# Pressure boundary condition

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

 August 27, 1998, 09:59 Pressure boundary condition #1 C-H Kuo Guest   Posts: n/a I am new here, I hope the following question is also new. For a inlet-outlet flow problem, if only pressure is imposed on both in/out boundary, can we get a convergent or unique solution? I asked this question to many, and most answers are positive. There should be a solution for the imposed pressure drop across the flow domain. I do not agree with it, but I am not confident with myself and it is in my mind for long. Here, I found a place to make it clear. My point is that if no velocity constraint is imposed on either in or out boundary, there is no convergence or the solutions have infinite sets. 1.Pressure gradient is a driving force for the momentum, it should drive whatever given velocity at inlet and render a certain velocity at outlet. If no velocity constraint at in or out boundary, target is missing. 2.Usually, up to my knowledge, at pressure boundary a zero normal gradient (or similar) B.C. is internally set to velocity field in order to solve the momentum equation. This leads the momentum equation to a situation similar to the Pressure Poisson equation of segregated solution method. 3. Possibly, some equation may be used to calculate velocity at in or out boundary based on a pre-calculated pressure field. Would this fix the velocity? sepidehkavousi likes this.

 August 27, 1998, 11:18 Re: Pressure boundary condition #2 John C. Chien Guest   Posts: n/a For incompressible flow, you can specify the pressure at one location only in the computational domain. Normally, this pressure value is specified at the inlet ( one point only). This will give you the freedom to specify the inlet velocity distribution. For the compressible flow ( where the density is related to the equation of state, or the similar equation), you can set the pressure at the inlet and the outlet. Be careful not to over-specify your boundary conditions. In the incompressible flow, when you specify the inlet velocity distribution and the pressure at one point, your whole problem is fixed. You can not specify the exit velocity ( possible violation of continuity equation) or exit pressure . In the compressible flow, the density will adjust itself to fit the pressure conditions.

 August 27, 1998, 11:53 Re: Pressure boundary condition #3 C-H Kuo Guest   Posts: n/a Thanks for your comments; it makes me relaxed. Indeed, I believe that in most commercial codes, pressure boundary condition has internal or user specified flexibility to adjust pressure values at each boundary node or face. If I fix my question on putting only pressure (static) on in/out boundaries, and no velocity is specified, would this make a solution? Incompressible flow should fail in this B.C. Is there any way for compressible flow to fix the velocity? I know stagnation at inlet can confine the velocity, which actually fix the total pressure and flow direction, and thus a limitation for the inflow velocity magnitude. My experience is limited to finite volume code. Is there any other way out?

 August 27, 1998, 12:29 Re: Pressure boundary condition #4 John C. Chien Guest   Posts: n/a For laminar , incompressible fully-developed constant diameter pipe flow , the velocity profile is second-order parabolic profile. The pressure drop (between inlet and the exit ) is a function of the flow rate ( or the mean velocity ) and the viscosity. So if you specify the pressures at the inlet and the exit, the pressure drop is known. The flow rate is also known. Thus the velocity profile is known. You are not allowed to change ( or specify) the velocity in this case. You can specify the velocity at the inlet for subsonic flow. You must specify the velocity at the inlet for the supersonic flow ( the inlet condition for supersonic flow has to be fixed .) But, you can not over specify the inlet conditions. The stagnation condition at the inlet is just a local derived condition, that is , it is just an algebraic relationship between other flow variables. Let's say A, and B are two flow variables ( or thermodynamic variables), you can defined a new flow variable C = A + B. You can use A and B, or C and B, or C and A.

 August 27, 1998, 13:18 Re: Pressure boundary condition #5 andy Guest   Posts: n/a Imposing a constant pressure drop and allowing the mass flow to adjust is probably the most common inlet/outlet boundary condition for simple LES predictions. The inlet/outlet velocity boundary condition is periodic as is the inlet/outlet pressure condition plus a constant for the pressure drop. The flow adjusts until the wall shear stress balances the imposed pressure drop. The same would hold true for a RANS prediction. There will be no problems so long as the net mass flux is exactly zero when the pressure correction equation is solved and there is only one exit (otherwise the split would have to be specified). The inlet and outlet velocity profiles would have to be adusted together at the end of each time step. The obvious thing to do would be to integrate the forces on the solution domain and use the imbalance to adjust the momentum flow (depending on assumed velocity profile shapes/angles etc...). I am not sure if you can do this with commercial codes? It would be disappointing if you could not.

 August 27, 1998, 14:35 Re: Pressure boundary condition #6 C-H Kuo Guest   Posts: n/a thanks for your comments. Indeed, I missed the point of force balance. I need to correct my previous statement that "infinite set of velocity" was wrong. From your explanations, we should have the shear stress and velocity/turbulence well correlated so that they will converge consistently. Actually, you gave me a good point to start with. Is there any stability or consistency trap hide in your approach?

 August 27, 1998, 15:47 Re: Pressure boundary condition #7 andy Guest   Posts: n/a Not in an LES prediction with periodic boundary conditions and a time step below the Courant number. For an implicit RANS prediction it is likely the boundary treatment would be explicit so it may be wise (necessary) to add relaxation. I am uncertain quite what you mean by consistency (and I would hestitate to make absolute statements about coupled non-linear equations) but in my experience if the treatment is based on sound physical reasoning there should be no problems. I would suggest a force balance fits into this category.

 August 27, 1998, 20:46 Re: Pressure boundary condition #8 Philip Zwart Guest   Posts: n/a There is nothing wrong with specifying pressure at both the inflow and outflow; many systems require just that. But specifying only pressure at an inflow leads to an underconstrained system and poor convergence. The commercial code I know (CFX-TASCflow) requires flow direction to also be specified at pressure inflows; I have tried this also with my research code and it works well. Hope this helps, phil

 August 28, 1998, 03:31 Re: Pressure boundary condition #9 laliong Guest   Posts: n/a I agree with you. Since only the gradient of pressure is contains in the incompressible NS equation, the absolute value is not necessary to be specified.

 August 28, 1998, 12:07 Re: Pressure boundary condition #10 John C. Chien Guest   Posts: n/a When using someone else's code ( a commercial code, a research code, a modified code or ....), if you are not sure of the boundary conditions required, the best approach is to check the final computed results in the area of boundary conditions against the boundary conditions you specified. If the computed result is different from your input condition, or if there is a sudden change in the smoothness of solution at the inlet, exit, or boundary locations, then you may have over-specified boundary condition problem. This is especially true, when the code was streamlined by non-CFD programmer. ( it happens from time to time.) In the modified version, sometimes you are asked to provide all the information at the inlet. So be careful. Fine likes this.

 August 26, 2015, 07:45 Reagarding Mass flow analysis of a control valve #11 New Member   Palash K. Bhowmik Join Date: Mar 2014 Posts: 3 Rep Power: 4 I a novice in CFD. Regarding mass flow analysis of a control valve, I need your suggestion. For my study: Fluid is air, iso-thermal process. (1) Inlet boundary condition is Total pressure inlet, outlet boundary condition is static pressure outlet. Suppose for a pressure ratio (Static Pr. @outlet/ Total Pr.@inlet) 0.5 if I set my inlet total pressure 2 Bar, the outlet static pressure will be 1 Bar. But my confusion is that in the software the outlet pressure is marked as relative pressure. If I consider the reference pressure that is the atmospheric pressure (~1 Bar) than the outlet relative pressure will be zero or one? I am confused !!! (2) And one more thing for my process may I use constant density?

 September 17, 2015, 11:41 How to properly set up boundary conditions #12 New Member   Join Date: Sep 2015 Posts: 1 Rep Power: 0 Maybe you will find this article useful. It's written by an expert in simulation, he talks about Dirichlet, Neumann and Robin. https://blog.simscale.com/blog/2015/...ur-simulation/

September 12, 2016, 09:03
#13
Member

annn
Join Date: Jun 2016
Posts: 37
Rep Power: 2
Quote:
 Originally Posted by John C. Chien ;465 For the compressible flow ( where the density is related to the equation of state, or the similar equation), you can set the pressure at the inlet and the outlet. Be careful not to over-specify your boundary conditions.
if you specifiy the pressure at the inlet and outlet can you not even fix any other feild? for example not even temperature, k, omega, etc.?

September 15, 2016, 10:07
#14
New Member

Marion
Join Date: Apr 2013
Posts: 15
Rep Power: 5
Quote:
 Originally Posted by cleoo if you specifiy the pressure at the inlet and outlet can you not even fix any other feild? for example not even temperature, k, omega, etc.?
You have to. Temperature, k and omega(epsilon or whatever turbulent variable you are using) should be specified

September 15, 2016, 10:58
#15
Member

annn
Join Date: Jun 2016
Posts: 37
Rep Power: 2
Quote:
 Originally Posted by cymbourne You have to. Temperature, k and omega(epsilon or whatever turbulent variable you are using) should be specified
Thanks for responding,
does the fact that the case is incompressible or compressible make a difference?

September 15, 2016, 11:55
#16
Senior Member

Filippo Maria Denaro
Join Date: Jul 2010
Posts: 2,518
Rep Power: 31
Quote:
 Originally Posted by cleoo Thanks for responding, does the fact that the case is incompressible or compressible make a difference?
yes, greaat differences.

September 15, 2016, 16:50
#17
New Member

larmes
Join Date: Aug 2016
Posts: 24
Rep Power: 2
Quote:
 Originally Posted by FMDenaro yes, greaat differences.
I meant in terms of fixing the other variables that is if pressure is fixed at the inlet and outlet in a compressible case can I still fix the other variables like T, omega,k etc?

September 15, 2016, 17:03
#18
Senior Member

Filippo Maria Denaro
Join Date: Jul 2010
Posts: 2,518
Rep Power: 31
Quote:
 Originally Posted by yeya I meant in terms of fixing the other variables that is if pressure is fixed at the inlet and outlet in a compressible case can I still fix the other variables like T, omega,k etc?

https://www.researchgate.net/publica..._viscous_flows

September 16, 2016, 03:19
#19
New Member

Marion
Join Date: Apr 2013
Posts: 15
Rep Power: 5
Quote:
 Originally Posted by yeya I meant in terms of fixing the other variables that is if pressure is fixed at the inlet and outlet in a compressible case can I still fix the other variables like T, omega,k etc?
You still have to fix other variables (try to think in terms of the number of transport equations you are solving).

It would be different if you considered a supersonic flow instead. In that case, you'll have to specify one more variable at the inlet instead of doing it at the outlet.

Cheers,

 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 Saturn CFX 45 February 8, 2016 05:42 peob OpenFOAM Running, Solving & CFD 2 August 14, 2014 09:07 Attesz CFX 7 January 5, 2013 04:32 abishek FLUENT 1 July 28, 2008 08:14 chiseung FLUENT 1 June 19, 2001 21:05

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