CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   FLUENT (http://www.cfd-online.com/Forums/fluent/)
-   -   Convergence Problem after considering buoyancy (http://www.cfd-online.com/Forums/fluent/115253-convergence-problem-after-considering-buoyancy.html)

Tarantino March 27, 2013 03:31

Convergence Problem after considering buoyancy
 
Hi!

I am working with air-conditioning system in a room. the inlet flow set as mass-flow-inlet with temperature 20 C (Around 0.3 m/s) and there are several outlets which are set as outflow. the turbulence model in RNG k-epsilon and there are some heat sources in the room. I got a very smooth converge before I add buoyancy force and all the residuals are fall below 1e-4 in first 1000 iteration.
But by adding gravity in (Operation Condition) to impose buoyancy using Boussinesq model, the residuals jump over zero and after so many iterations they don't fall below 1e-1. Actually they become straight. I don't what should I do. Maybe I should assign more accurate numbers for the Operation Pressure, Operation Temperature and Operation Density in Operation condition option.
Does anyone know what is the problem? Should I use Boussinesq in this case or not? Generally, in which cases ones should employ Boussinesq model? How should I find the most accurate values for operating pressure, density and temperature.
Thanks in advance for your help and reply.

oj.bulmer March 27, 2013 07:24

Boussinesq approximation is a faster way to achieve convergence in natural convection, using steady state physics, since the density is constant in all governing equations, except the buoyant term in momentum equations - where it is an empirical function of temperature difference and thermal expansion.

But this only applies when temperature gradients in the room are smaller. You mentioned the heat source, are you sure it is not creating large differences in temperature field throughout the domain?

OJ

Tarantino March 27, 2013 08:09

Hello and thanks for your reply.

I have some people in the room with 100 w/m^2 heat flux. But I am not sure about the amount of temperature differences. I think heat generation by the people in a room cannot generate a very big temperature difference.

oj.bulmer March 27, 2013 08:37

It should not create big differences in temperature. Are you sure you put right thermal expansion factor? Have you tried different turbulence models? Why RNG? I have experienced better convergences with Realizable model. Try using PRESTO scheme, it is reportedly good for natural convection, typically suited for higher Raleigh numbers.

Also, try improving quality of mesh and start with first order schemes till you get adequate reduction in residuals, before switching to second order.

If you see oscillations in residuals, the problem may as well be transient.

OJ

jthiakz March 27, 2013 09:57

"Heat source". you mean to say man continuously add heat to the room.
I thought human body temperature will change with in 2degree C. so in simplified manner it is constant.

Pls correct me if i'm wrong.

Tarantino March 27, 2013 10:34

Hello again.

@ OJ: Well, RNG because it is recommended by several previous publication in the similar cases. I double check the heat fluxes from the persons, and they are assign correctly. Moreover, I run with first order, but I will check Realizable also. It is really strange, because I have no problem before buoyancy driven flow.

@ jthiakz: Usually for simulation human in the room, a sort of a human shape with 1.6 m^2 area and heat flux of 100 w/m^2 considered. the simulation is run in steady state.

kingjewel1 March 27, 2013 10:38

2 things to try:
1: coefficient of pressure =0.7, momentum=0.3 for 1000 iterations then gradually change until you get 0.5 0.5
2: gradually increase gravity from 2.5m/ss to 9.8 m/ss over 5000 iterations.

Some combination of those works eventually.

asal March 27, 2013 10:49

I totally agree with kingjewel1. Impose the gravity gradually rather than all on a sudden. Starting with lower Relaxation factor might work also.

oj.bulmer March 27, 2013 11:07

I mentioned thermal expansion factor because if higher value is mistakenly used, Boussinesq model will not be applicable.

OJ

Tarantino March 27, 2013 14:03

Well, thanks all of you for your answers.

Just a few more questions? Should I use pressure based solver or Density based might work here?
Also I read somewhere about temperature dependent fluid density must be correct when ones want to apply buoyancy, what does it mean and how can I check it?!
Which method for pressure-velocity coupling in the best in this case? PISO, Couple or Simple/SimpleC
Do you recommend to use double precision?
Thanks again.

Lionel Trébuchon April 25, 2014 18:31

Velocity induced by gravity, buoyancy, initialisation
 
Hello!

Thanks a lot for this thread, it was very interesting to read through it. Myself I am modelling high temperature surface buoyancy so I prefer to use k-epsilon as a model. What is your experience with air and surfaces at 1200 [K]?

I have a fast very general question however. I initialise an air-box with gravity in negativ y-direction and entrainments on every face, so basically only an air box, with no energy source whatsoever. Pressure and temperature at entrainments is standard pressure and temperature conditions, as well as the domain initialization and the references.
I immediatly get those velocities (10 iterations). Do you know where it can come from?

Thanks!
Lionel

http://www.trebuchon.com/wp-content/...ty_Capture.jpg

jthiakz April 25, 2014 21:11

mostly because of the domain initialization,but what do you mean by "initialize an air-box with gravity in -ve Y dir"

Lionel Trébuchon April 26, 2014 06:19

Hello thiagu!

This parallelipiped (cube) just is air. All the BCs are the same.
In the buoyant settings, gravity is set with g in the -y direction. You can see the y direction thanks to the triad on the bottom right of the pic.

I didn't initialise no velocities nowhere.
Maybe it is due to the pressures? Ref pressure 1 atm, boundary pressure 1 atm, initialization pressure 1 atm.

If i take the same box and set and inlet flow at the bottom instead of an entrainment ("bottom" is the bottom on the picture) i however have a constant velocity field, with no deceleration. Meaning that the air just flows from bottom to top without effect (what i hoped for in that case.)

What could explain those velocities in the setup shown above? Setup with only entrainments.

Thanks already for the reply.
Friendly greetings,
Lionel

jthiakz April 26, 2014 12:26

is it entertainment with "static pressure" or "opening pressure". It looks like you have used "Entrn. with static pressure" and gravity air flows to bottom side. need to check converged solution.

CFD-fellow April 26, 2014 13:07

Hi
Try double precision for fluent to converge. If it didnt work use SIMPLEC with double precision.
Regards

Lionel Trébuchon April 26, 2014 21:46

Thanks a lot Thiagu and Behroz!

I set the opening pressure as 1 atm. Maybe you are right, actually the pressure that is at 1 atm should be the static one.
But does this explain why, even if every single opening is set the same (as on this cube)l, there is a velocity gradient in the direction of the gravity? I don't manage tu understand.

Thanks a lot!
Lionel


This is just a test set up because I was annoyed by air flows appearing out of ("apparently" - which obviously means "a mistake by the implementer - me in that case") nowhere.
I am using CFX. I don't think that double precision has anything to do with this, it is just a behaviour of fluid flow in cfx. More interesting is that as soon as a little bit of movement is defined somewhere, the effect disappears. But as a matter of fact, I don't want no movement nowhere from wind or other forced factors, and that's why it is disturbing.

CFD-fellow April 27, 2014 01:25

Hi Lionel
My answer was for Tarantino.This Forum is for Fluent Users. I myself am new to CFX. You should post a new thread in CFX forum. Glenn Horrocks is a profession in that forum and can help you.
Regards


All times are GMT -4. The time now is 11:07.