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

Heat transfer within Porous Media

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

Like Tree2Likes
  • 1 Post By DaveD!
  • 1 Post By Opaque

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   March 26, 2006, 22:41
Default Heat transfer within Porous Media
  #1
Twiti
Guest
 
Posts: n/a
Is that possible to accout for both flow and heat transfer in porous media? I have checked the ANSYS CFX manual and found that the energy equation only take the consideration of fluid (section: ANSYS CFX-Solver, Release 10.0: Theory | Basic Solver Capability Theory | Flow in Porous Media | ). I wonder how can I add the heat transfer from solid framework to fluid flow under the assumption of either thermal equilibrium or non thermal equilibrium.
  Reply With Quote

Old   March 27, 2006, 00:55
Default Re: Heat transfer within Porous Media
  #2
Opaque
Guest
 
Posts: n/a
Dear Twiti,

If you want to do the thermal equilibrium approximation, that is T_solid = T_fluid, you can "fake" the thermal conductivity within the porous domain as

K = (K_fluid * Volume Porosity + K_solid * (1-Volume Porosity)) / Volume Porosity..

That should work..

For the non-thermal equilibrium, the workaround is more elaborate (via additional variables), and you should contact your CFX help desk for details..

Good luck, Opaque..

  Reply With Quote

Old   March 27, 2006, 03:24
Default Re: Heat transfer within Porous Media
  #3
Eugeny Pavlov
Guest
 
Posts: n/a
Yes, this is problem of CFX. I ask my frend in Moskow, and they reply to my -"It is impossible, becouse no contact access to nodal value of function". In STAR-CD this is possible.

Sorry for my english Russia, Syberia, Krasnoyarsk
  Reply With Quote

Old   March 27, 2006, 11:08
Default Re: Heat transfer within Porous Media
  #4
opaque
Guest
 
Posts: n/a
Dear Eugeny,

If your friend is interested in solving a similar problem as Twiti, and has ANSYS CFX 10.0 already, sugggest to contact the CFX help desk.. Help desk can give them a note describing how to solve this issue using Additional Variables.. Requires a bit of a variable substitution for the equations to introduce the solid properties in a fluid equation..

It has been done for steady and transient problems.. You just need to know what the ANSYS CFX solver is doing, to workaround the current limitations.. There is no need to access internal data..

Good luck, Opaque
  Reply With Quote

Old   March 28, 2006, 16:23
Default Re: Heat transfer within Porous Media
  #5
martin
Guest
 
Posts: n/a
the solution is "Diffusive Transport Model" This equation does not compute the convective part. So the quantity is only transported by diffusion and will stay in place.

that's the way I've done:

Add some additional variable(unspecified): cpSolid rhoSolid VSolid ASolid mSolid TSolid kSolid

and AV specific: HSolid

In Fluid Model you can define the values for individual AV eg. (all algrebaic eq): cpSolid=500[W/(m^2*K)] rhoSolid=200[kg/m^3] VSolid=0.1*Volume of Finite Volumes ASolid=200[m^2/m^3]*Volume of Finite Volumes mSolid=VSolid*rhoSolid TSolid=HSolid/(mSolid*cpSolid) cpSolid=1000[J/(kg*K)]

and HSolid as Transport Equation. Kinematic Diffusity is the thermal diffusivity. But as you just want to have it in your subdomain you should define: 2e-4[m^2/s]*Subdomain, so outside the subdomain it is 0.0.

You can't define Diffusive Transport in Pre, so define normal transport and edit the def-file later.

the sources in your subdomain are: for the fluid kSolid*ASolid*(TSolid-Temperature)/Volume of Finite Volumes for the solid kSolid*ASolid*(Temperature-TSolid)* Density

If you expect great gradients it is good to define source coefficients.

that's it. bye martin
  Reply With Quote

Old   March 28, 2006, 16:38
Default Re: Heat transfer within Porous Media
  #6
opaque
Guest
 
Posts: n/a
Dear Martin,

Thanks for the hints, but this applies to the porous domain approximation via Fluid Domain plus a SubDomain.. I think that Twiti wants to use the Porous Domain as in 10.0 (this is a new feature)..

Your approximation does not account for the fact that the solid matrix has a different volume than the fluid part.. Here , the solid and fluid are within the same porous domain. However, the idea is very similar but you must include the Volume Porosity in your terms..

Twiti, you can also pick it up from here.. Good luck, Opaque
  Reply With Quote

Old   November 7, 2015, 10:29
Default
  #7
New Member
 
jogendra pal
Join Date: Oct 2015
Posts: 7
Rep Power: 7
JOGENDRA PAL is on a distinguished road
dear all.. i am facing same problem. can u please tell me how to simulate convection effect of fluid in porous media
JOGENDRA PAL is offline   Reply With Quote

Old   January 14, 2021, 13:27
Default
  #8
New Member
 
Join Date: Feb 2016
Posts: 8
Rep Power: 6
DaveD! is on a distinguished road
Quote:
Originally Posted by Opaque
;75637
Dear Twiti,

If you want to do the thermal equilibrium approximation, that is T_solid = T_fluid, you can "fake" the thermal conductivity within the porous domain as

K = (K_fluid * Volume Porosity + K_solid * (1-Volume Porosity)) / Volume Porosity..

That should work..

For the non-thermal equilibrium, the workaround is more elaborate (via additional variables), and you should contact your CFX help desk for details..

Good luck, Opaque..

Maybe there could be a mistake in Opaque's equation. According to https://www.comsol.com/blogs/thermal...-porous-media/, the equation should read as follows:

K=K_{f}\cdot\theta_{f}+K_{s}\cdot(1-\theta_{f}) where \theta_{f} is the Volume Porosity

Further division by \theta_{f} may be wrong and lead to too high equivalent thermal conductivity.


Edit: Please read further discussion carefully. Obviously, CFD programs differ in the way they modeling the equivalent thermal conductivity.

Last edited by DaveD!; January 15, 2021 at 08:20.
DaveD! is offline   Reply With Quote

Old   January 14, 2021, 15:57
Default
  #9
Senior Member
 
Join Date: Jun 2009
Posts: 1,301
Rep Power: 25
Opaque will become famous soon enough
I advise you to read the ANSYS CFX documentation in detail, read the statement carefully of what "fake" means, and compare the equations.

Comparing Comsol documentation vs another code w/o reading its documentation may lead you to wrong conclusions.

I can still be mistaken, but I welcome you to show me where the mistake is
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.
Opaque is offline   Reply With Quote

Old   January 15, 2021, 08:16
Default
  #10
New Member
 
Join Date: Feb 2016
Posts: 8
Rep Power: 6
DaveD! is on a distinguished road
Hey Opaque,


I've read through the documentations as you recommended and here is what I've found out so far:


Comsol:
\left(\rho C_{p}\right)_{\mathrm{eff}} \frac{\partial T}{\partial t}+\rho_{\mathrm{f}} C_{p, \mathrm{f}} \mathbf{u} \cdot \nabla T+\nabla \cdot\left(-k_{\mathrm{eff}} \nabla T\right)=Q

with the effective volumetric heat capacity

\left(\rho C_{p}\right)_{\mathrm{eff}}=\theta_{\mathrm{s}} \rho_{\mathrm{s}} C_{p, \mathrm{~s}}+\theta_{\mathrm{f}} \rho_{\mathrm{f}} C_{p, \mathrm{f}}

and effective thermal conductivity k_{\mathrm{eff}}

1. Volume average, which symbolically represents solid and fluid stripes in parallel to the heat flux:
k_{\mathrm{eff}}=\theta_{\mathrm{s}} k_{\mathrm{s}}+\theta_{\mathrm{f}} k_{\mathrm{f}}

2. Reciprocal average, for solid and fluid stripes perpendicular to the heat flux:
\frac{1}{k_{\mathrm{eff}}}=\frac{\theta_{\mathrm{s}}}{k_{\mathrm{s}}}+\frac{\theta_{\mathrm{f}}}{k_{\mathrm{f}}}

3. Power law, for a random geometry with similar thermal conductivities for the solid and fluid:
k_{\mathrm{eff}}=k_{\mathrm{s}}^{\theta_{\mathrm{p}}} \cdot k_{\mathrm{f}}^{\theta_{\mathrm{f}}}

with the solid volume fraction \theta_{\mathrm{s}} and the fluid volume fraction \theta_{\mathrm{f}}=1-\theta_{\mathrm{s}}

Source: https://www.comsol.com/blogs/thermal...-porous-media/

Ansys CFX:

\frac{\partial\left(\rho \gamma h_{\mathrm{tot}}\right)}{\partial t}-\frac{\partial p}{\partial t} \gamma+\nabla \cdot\left(\rho \boldsymbol{K} \cdot \boldsymbol{U} h_{\mathrm{tot}}\right)=\nabla \cdot\left(\lambda_{e} \boldsymbol{K} \cdot \nabla T\right)+\nabla \cdot(\boldsymbol{K} \cdot \boldsymbol{U} \cdot \tau)+S_{E} \gamma

where \lambda_e is an effective thermal conductivity and K is a symmetric second rank tensor, called the area porosity tensor.


Ansys Fluent:

\begin{aligned}
\frac{\partial}{\partial t}\left(\gamma \rho_{\mathrm{f}} E_{\mathrm{f}}+(1-\gamma) \rho_{\mathrm{s}} E_{\mathrm{s}}\right) &+\nabla \cdot\left(\vec{v}\left(\rho_{\mathrm{f}} E_{\mathrm{f}}+p\right)\right) \\
&=S_{\mathrm{f}}^{h}+\nabla \cdot\left[k_{\mathrm{eff}} \nabla T-\left(\sum_{i} h_{i} J_{i}\right)+(\bar{\tau} \cdot \vec{v})\right]
\end{aligned}

The effective thermal conductivity in the porous medium, k_{\mathrm{eff}}, is computed by ANSYS Fluent as the volume average of the fluid conductivity and the solid conductivity:

k_{\mathrm{eff}}=\gamma k_{\mathrm{f}}+(1-\gamma) k_{\mathrm{s}}

where

k_{\mathrm{f}} = fluid phase thermal conductivity (including the turbulent contribution, k_{\mathrm{t}})
k_{\mathrm{s}} = solid medium thermal conductivity


So, if in Ansys CFX, \lambda_e is only the sum of the molecular and the turbulent thermal conductivity of the fluid, then you might be right and introducing your "fake" thermal conductivity would lead to canceling of the porosity in the demoniator and in K. Do you have this approach from the Ansys Help Desk? Unfortunately, there are no further information in the CFX Theory Guide than the ones I posted above.
aero_head likes this.

Last edited by DaveD!; January 18, 2021 at 04:55.
DaveD! is offline   Reply With Quote

Old   January 15, 2021, 09:13
Default
  #11
Senior Member
 
Join Date: Jun 2009
Posts: 1,301
Rep Power: 25
Opaque will become famous soon enough
You got it.

For isotropic porosity (default setting), the porosity tensor is diagonal and equal to the volume porosity, Porosity * [I]

No need for the help desk to confirm that.

As you showed the 3 codes are using the same formulation for the diffusion term.
aero_head likes this.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.
Opaque 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
heat transfer to porous media... club68512 FLOW-3D 5 November 4, 2010 00:20
Conjugate heat transfer problem with porous media piko Siemens 1 April 17, 2009 16:41
heat transfer with porous media gokul FLUENT 0 February 24, 2009 14:43
heat transfer in porous media Miko Siemens 5 May 24, 2007 06:12
REG POROUS MEDIA HEAT TRANSFER Rashmi Venkat FLUENT 6 June 1, 2006 06:13


All times are GMT -4. The time now is 18:44.