pressure.  This will have a dramatic impact on the flow of your venturi as well the other parameters.


          As for the oxygen content increasing - if your ambient is oxygen and your exit tube is too short you may have reveresion of the ambient into the tube (were there any "a vortex crossed the boundary" warnings during simulation?)


          I used Flow to simulate a simple high temperature exhaust venturi system in the past and while I never verified it was spot-on, it was close enough that the system was tunable for desired performance.

            • Re: Flow simulation in a venturi-type gas mixer?
              Jeff Anderson


              You are right about gage pressure.  I essentialy have a tank of oxygen with a gage pressure of 50psi.  I have also run a simulation with the added 14.7 psi of atmosheric pressure.  I still didn't see the right flow results.  But I don't know if there are other conditions that also need to be set correctly.  I have run a simulation on just the orifice as well and I measured the flow exiting the orifice.  I tried increasing the pressure to 300 psi and it still didn't reach the right flow.   I have model some other compoenents that are upstream of the orifice and included them in the simulation with similar results.  I have set the boundary conditions at the correct oxygen/nitrogen ratio for air 20.9% oxygen to 79.1% nitrogen.  Solidworks didn't recognize that air is comprised of oxygen and nitrogen (plus other small amounts of gas).  Is the "ambient gas" the same as the boundary condition gas?

              Also I always get the warning ""a vortex crossed the boundary".  I just assumed that meant that I had gas (air) entering the inlet at the bottom of the device, which is true.

              Should I have the air inlet and the mixed gas outlet set to 14.7 psi with atmospheric pressure setting or with static pressure setting?  Thanks for the quick response.


                • Re: Flow simulation in a venturi-type gas mixer?
                  Chris Michalski

                  Jeff -


                  do you have a local mesh at the nozzle to get the resolution you need relative to the rest of the system?  If it approximates the inlet poorly then the area will be off and the volume flow will be incorrect also.


                  Yes, the ambient gas at each opening would be the same as the boundary conditions.  Flow has properties of air, but it does not sub-divide that into N2 and O2 and such, it is assumes constant concentration and uniform properties.


                  As for the "vortex" warning - if you take a cut plot and look at x-velocity (or whichever exit gives you axial velocity) you will likely see that gas is swirling at the inlet/exit so some of the ambient is pulled back in (or pushed out) the tube a short distance by an eddy current.  This means that you need to add a longer tube (or if the conditions at the end aren't critical I typically ignore them as opposed to increasing model size).


                  I do all of my simulations in metric pressures, so ambient is 101325Pa and I add that to the pressure estimates.  Unfortunately all of the models I can recall had defined mass flow rates for the gaseous inputs, not constant pressures.

                    • Re: Flow simulation in a venturi-type gas mixer?
                      Rich Bayless

                      Hello Jeff and Chris,


                      Mesh size in the tight spots can also be adjusted using two features in the Automatic mode.


                      Manual specification of the minimum gap size


                      insert a dimension that's about one half of your smallest inside diameter passage.


                      Advanced narrow channel refinement.


                      make sure this option is checked.


                      Use the 'mesh' section under results to examine your resulting mesh.


                      I'm also using an orifice to set a gas flow rate based on a constant inlet pressure.  As part of my initial runs, I decided to turn it around, at least until I can confirm that the model is working as expected.  In other words, I'm inputting the expected mass flow rate directly and letting Flow solve for the pressure.  This way I can at least see how the flow (and the mixing) after the orifice is working, based on my expected flow rates.  Later on, I'll go back to setting the pressure.


                      For the 100% oxygen business, as you said, gas doesn't unmix itself.  I'm using two gases, air and propane, both selected during the wizard setup as default gases.  Later I select one inlet as 100% air and the other inlet as 100% propane.  Mixing proceeds as one would expect.  It might help if you post screen shots of your general settings.



                        • Re: Flow simulation in a venturi-type gas mixer?
                          Jeff Anderson

                          Rich and Chris,

                          Thanks for the tips.  I have been able to solve some of the problems with my simulations.  I was wondering though.  I have the settings for the mesh up all the way so that I can closely analyze the gas exiting the orifice.  But I noticed that the mesh is tight in some other areas where I don't need it to be.  I know that I can select parts of an assembly and have them have a smaller mesh by using the local mesh option.  However, it appears based off of my simulations that I will need a local mesh right in front of the orifice?  Is there a way to create a tight mesh near the orifice and inside the orifice, but not as much detailed mesh elsewhere?  Any ideas. 

                            • Re: Flow simulation in a venturi-type gas mixer?
                              Chris Michalski

                              Jeff -


                              create a solid body that represents the volume inside which you want a finer mesh - both the solids and the fluids.  Place this part into your model.  Create a local initial mesh - select this new part, and then tell it to disable that part.  (If you do not disable it Flow will consider it a solid, when you disable it Flow sees it as a ghost and only uses it to define the region for the mesh.)


                              This allows you to control the mesh in that region independent of the general settings.  You can likely reduce the overall mesh refinement and keep the refinement in this area.  You may want to adjust the size of this part versus the local and general mesh settings.  As you reduce the overall mesh refinement you will have to judge whether the transition from fine local mesh to coarse general mesh is in a local you can accept.


                              You should be able to define the volume in which you want a coarser mesh as an alternative - then you wouldn't have to adjust the overall settings, simply dumb-down the mesh in those areas that don't matter.  I've never had a use to try this way but it should work just like increasing the local mesh.