[enayath]

Hello Folks,

I am running Natural convection by using a 2D axisymmetric case in Fluent. The Rayleigh number is in the range of10^8 to 10^9....

I am wondering if anybody know how to detect the convergence...Any special parameter that I need to track in my simulation to make sure that it converged...The residuals are decreases by the order of 3 in each time step(for continuity and velocity 10^-7 and energy 10^-14)...I also check the Flux report ...it is in order of e-16...as Rayleigh number is high, I do not know that I need to expect the quasisteady situation...I have different contours of velocity at different time steps(I run the case up to 3000s)...is it logic to think that after a certain time I will have similar velocity contours or temperature contours?

I define a couple of nodes and tried to see how the average of velocity in that point in time is changed...there is no good pattern to see that the values are going to be stable around a certain value...

Any idea?

Thank you,
Hooman

[CFD-fellow]

Hi
It somehow depends on your geometry!
Sometimes, in transient and even steady simulation the velocity contours vary with time steps and iterations e.g. Von karmen street in flow over bodies simulations, but drag varies with a same repetitive manner so you can judge convergency.

[enayath]

Behrooz,

Thanks for the reply...I attached the geometry...I am working with Laminar model right now in Fluent...I am not sure that drag is the parameter I should check...Could you please share with me your new understanding as I provided you the geometry ?
On the left and upper hand side, I set isothermal BC(T1) and on right and upper one also isothermal BC(T2)...but T2<T1...and gravity is applied in -x direction. The Fluid domain is surrounded by a solid one and thermal BC are applied on solid domain.

Regards,
Hooman

[CFD-fellow]

No drag isnt proper, it was just an example. what is your time step value? I recommend you first converge a steady run.

[enayath]

Behrooz,

I run the case first in stedy mode for 200,000 iterations. then import the SS results as the initial for the transient calculation. The time step that I use now is 0.01....I checked with 0.1 also and it did not diverge...What do you mean by " first converge a steady run. "?
What criteria do you mean to check in steady run?

Regards,
Hooman

[CFD-fellow]

This is not such a complex setup to have 200000 iterations. Were your residuals descending? were they smaller than 1e-6? I think your geometry should have the same contours.

[ghost82]

Usually when you use laminar model in natural convection problems it's difficult to obtain a steady state solution because of the intrinsic unsteadiness of the problem.
I think you should simulate it with unsteady model, with time step approximatively in the range 0,01 - 0,001 s.
Monitor velocity in some points in your geometry: convergence will be reached if for each time step velocity in that points doesn't change anymore and all residuals are < 10^-4 - 10^-5.

Daniele

[enayath]

Behrooz,

Based on previous works, I need to run my case in transient. I just wanted to have some values for velocity and temperature to accelareat emy transient calculation. In steady calculation, the residual for velocity was almost in order of -2 and energy was -5. when I change to transient mode, they are -6 and -14 respectively.

[enayath]

Daniele,

Thanks for the reply. I created some points and lines in my fluid domain. I checked the maximum and mean value for velocity in some points. there is no sign of convergence...I am wondering the nature of my simulation is not going to reach a stead or quasi steady one...not sure about this...any book title or paper you can suggest me to make sure that I would see steady flow in my transient calculation?

Regards,
Hooman

[CFD-fellow]

Hi Hooman
In my opinion obtaining a steady solution in natural convection is not really difficult, its somehow tricky. Residual 10e-2 is not enough in steady run.
What pressure-velocity coupling do you use?
If SIMPLE, turn into SIMPLEC in steady run and report the result.

[enayath]

Behrooz,

Thanks for the time...

I am running now with simplec...up to now(22000iteration) the residuals are the same as the previous case-simple)...
Based on your comments, I am now thinking about the procedure of my set up in Fluent...I used piecewise-polynomial when I set up the material for my fluid working material. that means K,Cp,density are changing by a function of Temperature...the function is the polynomial and I got the constants of that from NIST. based on this, I did not set operating density in the"cell zone-operating condition"...do you think I need to do that? I did not use boussinesq approximation also...in Fluent user guide 14.5 (page 751),it is mentioned that "if neccesary" use operating density...I have searched in this section on web...did not get a good answer when to use operating density in natural convection...it would be much appreciated if you could share with me your opinions regards to this part of set up...

Regards,
Hooman

[CFD-fellow]

Hi
Dont set operating density, its better to use this in multiphase problem(which is recommended to set operating density to the lower density value). Fluent use average of cell density values by default.
But for your steady run convergency: If you have set gravity value to 9.81, now change it to 0.1 and see if the residuals converge or no. If converge, let it to continue.After good convergency increase the value of gravity acceleration to 9.81 in three or four steps.

[enayath]

Behrooz,

I changed the gravity to 0.1 and then run the case both with simple and simple c...theresiduals are again in order of -2 and -5

Hooman

[CFD-fellow]

Hi
Could you send me your zipped case&data of your steady setup? I sent you my email as private message.

[CFD-fellow]

If I imagine that all of your setup is correct, The only think that I guess is that your flow pattern is not axisymmetric. This happen in natural convection problems when Gr number is critical(Im not expert in its details). Simulate your geometry in 3 dimensions. Check that if you can simulate half of domain and use symmetry boundary condition.

[enayath]

Behrooz,

I am running 3D model, but as it takes too much time... I am trying to find if the axisymmetric model works or not as it takes less time...As I pointed out in the initial questions, the problem that I face now is how to check the convergence criteria in the unsteady calculation...Do you have/know any source/paper/book regards to this topic(critical Gr number)?

I have one more question...in my calculation, when I import my mesh in Fluent, it gives me the error that it is under Y direction but in the design modeler it is correct. I used "trasnfer" option in Fluent to shift the position to the value close to zero(10^-170)...this value is zero but not exactly...Do u think it can affect the results?

Thank you in advance!
Hooman

[CFD-fellow]

Im not sure about its effectiveness.
Look at this paper for axisymmetric flow pattern:
"Axisymmetry breaking instabilities of natural convection in a vertical bridgman growth configuration"