Simulation of an oil flow through a nozzle

JoschJosch Member

Hello,

I want to simulate the oil flow through a nozzle and examine the pressure conditions behind it (Vacuum chambers in the picture).
I use a tetrahedron mesh with inflations at the wall. The Mesh-Quality and the Skewness is good and the y+ is < 1 ( sst k-omega turbulence model is used)
The oil has a constant temperature of 50 degrees celsius

The pressure at the Inlet1 is 3000000 pascal.
The pressure at the Inlet2 is 150000 pascal.
The pressure at the Outlet is 0 pascal (atmospheric pressure)

for a better estimation of the dimensions: The nozzle reduces the diameter from 7mm to 1mm
 


Settings in the "setup": -Pressure-Based Solver
                                     -Steady
                                     -sst k-omega turbulence model
                                     -Energy is off (because of the constant temperature)
                                     -The Solution Methode is "coupled"

My Problems: the calculation does not converge

   


Do I use the right turbulence model?
What can i do to improve the convergence?


Thank you in advance

Comments

  • Kalyan GoparajuKalyan Goparaju Forum Coordinator
    edited May 2019

    Hello, 

    Your setup seems alright to me. Regarding pressure at inlet-1, are you sure it is 3 million pa or was it a typo for 300,000 pa? Also, please note that you are working with gauge pressures by default.

    Do you have pseudo-transient turned on? If so, try decreasing the timescale factor to a smaller number. This usually aids in achieving convergence. 

    Thanks, 

    Kalyan

  • JoschJosch Member
    edited May 2019

    Hello Kalyan,

    Thank you for your Help.
    The gauge pressure at inlet-1 is 3.000.000 pascal it wasn´t a tipo.
    I did not turn on pseudo-transient.
    But I will try it now.

    Thanks

  • JoschJosch Member
    edited May 2019

    When i try to turn the pseudo-transient on with the settings in the following image, the divergence detected in AMG solver: pressure coupled

    What can i do now?

    Thank you in advance

  • Kalyan GoparajuKalyan Goparaju Forum Coordinator
    edited May 2019

    Can you try lowering the under-relaxation values of the variables? Also, reduce the time scale factor to 0.5 may be and give it a shot? Also, while initializing ensure the conditions are reasonable. 

  • JoschJosch Member
    edited May 2019

    I have tried a new Simulation and lower the under-relaxation values of the pressure from 0.5 to 0.4, momentum from 0.5 to 0.4, density from 1 to 0.9, k from 0.75 to 0.5, Dissipation rate from 0.75 to 0.5 and the turbulent viskosity from 1 to 0.9. Furthermore I reduce the time scale factor to 0.5 and the variables converge like this...

    During the initialization i use the values in the following picture.
     
    image">
     
    In the first 30 iterations i get a reverse flow at the pressure inlet and the pressure outlet. Afterwards there were no complications.

    Can I improve convergence even further?
    Or do you think that the results are satisfying?

     

  • Kalyan GoparajuKalyan Goparaju Forum Coordinator
    edited May 2019

    If your inlet pressure is 3million pa and outlet pressure is 300,000 pa, is there a reason for initializing the domain to 50000 pa? Try the hybrid initialization to get better initialization conditions and see if the simulation converges better. To judge if the convergence is satisfactory, please consider having other monitors and checking if their trends saturate

  • JoschJosch Member
    edited May 2019
    Hello,
    by further changing the relaxation values, I have achieved a better convergenz. Thanks for that!!
     


    Now I have a problem with the interpretation of the results.

    If I plot the static pressure on the line which is entered in the picture below, the following values are given to me.
    I do not understand why a negative static pressure can arise there?



     
    and the total pressure looks like this..
     

     

  • JoschJosch Member
    edited May 2019

    To your previous answer:

    I have two inlets. The first pressure inlet with 3 million pa and the second with 150.000 pa. At the pressure outlet 0 Pa.
    I first used the hybrid initalization and got a bad convergence.Then i have used the standard initialization and tried to find suitable values
    for a better convergenz.

  • Kalyan GoparajuKalyan Goparaju Forum Coordinator
    edited May 2019

    Static pressure is also relative to the operating pressure i.e. it is also a gauge pressure. So, a negative value indicates that the pressure in the region is less than operating pressure by that amount

  • JoschJosch Member
    edited May 2019

    Thanks for the answer,
    the operating pressure is 101325 pa.
    Thus, there would still be a negative static pressure.
    However, this is not possible in reality. Therefore I do not know how to interpret this pressure distribution.

    Is this a signal for cavitation?

    What do you think about it?

Sign In or Register to comment.