Dear Anil Kumar, Ch.

Since mass flow rate of air is known, you can calculate velocity of air passing through the restricted passage by continuity equation. From the velocity of air, and sond velocity (at room temperature) inlet Mach number can be predicted. Knowig these parameters all other parameters at outlet of restrcted passage can be calculated from Gas tables.

Reference: Chapter-4; Isentropic flow-" Fundamentals of compressible fluid flows" by S.M. Yahya; New Age International Publishers, Delhi, India 

Gas Tables by the same author 

By using the equations and tables you can calculate the outlet pressure but this is not require at prior stage, since you are already simulating that flow over fluent so after simulation you can get the required properties at the specific point of domain.

So  for a case study you just apply different outlet  condition at the outlet and after followed by your analysis & grid independence test , you ill able to get the required data when you compared with the experimental data at validation stage.

use out let condition 

Thanks for the answer Prof.Maddali V S Murali Krishna,surely  I would try the method.

@Mr. Shirish Shukla ,I am using a compressible flow condition so outflow condition is not applicable in fluent ,looking forward for a reply.

Hi Anil,

I fully agree with Maddali, it is the best method to follow in your case as you dont have pressure information at exit, from my point of view.

@ Shrish, Raju and Anil,

It is always good, not to use Outlet boundary condition for any CFD analysis (in Fluent). Because pressure information is not accounted into the domain correctly, leading to a wrong results. Outlet condition is something like continuity, i.e. what ever comes into the domain will leave from the domain as well.

Outlet boundary condition works only with velocity boundary condition. Whenever pressure boundary condition is present, we pose additional condition to calculate pressure, which end up in wrong calculation. Also if there are more than one exit (outlet), in this case also outlet boundary condition won't work.

thanks!

Regards,

Rajesh.

@ Anil , Well there is two way to calculate that either by equations and tables data mathematically and second is the case study so i was suggested the same if you not sure about outlets then go through with case study and compare all the case study results at the end you ill come up with a exact conclusion as well as proper justification.

@ rajesh  you might be not come across with uncertainty in the cfd, some time just change solver setting from single to parallel leads the reason of wrong results. And we cant assume things without any exact justification and  case study  is the best way to deal with uncertainty because at end you ill able to justify your assumption.

Dear Anil,

Hope that some understanding has come by now. One thing that struck in my memory is about " Bernouli's Principle'. In a steady flow of liquid the total sum of energy is constant. That's what I remember. In that case the sum of Pressure energy, Kinetic energy, Potential energy is same. Pressure if to be increased, reduce other parameters. Hope this information is of some use.

@ Shrish, i do agree on the uncertainty associated with CFD. But the comments that i gave earlier are for my experience and based on the discussion that I had with the ANSYS techanical support orginations.For everthing that happens in CFD there is a reason, but most of the time we are not aware of them.

for more details please contact ANSYS techanical support orginations, link attached.

https://support.ansys.com/AnsysCustomerPortal/en_us

Dear Anil,

First thing I would do, is to calculate whats your critical mass flow rate, formulas for it can be easy found on the internet. If your geometry is like a sharp edged orifice, than your real critical mass flow rate is around 0.8-0.85 (i think 0.82 most often, depends also onthe geometry upstream of the restrictor) of the calculated theoretical value. You do that, to check if you are below the chocking point. If the mass flow you try to impose is greater than the critical one, than this is phisically impossible because no matter how low the backpressure would be, with given inlet total pressure, no more flow than critical can be achieved. If you are below the choking point, than you should be able to find the pressure with outlet set as "mass flow inlet" with the direction specified as "outward normals". (this is in the density based solver). The problem is that if the restrictor is working as choked, than your mass flow is fixed and the outlet pressure depends on what volume of flow the engine is taking. You should be able also to simulate your critical mass  flow by giving an outlet pressure lower than critical (2-3 times lower than inlet total pressure).

Hope this sounds clear

And sorry for any mistakes was writing by phone.

Cheers, and good luck

Dear Mr.Bartosz Ziegler

I totally agree with you ,even I had used the same process of making the outlet as a mass inlet condition and mentioning the appropriate direction,the mass flow I used was  0.04kg/s which was well below the choking mass flow of 0.073(calculated using the compressible flow equation at NTP) but when the solution was initialised from inlet I got an divergence error,if outlet values were used I got  convergence so I was unsure of how valid the assumption was ,if you could cite an example of where such a method was used it would be of great help ,looking forward for an answer

Cheers! 

note :below is the link for the formula I had used for finding the Choking mass flow 

http://www.grc.nasa.gov/WWW/k-12/airplane/mflchk.html

Dear Anil,

Have you tried the FMG initialization ? I dont have much experience but from what I have experienced, compressible flow solutions are very sensitive to mesh quality and initialization. Performing FMG initialization after standard initialization gives you a coarse "initial solution" from which the solver can start. It often helps to deal with initial instabilities and divergence. It also significantly reduces the number of iterations needed for convergence.  However, FMG sometimes goes wrong way and can lead to very unphysical flowfields, thats why after such initialization, you have to stop the solver and check the flowfield. What is also interesting for me, is why you impose the mass flow. If we are talking about a piston engine with a restrictor on its inlet duct how can you now a mass flow rate? I'm not into piston engines but I belive that both massflow and pressure after restrictor would be a product of inlet parameters (like atmosferic) restrictor and inlet geometry and the volume flow, which is imposed by the engine and relies mainly on displacement, rpm and losses. I dont know what is the aim of your study but I would rather do a characteristic of the restrictor (for example mass flow vs. engine inlet pressure) you could than use two pressure boumdary conditions which from my experience are easier to work with and for me "intuitively more natural". Such characteristic would give you the whole range of mass flows and restrictor downstream pressures which you could then match to the engine rpm range. This still leaves us with an assumption of steady flow which in case of a piston engine inlet is not too suitable.  When it coes to citations I cant think of anything. If I will run into something usefull than I will write again. 

Good luck with your work.

Bartosz.