Learning Forum

[Rashi.Gupta]

I am running a simulation where air ideal gas is passing through tube in CFX. The air ideal gas is selected to account for compressiblity effect. The speed of gas is 100 m/s at inlet. I am getting high mach no. related warning and it is stopping due to floating point error. I have given pressure at outlet around -50 Pa and velocity of 100 m/s at inlet. I have tried same case with giving mass flow rate at inlet but it is calculating a very low velocity and very high density at inlet. How to proceed with this simulation?

[Rob]

Have you checked against any of the tutorials in Help? 

[Mark Owens]

For an ideal gas

density = W*Pabs /(R*T)

where

 

W = molecualr weight

Pabs = absolute Pressure = solver pressure + reference pressure

R = ideal gas constant

T = temperature

 

You should check what reference pressure you have set for the domain.

 

For a velocity inlet both the velocity and temperature is fixed  and only the inlet density (and hence mass flow) will be a function of the solution pressure which will be changing over time to satisfy the boundary conditions. For subsonic flow pressure propagates upstream from the outlet. For a mass flow inlet both the density and velocity  will vary as the solver tries to find a solution. If you cannot get a velocity  inlet to work then it is unlikely that you will get a mass flow inlet to work.

 

In either case you should be able to use the ideal gas formula to check the density. If it is too high it could be because the reference pressure is too high. That might also explain why the velocity inlet is giving wranings about a high mach number since the speed of sound varies inversley with the square root of the density.

[Rashi.Gupta]

One thing I have noticed in this case, the model is not taking -50 Pa static preesure that I am specfying in pre file at outlet, it is showing a value of around 0.2 bar at outlet when I looked in expression (areaAve(Pressure)@outlet). That is the reason solver increased the pressure at inlet and showing high density. Also when I see the contour at outlet for pressure it is showing uniform pressure of -50 Pa. Why the expression value of pressure not matching with what is specified in pre-file?

[Mark Owens]

All CEL expressions use the conservative values of a variable which is the cell value. So areaAve(Pressure)@outlet is the pressure in the cells next to the outlet. If you explicitly want the boundary value use areaAve(Pressure.Boundcon)@outlet see

15.2. Quantitative CEL Functions in Ansys CFX

and

16.1. Hybrid and Conservative Variable Values

[Mark Owens]

PS. The density does not depend proportionatey on the "Pressure" variable. It depends on "Absolute Pressure".

[Rashi.Gupta]

 

I ran the simulation in 2020R2 and when I am using the above mentioned pressure expression, I am getting this error-

Also, the near cell value or conservative value is coming around 0.2 bar and at the boundary I have given -50 Pa. There can be such large difference of 20050 Pa between these value? I am using a refrence pressure of 1 atm.