Hi  Bholu,

Is it your outlet condition exactly in the exit of nose? Have you some sketches of your problem? 

Dear Sir,

 I have not added the nasal cavity to my model. My model is from mouth to sixth generation. I run the simulation by taking velocity inlet and pressure outlet in case of inhalation. In this case the velocity was not changing at inlet but I could not validate the inhalation results with exhalation. Now I am running it by taking pressure inlet and pressure outlet bcs and in both cases pressure at inlet is slightly changing, which is supposed to remain same. Why it is happening? Could you please help me?

Dear Abdul Sir,

First of all thanx a lot. I am totally satisfy with your answer.  But when I am comparing my inhalation results with exhalation, I found there is about 4-5% of changes. The amount of volume inhale must be equal to the amount of volume exhale. I thought because of this change it is happening. Sir I am totally agree with your answer but whether we can fixed pressure or not ? 

Dear Bholu,

I think that prescribing pressure at the inlet and outlet is not favorable practice in CFD when using SIMPLE algorithm. Imagine steady friction-less flow in a straight horizontal tube. At any flow-rate the pressure at the inlet and outlet is the same. In this case there is no unique solution for the flow when prescribe inlet and outlet pressure. When you deal with friction flow in a pipe, the flow-rate is unique for a given pressure difference, but according to my experience this solution is hard to achieve by standard CFD codes. To test your CFD solver, try to find a solution of laminar flow (let say at Reynolds number of 2000) in a short straight horizontal pipe when prescribe pressure difference from the analytical solution. If you obtain a poor solution, my advice is to reconsider the boundary conditions in your problem (it is always better to have some boundary conditions with prescribed velocities).

Dear Bholu,

I am afraid you cannot impose the pressure at both the inlet and the outlet. Your problem will be overdetermined. Despite the pressure correction equation is of second order, the continuity equation, through which the pressure correction originates, is first order. Specify both inlet and outlet is not good. I suggest you to specify a volume flow rate at the inlet and the pressure at the outlet.

Dear Zdravko Sir,

Thank you sir. I was not getting trouble by taking combination of pressure and velocity boundary condition. Since flow inside human airways is causes due to the movement of diaphragm and hence creates the pressure difference. Even I could not match my inhalation results by results of exhalation with velocity inlet and pressure outlet bcs. The results was differ by 4-5 %. Is it acceptable in CFD ? That's why latter I was used Pressure inlet and pressure outlet bcs and could not match the results. Your answer is helpful for me and I will check it according to your suggestion. 

Hello Bholu,

Why don't you try with mass flow, if it is known to you. Otherwise try applying opening BC at outlet, find mass flow and then apply it. Mass conservation has to be there in any case. Please check.

hope it helps.

(I am assuming mesh convergence study is conducted)

You should try a total pressure boundary condition for the inlet. This BC does not fix pressure or  velocity, but the total pressure wich is p+0.5*rho*V^2. And a fixed pressure value at the outlet. I also suggest that you take the outlet of your domain as far as you can from the area that interests you the most.

What software are you using?, I could tell you how to implement this in OpenFOAM.

What you are triyng to solve is a pressure driven flow problem. So you can google "prssure driven flow Boundary conditions"  for whatever software you are using.

Hope this helps.

Dear Luis Francisco Sir,

First of all thank a lot. I am using Ansys fluent 15 for my simulation. How I will give the total pressure. In Pressure inlet boundary condition we get two options (i) Gause total pressure and (ii) supersonic/initial gauge pressure, so where we will provide total pressure? Dear Luis sir how can I implement this in OpenFoam ?

 Dear Abdrea and Sanket Sir,

As per your suggestions I have used mass flow inlet bcs and pressure outlet bcs in the both cases of inhalation and exhalation. It is satisfying the mass conservation at both ends. I reported a velocity of 2.65 m/s ( correspond to 60 l/m) at mouth in case of inhalation and a velocity of 2.85 m/s in case of exhalation. In both cases I have checked the area average velocity. Why the two different velocity reported at the mouth inlet ? Could you please help me?  And can be check absolute velocity in CFD Post ?

Mr. Kumar, I agree with Andrea Boghi that your problem will be overdetermined with both pressure conditions specified. Any solution you may force will naturally be in error. I would assume that you need to consider the basic facts that during inhalation only the inlet pressure is known and during exhalation, only the outlet pressure is known. The outlet pressure during inhalation (suction) has to be < inlet pressure and the inlet pressure during exhalation (blowing) should be  > the outlet pressure. The effect on air volume is not very great but it may introduce some error if you equate the volume flows. Similarly with mass flow: replacement of oxygen with CO2 and addition of water vapor. For a first order model, I suppose you may ignore these effects. If you have taken correct cognizance of the physics of the problem, a few % error is all right in the numerical solution, which is inherently always in error.

I don't think I can answer without additional data. The differences are  small in percentage (10%), Are you sure that the time averaged flow rate is zero? How the domain looks like? How many outlets? Is it rigid? Cheers

Respected Vijay Raghwan Sir,

Thank you very much and Its my pleasure to see you. I did My B.Tech from Dr. M.G.R University and I read lots of your books in my B.Tech. Sir I have one more doubt.. At time of exhalation I have reported different pressures at inlets (total 32 inlets - sixth generation model). Whether it should same or Different Sir ? At time of exhalation diaphragm relaxed and I thought there will be equal pressure difference through out all bronchus of the human respiratory tract. Whether am I right or wrong ? 

Dear Boghi Sir,

My model having one inlet (mouth) and 32 outlets and it is rigid. I run simulation of steady state and I have assumed fluid is incompressible. Sir I have attached a file that having sketch and bcs of it. Please help me sir.

I agree with Dr. Vijay. But let us simplify a bit the problem in order to extend the coverage to other people who might be interested in this matter. Suppose the flow of air in a convergent-divergent nozzle. Many people defend the idea of fixing the pressure in the inlet and outlet sections. In my opinion fixing the pressure at the outlet is possible only if you know the solution before hand. The pressure in the outlet section will be established by the conditions at the entrance and the geometry of the nozzle. If one tries to fix another pressure at the outlet section, a system of waves will form in the nozzle running up and down and trying to change one of the two pressures, inlet or outlet, in order to conform. The flow gets to a non-steady situation and an  eventual steady-state solution will never be obtained. So the best boundary conditions at the outlet would  be, in a general case, the so called convection-induced condition.

I'm in agreement with Luis Francisco. You can define a value of total pressure (absolute) at the inlet. The supersonic/gauge pressure in fluent, is used for an estimation of the inlet velocity (in incompressible flows Bernoulli equation is used, as Luis Francisco said) for initialise the flow field. In Fluent, you also can define a reference value of pressure, because Fluent computes pressure differences. You can put zero here, and use absolute pressures in both ends (inlet and outlet). If you consider a non-steady simulation maybe you can programme a UDF in Fluent with an f(t) for pressure...this maybe be work... But, what is your subject/interest for simulate this?

Hello,

I need some assistance regarding my problem ? I am modeling horizontal placed rectangular open microchannel with height, width, and length of 2 , 15, and 100 micrometers. The mesh is hexahedral mesh with all quadrilateral. In General section choose pressure-based and transient time. By marking absolute velocity. In setup use VOF model, which includes open channel flow, coupled level set method and Implicit body forces. Taking air as a primary phase and water as secondary phase. In which interaction include surface tension between water and air of 0.0735 mN/mM.

I am putting drop of water in contact with open microchannel. In boundary condition, inlet(water) is pressure inlet with volume fraction 1. outlet (mixture of water and air) is pressure outlet with 0 volume fraction. Atmospheric(air) as pressure outlet. In all this boundary condition I select open channel flow in the multi-phase option with free surface level 2 micrometer. Also, choosing operating density by default. By considering mixture for Wall Zone with stationary wall, no slip condition with wall adhesion between water and air of 90 degree.

Solution method, scheme - PISO, gradient - least square cell based, pressure - presto, Momentum - quick, Volume frcation - Implicit scheme.

Solution Initialization, Compute from - Inlet and initialize it. In patch select water and variable volume fraction with value 1 and zone to patch is liquid.

Run calculation with time step 1.0e+6 microsecond with 1000 iteration.

Please, help me if anything wrong in the above explanation of model. In this, I want to find out how much time fluid takes to travel through the end of channel with the effect of capillary force. But, I didn't got the correct results.

So. I hope somebody help me on this. Thank you in advance.