# Pressure Driven Supersonic Flow in Converging-Diverging Nozzle

 Register Blogs Members List Search Today's Posts Mark Forums Read

 June 4, 2013, 15:12 Pressure Driven Supersonic Flow in Converging-Diverging Nozzle #1 Member   Join Date: May 2013 Location: Canada Posts: 32 Rep Power: 4 After extensively reading through the forums and running a number of test cases, I still can't find suitable boundary conditions for my geometry. Hopefully someone here will have had previous experience and may be able to provide some input. I'm trying to simulate a supersonic converging-diverging nozzle for comparison to experimental results. The known conditions are: stagnation p and T at inlet of 300kPa and 1200K, wall temp roughly 600K, Mach number of 2.03 at outlet, and based on a gas dynamics analytical calculation for design conditions, the outlet static pressure should be roughly 37kPa (isentropic). I've tried a number of boundary conditions as below, implemented in OF 2.1.1, and using rhoCentralFoam with kOmegaSST. For all cases, the temperature was defined as follows: Code: ``` INLET { type totalTemperature; gamma 1.34; T0 uniform 1200; value uniform 1200; } OUTLET { type zeroGradient; } WALL { type fixedValue; value uniform 600; }``` Case 1: This case has been the most promising; however, the flow settles with an outlet static pressure around 31 to 36kPa, below the expected 37kPa. Maybe this is an effect of a turbulent boundary layer or something else? Further reducing lInf to 0.001 causes the simulation to crash with a high pressure gradient near the outlet. Pressure, P Code: ``` INLET { type totalPressure; p0 uniform 300000; U U; phi phi; rho rho; psi none; gamma 1.34; value uniform 300000; } OUTLET { type waveTransmissive; value uniform 37000; field p; gamma 1.34; phi phi; rho rho; psi psi; lInf 0.1; fieldInf 37000; } WALL { type zeroGradient; }``` Velocity, U Code: ``` INLET { type zeroGradient; } OUTLET { type zeroGradient; } WALL { type fixedValue; value uniform (0 0 0); }``` Case 2: This case implemented the desired static pressure at the outlet of 37kPa. The velocity was defined as in Case 1. The solution crashes after a few thousand iterations with a large pressure gradient at the outlet (similar to the small lInf in Case 1). Pressure, P Code: ``` INLET { type totalPressure; p0 uniform 300000; U U; phi phi; rho rho; psi none; gamma 1.34; value uniform 300000; } OUTLET { type fixedValue; value uniform 37000; } WALL { type zeroGradient; }``` Case 3: This case is the same as Case 2, except for a fluxCorrectedVelocity boundary implemented at the outlet. Again, there is a large pressure gradient (even larger this time) at the exit. Velocity, U Code: ``` OUTLET { type fluxCorrectedVelocity; phi phi; rho rho; }``` Case 4: This case implements the fluxCorrectedVelocity outlet velocity boundary condition (as in Case 3) with a waveTransmissive outlet pressure boundary condition (similar to Case 1, but lInf = 0.01). The simulation does not crash, but the pressure is far too high (between roughly 200 and 400 kPa) and fluctuates wildly with no apparent trend to settle. Conclusions: Does anyone have any suggestions for further boundary conditions that I could explore? Or any comments on the above cases? Case 1 is the only usable result so far, but I'm not confident that waveTransmissive is beneficial in this case since I don't have any shocks in the developed flow and I want the flow to relax to a given static pressure at the outlet, not artificially at a distance from the outlet. But when I specify the desired static pressure, a pressure gradient develops at the outlet and crashes the simulation. Thanks for reading, and I appreciate any help. Last edited by cdm; June 4, 2013 at 16:30. Reason: Case 4 BC correction.

 June 5, 2013, 08:00 nozzle #2 Member   Join Date: Nov 2012 Posts: 55 Rep Power: 4 im using this BC: pressureInletOutletVelocity for U are you just simulating the nozzle without a wake?

 June 5, 2013, 12:49 #3 Member   Join Date: May 2013 Location: Canada Posts: 32 Rep Power: 4 I tried using that boundary condition on the outlet, but it didn't help when specifying a static pressure. What pressure BC do you use with it? There are no shocks in my system, and I'm not concerned with the wake. What I'm trying to investigate is temperature distribution in a constant area downstream of the throat.

 July 19, 2013, 10:32 #4 New Member   Jason Pearl Join Date: Jul 2013 Location: Burlington Posts: 10 Rep Power: 3 I'm working on a similar problem supersonic flow in a MicroNozzle. for your temperature field have you tried using totalTemperature BC for the inlet with inletOutletTotalTemperature at the exit? might be something to look into. Though it might be difficult to use when the walls are not adiabatic. Also for the velocity I had better luck with pressureDirectedInletOutletVelocity and pressureNormalInletOutletVelocity (just be aware of patch orientation for the latter) for pressure I am using totalPressure and waveTransmissive. Also what is the exact function of Linf. Does it weight the impact of the farfields effect on the BC? where larger would Linf decrease the effect of the farfield on the BC? cheers

 July 21, 2013, 16:24 #5 Member   Join Date: May 2013 Location: Canada Posts: 32 Rep Power: 4 jaason, thanks for your input. I'll have a look at your suggested boundary conditions. Right now I've been using (inlet / outlet, respectively) totalPressure / waveTransmissive for Pressure, totalTemperature / zeroGradient for Temperature, and zeroGradient / inletOutlet (with inletValue uniform (0 0 0) for the outlet). I believe what you say is roughly how lInf is expected to work. It relaxes the BC pressure such that it would realise a farfield pressure pInf at a distance lInf from the BC patch. If lInf = 0 it would essentially be forcing a fixedValue. However, for large lInf, I think I read that sometimes there is trouble with convergence and having large oscillations in the outlet pressure. So far it appears to work fine for my supersonic flow nozzle with over-expanded conditions.

 Tags converging-diverging, nozzle, pressure driven, supersonic

 Thread Tools Display Modes Linear Mode

 Posting Rules You may not post new threads You may not post replies You may not post attachments You may not edit your posts BB code is On Smilies are On [IMG] code is On HTML code is OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post jr33 OpenFOAM Running, Solving & CFD 1 August 7, 2013 11:00 Betty Main CFD Forum 13 May 24, 2012 00:26 kokoory FLUENT 0 August 17, 2011 02:07 farhan OpenFOAM Running, Solving & CFD 1 April 14, 2009 14:34 jane luo Main CFD Forum 15 April 12, 2004 17:49

All times are GMT -4. The time now is 03:16.