# Pressure Inlet Velocity

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

 June 19, 2009, 00:18 Pressure Inlet Velocity #1 Senior Member   Prapanch Nair Join Date: Mar 2009 Location: Bangalore, India Posts: 105 Rep Power: 9 Hi, I am trying to solve flow through a 'S' shaped pipe. Both the bends in the pipe are very close to the inlet and the outlet. The inner wall of the pipe has a lot of projections. I want to see what average flow velocity I would be getting after setting a pressure difference between inlet and outlet. I had set a pressure value 15 Pa at the inlet and 0 Pa at the outlet. I used pressureInletVelocity BC at inlet and inletOutlet BC for outlet for the velocity. And for pressure, I used fixedValue BC at the inlet and outlet. After about 400 iterations ( steady state incompressible flow) I checked the field and found very high value for pressure within the field ( of the order of 10^30 ) . Could someone please point me the mistakes with my boundary condition or suggest me a solution? Thanks, Prapanj.

 June 19, 2009, 04:10 #2 Member   Julian Krick Join Date: May 2009 Location: Guelph Posts: 88 Rep Power: 9 Hi, I have experienced a similar effect. I'm simulating a convergent-divergent supersonic nozzle. I also set the pressure difference of 300mbar between inlet and outlet. BCs for inlet: - pressure: 'totalPressure - velocity: 'pressureInletVelocity' BCs for outlet: - pressure: 'static pressure' - velocity: 'zeroGradient' I'm using the sonicFoam solver. What happens is that at some point during the iteration process the velocity near the outlet increases drastically, furthermore, also at the outlet, value for pressure are either very high or negative. I suppose this effect is evoked by the outlet boundary condition. __________________ grid generation: ICEM CFD 13.0 solver: CFX 13.0

 June 19, 2009, 05:23 #3 Senior Member   Prapanch Nair Join Date: Mar 2009 Location: Bangalore, India Posts: 105 Rep Power: 9 Julian, Could you explain why you used totalPressure at Inlet? For viscous compressible flow, there will be a total pressure loss if there is a stationary shock in the CD nozzle. Have you used totalPressure at inlet before? Prapanj.

 June 19, 2009, 05:41 #4 Member   Julian Krick Join Date: May 2009 Location: Guelph Posts: 88 Rep Power: 9 Actually my task is to compare the results of the OpenFoam simuatlion of the CD nozzle with results we got from calculation with a different solvers. In these calculations there was a total pressure defined at the inlet., so I did the same in order to be as synchron as possible. Nevertheless, I also used the 'fixedValue' BC-type for the pressure at inlet and outlet and got the same effect of instability. I didn't use the 'totalPressure' BC in any of my other simulations. __________________ grid generation: ICEM CFD 13.0 solver: CFX 13.0

 June 19, 2009, 06:00 #5 Senior Member   Prapanch Nair Join Date: Mar 2009 Location: Bangalore, India Posts: 105 Rep Power: 9 Hey, When you say static pressure, do you mean fixedValue? If not, set a fixedValue for pressure at the outlet. Or, try this: Use wave transmissive pressure . I hope you have the user guide for openfoam, which available for download (google for it). Page U-129, there is table. Look for pressureTransmissive, that lets you set a pInf for ambient pressure. You issue may be due to shock waves being reflected off the outlet. Have you tried visualizing your interim results? Prapanj.

 June 19, 2009, 07:38 #6 Member   Julian Krick Join Date: May 2009 Location: Guelph Posts: 88 Rep Power: 9 Yes, by static pressure I mean 'fixedValue' type of boundary condition for pressure - I hope my interpretation of 'fixedValue' for pressure is correct. Thus, as mentioned, I already tried a 'fixedValue' BC for pressure at the outlet but came the same result -but thanks for the hint. As you suggested, I looked at page U-129 for finding the definiton of the 'pressureTransmissive' BC. That sounds promising. However, when I was looking in the internet for a description on how to define 'pressureTransmissive' I found that this BC was substituted by the 'waveTransmissive' BC in OpenFOAM v.1.4: http://www.openfoamwiki.net/index.ph...dary_condition Furthermore, I couldn't find 'pressureTransmissive' BC in the OF C++ Source Guide. Anyway, I applied the 'waveTransmissive' BC to the outlet and it seems to work! However, the simulation is still running and I couldn't yet take a look at the results. But anyway, thank you very much prapanj ! Here is my /0/p file: Code: ```inlet { type totalPressure; p0 uniform 1.01325e+05;//:p_in U U; phi phi; rho none; psi none; gamma 1.4; value uniform 1.01325e+05; } outlet { type waveTransmissive; value uniform 71325; //important for correct I/O field p; //the name of the field that we are working on gamma 1.4; //the ratio of specific heats phi phi; //the name of the volumetric flux field (or if you use the mass flux phi, it will be divided by rho) rho rho; //the name of the density field psi psi; //the name of the field that is the deriv. of density with respect to pressure lInf 1; //a measure of how far away the far-field condition should be fieldInf 71325; //the far-field value to be applied to p }``` While I was searching the internet I found the following BCs, which could also be adequate for my problem: - waveTranmissive (- pressureTransmissive) - freestream - frestreamPressure - supersonicFreestream Unfortunately, I wasn't able to find an appropriate description of the last three BCs, listed above. Do you know, what they do? __________________ grid generation: ICEM CFD 13.0 solver: CFX 13.0

 June 19, 2009, 07:48 #7 Senior Member   Prapanch Nair Join Date: Mar 2009 Location: Bangalore, India Posts: 105 Rep Power: 9 Hey, What version of OF do you use? Is it 1.4? Well ther eis a later version 1.5 that is realease. And a even recent version 1.5.x released. However you will have to compile 1.5.x. The boundaries that are missing in your installation may be found in 1.5.x Freestream as I understand is suitable for use in external compressible flow. Like, flow around aerofoil etc. And I haven't looked into the codes of those (Even if I look, I am not sure I can figure out). Check the intermediate results and say if it works. Prapanj. (Ps: are you from a German University? )

 June 19, 2009, 08:06 #8 Member   Julian Krick Join Date: May 2009 Location: Guelph Posts: 88 Rep Power: 9 I'm using OF 1.5. The interim results look okay; simulations are still running and stable. Thanks!. I hope they won't blow up again. At the beginning of next week I can tell if it worked out. Yes, I'm a Bachelor student at the university of Duisburg-Essen, located in Duisburg, Germany. __________________ grid generation: ICEM CFD 13.0 solver: CFX 13.0

 June 19, 2009, 08:08 #9 Senior Member   Prapanch Nair Join Date: Mar 2009 Location: Bangalore, India Posts: 105 Rep Power: 9 Np. And do post if it worked .

 June 22, 2009, 05:40 #10 Member   Julian Krick Join Date: May 2009 Location: Guelph Posts: 88 Rep Power: 9 Today, I looked at the results of my calculations. They are stable ! The BC 'waveTransmissve' seems to stabilize the simulations. There is no drastic increase anymore in pressure or velocity. So far so good. However, there is a different problem. For the simulation of my nozzle I need to have a pressure difference of 300mbar between the outlet and the inlet. At the inlet I have atmospheric pressure: Code: ```inlet { type totalPressure; p0 uniform 1.01325e+05;//:p_in U U; phi phi; rho none; psi none; gamma 1.4; value uniform 1.01325e+05; }``` At the outlet I have 'atmospheric pressure' - 300mbar: Code: ```outlet { type waveTransmissive; value uniform 71325; //important for correct I/O field p; //the name of the field that we are working on gamma 1.4; //the ratio of specific heats phi phi; //the name of the volumetric flux field (or if you use the mass flux phi, it will be divided by rho) rho rho; //the name of the density field psi psi; //the name of the field that is the deriv. of density with respect to pressure lInf 1; //a measure of how far away the far-field condition should be fieldInf 71325; //the far-field value to be applied to p }``` Now, the problem is that after some time, the pressure at the outlet will tend towards a value of 120mbar, which is far too low. With this pressure the instationary effects which I want to observe in the nozzle will not occur. Instead, the flow through the nozzle becomes stationary. So, what can I do to establish a pressure of ~700mbar at the outlet using the 'waveTransmissive' BC? Maybe I have to change the value for 'lInf'. What measure does this variable have, anyway? Is it in m or mm or dimensionless? By the way, can I use the 'waveTransmissive' BC for the inlet, as well? I encountered some shock waves, which traveled towards the inlet and unfortunately were reflected. __________________ grid generation: ICEM CFD 13.0 solver: CFX 13.0

 June 22, 2009, 23:57 #11 Senior Member   Prapanch Nair Join Date: Mar 2009 Location: Bangalore, India Posts: 105 Rep Power: 9 Hi Julian, You have set 'rho' as none at the inlet. Can you change it to 'rho' as in " rho rho; " and try again. I don't know if this would help. Prapanj.

 June 23, 2009, 11:15 #12 New Member   Join Date: Jun 2009 Posts: 8 Rep Power: 9 Hey ive been following this discussion I am trying to model barrell shocks in an axisymmetric model. Inlet air is M=1. The exit is a subsonic outlet. I am using rhoSonicFoam [modified to read p , rho, T, U fields , so that the solver can accept derived BCs ] , Im using non-reflective BCs at the exit for rho, since for subsonic outlet , the eigenvalue correspding to rho is -ve. However i am not getting the inlet BCs correct . I however am not getting the right combination of BC at inlet for p & rho. I ll summarize the Bc i have tried :-- p Inlet : totalPressure outlet : fixedValue [ static] rho inlet: fixedValue outlet : nonReflective. U inlet : 350 outlet : zeroGradient T Inlet : 250 outlet : zerogradient kindly suggest me a better combination ....

 Tags pipe, pressure difference, pressureinletvelocity

 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 emueller CFX 0 May 5, 2009 11:08 coolyihao FLOW-3D 0 March 17, 2009 11:17 eu-ric thean CFX 2 December 28, 2005 13:06 eric FLUENT 3 January 26, 2004 21:04 Ronak Shah FLUENT 0 June 4, 2003 09:44

All times are GMT -4. The time now is 11:35.