CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > FLUENT

Convergence Problem after considering buoyancy

Register Blogs Members List Search Today's Posts Mark Forums Read

Like Tree5Likes
  • 1 Post By oj.bulmer
  • 2 Post By kingjewel1
  • 1 Post By asal
  • 1 Post By jthiakz

Reply
 
LinkBack Thread Tools Display Modes
Old   March 27, 2013, 02:31
Question Convergence Problem after considering buoyancy
  #1
Member
 
Tarantino
Join Date: Feb 2013
Posts: 34
Rep Power: 4
Tarantino is on a distinguished road
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.
Tarantino is offline   Reply With Quote

Old   March 27, 2013, 06:24
Default
  #2
Senior Member
 
OJ
Join Date: Apr 2012
Location: United Kindom
Posts: 475
Rep Power: 11
oj.bulmer will become famous soon enough
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
oj.bulmer is offline   Reply With Quote

Old   March 27, 2013, 07:09
Default
  #3
Member
 
Tarantino
Join Date: Feb 2013
Posts: 34
Rep Power: 4
Tarantino is on a distinguished road
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.
Tarantino is offline   Reply With Quote

Old   March 27, 2013, 07:37
Default
  #4
Senior Member
 
OJ
Join Date: Apr 2012
Location: United Kindom
Posts: 475
Rep Power: 11
oj.bulmer will become famous soon enough
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
Tarantino likes this.
oj.bulmer is offline   Reply With Quote

Old   March 27, 2013, 08:57
Default
  #5
Member
 
Thiagu
Join Date: Oct 2012
Location: India
Posts: 59
Rep Power: 4
jthiakz is on a distinguished road
"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.
jthiakz is offline   Reply With Quote

Old   March 27, 2013, 09:34
Default
  #6
Member
 
Tarantino
Join Date: Feb 2013
Posts: 34
Rep Power: 4
Tarantino is on a distinguished road
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.
Tarantino is offline   Reply With Quote

Old   March 27, 2013, 09:38
Default
  #7
Senior Member
 
Join Date: Jul 2009
Posts: 211
Rep Power: 9
kingjewel1 is on a distinguished road
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 and Tarantino like this.
kingjewel1 is offline   Reply With Quote

Old   March 27, 2013, 09:49
Default
  #8
Senior Member
 
Astio Lamar
Join Date: May 2012
Location: Pipe
Posts: 154
Rep Power: 5
asal is on a distinguished road
I totally agree with kingjewel1. Impose the gravity gradually rather than all on a sudden. Starting with lower Relaxation factor might work also.
Tarantino likes this.
asal is offline   Reply With Quote

Old   March 27, 2013, 10:07
Default
  #9
Senior Member
 
OJ
Join Date: Apr 2012
Location: United Kindom
Posts: 475
Rep Power: 11
oj.bulmer will become famous soon enough
I mentioned thermal expansion factor because if higher value is mistakenly used, Boussinesq model will not be applicable.

OJ
oj.bulmer is offline   Reply With Quote

Old   March 27, 2013, 13:03
Default
  #10
Member
 
Tarantino
Join Date: Feb 2013
Posts: 34
Rep Power: 4
Tarantino is on a distinguished road
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.

Last edited by Tarantino; March 28, 2013 at 09:16.
Tarantino is offline   Reply With Quote

Old   April 25, 2014, 17:31
Default Velocity induced by gravity, buoyancy, initialisation
  #11
New Member
 
Schweiz
Join Date: Mar 2014
Posts: 16
Rep Power: 3
Lionel Trébuchon is on a distinguished road
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

Lionel Trébuchon is offline   Reply With Quote

Old   April 25, 2014, 20:11
Default
  #12
Member
 
Thiagu
Join Date: Oct 2012
Location: India
Posts: 59
Rep Power: 4
jthiakz is on a distinguished road
mostly because of the domain initialization,but what do you mean by "initialize an air-box with gravity in -ve Y dir"
jthiakz is offline   Reply With Quote

Old   April 26, 2014, 05:19
Default
  #13
New Member
 
Schweiz
Join Date: Mar 2014
Posts: 16
Rep Power: 3
Lionel Trébuchon is on a distinguished road
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
Lionel Trébuchon is offline   Reply With Quote

Old   April 26, 2014, 11:26
Default
  #14
Member
 
Thiagu
Join Date: Oct 2012
Location: India
Posts: 59
Rep Power: 4
jthiakz is on a distinguished road
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.
Lionel Trébuchon likes this.
jthiakz is offline   Reply With Quote

Old   April 26, 2014, 12:07
Default
  #15
Member
 
Behrooz Jamshidi
Join Date: Apr 2013
Posts: 75
Rep Power: 4
CFD-fellow is on a distinguished road
Hi
Try double precision for fluent to converge. If it didnt work use SIMPLEC with double precision.
Regards
CFD-fellow is offline   Reply With Quote

Old   April 26, 2014, 20:46
Default
  #16
New Member
 
Schweiz
Join Date: Mar 2014
Posts: 16
Rep Power: 3
Lionel Trébuchon is on a distinguished road
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.
Lionel Trébuchon is offline   Reply With Quote

Old   April 27, 2014, 00:25
Default
  #17
Member
 
Behrooz Jamshidi
Join Date: Apr 2013
Posts: 75
Rep Power: 4
CFD-fellow is on a distinguished road
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
CFD-fellow is offline   Reply With Quote

Reply

Thread Tools
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
convergence problem commonyue Main CFD Forum 1 December 1, 2009 04:54
Submerged fin, Convergence problem supermouniette FLUENT 10 July 6, 2009 10:47
Convergence of CFX field in FSI analysis nasdak CFX 2 June 29, 2009 01:17
3D Fluid Flow Convergence problem Emily FLUENT 2 March 21, 2007 23:18
Non Convergence of 3D Heat transfer cfd problem Balraj Main CFD Forum 3 December 9, 2004 01:24


All times are GMT -4. The time now is 20:21.