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

Natural convection regime in a small cavity

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

Like Tree4Likes
  • 2 Post By vinerm
  • 1 Post By vinerm
  • 1 Post By vinerm

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   April 29, 2020, 10:57
Default Natural convection regime in a small cavity
  #1
Member
 
Antonio
Join Date: Nov 2016
Posts: 36
Rep Power: 8
AntonioDesah is on a distinguished road
Hi all.

Trying to study the behavior of a fridge in natural convection regime. I have simplified a lot the problem, to understand if my model works but it seems not to. The cavity is very small 60cmx100cm and the flow is steady. I set up a density based model, activated the energy equation and set up the gravity along the y axes with negative value. I have used a laminar model and a k-omega standard but the results are very poor, although my mesh quality is correct. I am pretty sure that I am missing something in the B.C or reference value. The rear vertical is set with 277 K and zero heat flux. The other three walls are at the same temperature of 300K and thermal insulated as well. I would expect a contour of temperature as evidence of natural convection motion but none of this happened. The model has converged on 10E-5 values of the residuals after 10k iterations. Any help? Thanks in advance for any reply.

[IMG] https://ibb.co/Fz6NVLV [/IMG] mesh

[IMG] https://ibb.co/gyLbw6y [/IMG] Velocity contours for K-omega standard

[IMG] https://ibb.co/Pg5Tp2G [/IMG] Static temperature
AntonioDesah is offline   Reply With Quote

Old   April 29, 2020, 12:50
Default Natural Convection
  #2
Senior Member
 
vinerm's Avatar
 
Vinerm
Join Date: Jun 2009
Location: Nederland
Posts: 2,946
Blog Entries: 1
Rep Power: 34
vinerm will become famous soon enough
Natural convection requires two things - gravity and variation in the material density. You have included the gravity. But as far as density is concerned, you have to use some appropriate model to define Material Density. By density method you have mentioned, I suppose you mean the solver option under General. That's not required nor should it be used for such a scenario. So, keep it pressure based. For the density of material, you can either use Incompressible Ideal Gas or Boussinesq or Ideal Gas. But just by using one of these methods will not lead to a flow. Material density based on one of these models do not mean variation in the density; it only means that the variation is allowed. But for the variation to exist, either the temperature and/or the pressure (for the ideal-gas) have to change. You appear to have no temperature variation in the cavity in the vertical direction. In a direct cool refrigerator, evaporator is at the top; so there is a lower temperature at the top and a higher temperature at the bottom leading to natural convection. You have to apply some appropriate boundary conditions on the boundaries. Reference values do not affect the solution so you can neglect those.

And 60cmx100cm is not a small cavity; it is big enough for turbulence to exist. So, include turbulence model. Laminar will not converge.
AntonioDesah and mikulo like this.
__________________
Regards,
Vinerm

PM to be used if and only if you do not want something to be shared publicly. PM is considered to be of the least priority.
vinerm is offline   Reply With Quote

Old   April 29, 2020, 13:33
Default
  #3
Member
 
Antonio
Join Date: Nov 2016
Posts: 36
Rep Power: 8
AntonioDesah is on a distinguished road
Quote:
Originally Posted by vinerm View Post
Natural convection requires two things - gravity and variation in the material density. You have included the gravity. But as far as density is concerned, you have to use some appropriate model to define Material Density. By density method you have mentioned, I suppose you mean the solver option under General. That's not required nor should it be used for such a scenario. So, keep it pressure based. For the density of material, you can either use Incompressible Ideal Gas or Boussinesq or Ideal Gas. But just by using one of these methods will not lead to a flow. Material density based on one of these models do not mean variation in the density; it only means that the variation is allowed. But for the variation to exist, either the temperature and/or the pressure (for the ideal-gas) have to change. You appear to have no temperature variation in the cavity in the vertical direction. In a direct cool refrigerator, evaporator is at the top; so there is a lower temperature at the top and a higher temperature at the bottom leading to natural convection. You have to apply some appropriate boundary conditions on the boundaries. Reference values do not affect the solution so you can neglect those.

And 60cmx100cm is not a small cavity; it is big enough for turbulence to exist. So, include turbulence model. Laminar will not converge.
Thank you so much for your reply.

I changed into density base solver ( I know it is used for compressible flow) but the concept behind is that natural convection is based on difference in density, that's why I have used this. Is it completely wrong ?

Furthermore, I have designed the model in that way, with the cooler wall as vertical because I thought that the heat exchange was behind the fridge. Shouldn't the model working with a gradient of temperature along the x axes anyways? I mean, is it physically possible? I thought so.


The images I posted, refers to a model which has converged under 10E-4 residuals, quite fast with K-Omega standard and laminar. I used laminar because the flow is steady with 0 initial velocity.


Also, Before reading your comment I did the following :

I changed the density under material with variation according to boussinesq approximation, with initial value 1.225kg/m3.

Therefore, I have a density allowed to change and a different temperature among the different walls. The model under these conditions do not work at all. Natural convective motions do not initiate at all.

B.C. : For the horizontal wall and one of the vertical, I treated them as thermal insulted with an heat flux equal to zero. The cooler wall I used the temperature set to 277K ( 4 degrees C). I believe that the B.C. associated to the cooler wall has to be convection but I am not sure about the value of the heat flux to assign as input. I gave it a try setting the cool wall with just temperature.

Where do you think I am wrong ?

Also, this project is part of a wider project, aiming to study the increment of the temperature with respect to time, once the door is open, as transient, starting from a natural convection regime inside the fridge and inside the room where the fridge is located. Does this approach make sense ?

Thanks in advance for your help!!!
AntonioDesah is offline   Reply With Quote

Old   April 29, 2020, 14:02
Default Suggestions
  #4
Senior Member
 
vinerm's Avatar
 
Vinerm
Join Date: Jun 2009
Location: Nederland
Posts: 2,946
Blog Entries: 1
Rep Power: 34
vinerm will become famous soon enough
Density based solver is meant for high Mach flows with Mach > 2. Compressibility starts at as low as Mach 0.3. So, use pressure based solver; doesn't matter whether the fluid is incompressible or compressible.

Temperature difference in a horizontal plane will not cause any flow; there will be heat flow but only because of diffusion. Flow can set up only if you use ideal gas because in that case colder column will end up being heavier than the hotter column but with Boussinesq or Incompressible Ideal Gas, you won't observe any flow.

Case converges faster because there is nothing to converge to; initial condition of 0 velocity is the final solution. So, the solution is already converged. Initial velocity 0 does not imply that flow will be laminar once the convection has begun.

Boussinesq model does not allow density change, it keeps the density of the material constant; however, it allows effects of density change on the flow. But it requires further setup. You have to setup Boussinesq temperature and an operating density equal to material density in the Operating Conditions Panel. Initialize with 0 velocity and temperature of 300 K or some other value higher or lower than 277 K, which you are using for your wall. Do note that there should be some positive value provided for Volumetric Expansion Coefficient in the Materials panel for air. Else, there won't be any natural convection.

It appears you are trying to simulation soaking period of refrigerator. If that is the case, many researchers have worked on it and there should be a ton of material available online. But it won't work with Boussinesq since room is usually very hot and humid for Boussinesq to be valid.
AntonioDesah likes this.
__________________
Regards,
Vinerm

PM to be used if and only if you do not want something to be shared publicly. PM is considered to be of the least priority.
vinerm is offline   Reply With Quote

Old   April 30, 2020, 13:18
Default
  #5
Member
 
Antonio
Join Date: Nov 2016
Posts: 36
Rep Power: 8
AntonioDesah is on a distinguished road
Once again, thanks a lot for your help.

Quote:
Originally Posted by vinerm View Post

Temperature difference in a horizontal plane will not cause any flow; there will be heat flow but only because of diffusion. Flow can set up only if you use ideal gas because in that case colder column will end up being heavier than the hotter column but with Boussinesq or Incompressible Ideal Gas, you won't observe any flow.
Diffusion would be still part of the natural convection, wouldn't it? I thought that being a relative small cavity, the boundary layers would have mixed with a consequent velocity gradient along the horizontal axes as well. The solution of the NS would still have 2 components no? Probably, I am a bit confused here.

Quote:
Boussinesq model does not allow density change, it keeps the density of the material constant; however, it allows effects of density change on the flow. But it requires further setup. You have to setup Boussinesq temperature and an operating density equal to material density in the Operating Conditions Panel. Initialize with 0 velocity and temperature of 300 K or some other value higher or lower than 277 K, which you are using for your wall. Do note that there should be some positive value provided for Volumetric Expansion Coefficient in the Materials panel for air. Else, there won't be any natural convection.
I have tried the following set up with a consequent change of mesh:

Cell Zone Material: Fluid air, density variation with Boussinesq approximation with a value of density of reference of air in standard condition 1.224kg/m3 I did not get the meaning of associating the density of the air with the density of the material( as reference value), which in my case would be aluminium
Top horizontal wall: Thermal B.C. Temperature 277 K according to Ansys manual, in presence of a natural convection I have to consider convective b.c. but I am not sure about the heat transfer coefficient.

All other walls: Thermal B.C. Temperature 300K.

Reference Value: T= 300k V=0

Turbulence model k-omega standard.

Results: The results are attached. I was not able to reach the convergence after 20k iteractions nor a kind of stability of the variables. I attach the result related to Velocity, Temperature.

Where could the error could be ?


Quote:
It appears you are trying to simulation soaking period of refrigerator. If that is the case, many researchers have worked on it and there should be a ton of material available online. But it won't work with Boussinesq since room is usually very hot and humid for Boussinesq to be valid.
Which model should I use and what kind of B.C. shall I assign to one of the vertical walls to behave like a door opening? I was thinking about open b.c. in order to allow the flow in and out once the door opens, but it is a field Ive never ventured. Any suggestion?
Attached Images
File Type: jpg vel1.jpg (37.1 KB, 11 views)
File Type: jpg temp1.jpg (25.4 KB, 8 views)
File Type: jpg residuals.jpg (79.9 KB, 8 views)
File Type: png mesh1.png (14.9 KB, 11 views)
AntonioDesah is offline   Reply With Quote

Old   April 30, 2020, 15:26
Default Diffusion and Setup
  #6
Senior Member
 
vinerm's Avatar
 
Vinerm
Join Date: Jun 2009
Location: Nederland
Posts: 2,946
Blog Entries: 1
Rep Power: 34
vinerm will become famous soon enough
As long as there is a positive diffusion coefficient and/or turbulence and spatial gradient in the field, there is diffusion. However, the existence of flow depends on a driving force, which could be buoyancy or some other body force. In the case of natural convection, it is buoyancy. Solution of NS has three velocity components and one pressure value.

Where did you read the statement associating the density of the air with the density of the material( as reference value)? The natural convection term in manual is implied for the conditions outside the wall and not inside, i.e., the domain being solved. So, you can safely apply either temperature or a convection coefficient of 5-10 with temperature of 310 - 320 K depending upon the temperature in the room. 5-10 is the range for natural convection.

For setting up a case using Boussinesq, here is the minimum requirement

1. Provide a constant value of density in Materials Panel. Usually, whenever Boussinesq is chosen, value is changed to 0. User need to provide appropriate value. Same value of density must be used for the Operating Density in the Operating Conditions panel

2. Provide a positive value of volumetric expansion coefficient in the Materials panel. This will appear only after Boussinesq has been selected for density

3. Provide an average temperature as the Boussinesq Temperature under the Operating Conditions panel. Ideally, this Operating Density (as well as Material Density) should be corresponding to this temperature. Use a temperature of 290 or 293, average of minimum and maximum of your domain, which are 277 and 300.

4. Enable gravity in correct direction.

5. Initialize with all velocities 0 and a temperature value between 277 and 300.

Run with first-order and Coupled Pseudo-Transient method for first 200-500 iterations. Then, if you observe that the residuals are stable, change all discretization schemes to second-order. You may require up to a maximum of 10000 iterations. If you do not get very stable solution even after 2000 iterations, then it is not going to stabilize after 10000 as well.
AntonioDesah likes this.
__________________
Regards,
Vinerm

PM to be used if and only if you do not want something to be shared publicly. PM is considered to be of the least priority.
vinerm is offline   Reply With Quote

Old   May 4, 2020, 10:35
Default
  #7
Member
 
Antonio
Join Date: Nov 2016
Posts: 36
Rep Power: 8
AntonioDesah is on a distinguished road
Dear Vinerm

Sorry for the delay in the answer but I was busy with something else.First all thank you very much for your availability and also please accept my apologies. I did not want to argue with you about the heat flux. I can see you have much more experience than me in this kind of simulations. I was only trying to find a mathematical explanation of the predominance of the diffusion. Of course natural convection is driven by buoyancy force but I could not see how a vertical plate colder respect to the other walls could not generate any motion.

Nevertheless, I have followed your instruction. I set the value of the Boussinesq density as 1.225kg/m3. Then a coefficient of volumetric expansion of 0.0034. I have also set temperature of 290 under operating condition and I set up the same density of Boussinesq. all the walls are set up with temperature as thermal b.c. I initialize all the zone with zero velocity and Temperature of 290( although the value was coming automatically). Also set up all the methods to first order with pressure on PRESTO!, as per ansys manual.

I also set up a time step of 0.001 for for 250 time steps. The shape of the curve of the residuals is periodic, not constant but stable.

After 500 iterations, I switched to steady again, and run the simulation as pseudo transient. As soon as I launch the calculations the error of floating point exception pops up. Any other suggestion ?Thanks in advance for any reply!
AntonioDesah is offline   Reply With Quote

Old   May 5, 2020, 08:48
Default Natural Convection
  #8
Senior Member
 
vinerm's Avatar
 
Vinerm
Join Date: Jun 2009
Location: Nederland
Posts: 2,946
Blog Entries: 1
Rep Power: 34
vinerm will become famous soon enough
You don't have to be apologetic nor were we arguing.

A closed cavity using Boussinesq usually requires transient simulation. Steady-state may work with low values of URF. However, do ensure that you are using Fluent in double-precision. With single-precision, you will get floating-point error.
__________________
Regards,
Vinerm

PM to be used if and only if you do not want something to be shared publicly. PM is considered to be of the least priority.
vinerm is offline   Reply With Quote

Reply

Thread Tools Search this Thread
Search this Thread:

Advanced Search
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 Off
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
yPlus value in internal flow (natural convection in cavity) tarunw OpenFOAM Running, Solving & CFD 0 January 26, 2017 10:07
Thermophysical properties for natural convection Ciefdi OpenFOAM Running, Solving & CFD 0 November 7, 2013 12:44
Radiative heat transfer with natural convection inside a square cavity msarkar OpenFOAM 1 January 11, 2010 23:21
Natural convection - Inlet boundary condition max91 CFX 1 July 29, 2008 21:28
Instability at the onset of natural convection Magherbi Main CFD Forum 0 October 23, 2002 10:53


All times are GMT -4. The time now is 08:47.