CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   Phoenics (http://www.cfd-online.com/Forums/phoenics/)
-   -   mass generation with porosity setting (http://www.cfd-online.com/Forums/phoenics/52055-mass-generation-porosity-setting.html)

lily May 2, 2006 11:41

mass generation with porosity setting
 
Hi everyone:

My case is about porous media. I really want to know how to set my porous media with porosity=0.3 and gas generation rate of 1kg/M3*S.

I had set my object attributs with domin material and set its VPOR=0.3, and, use ------ PATCH (SOR ,VOLUME,2,0,0,0,0,0,1,1) COVAL (SOR ,P1 , FIXFLU, 1.0) ----- to set mass generation. But I think that's incorecte because the porosity is not 1,especially on Pressure results.

I need help. thanks

KALI SANJAY May 3, 2006 04:10

Re: mass generation with porosity setting
 
You can use CONPOR command to set porosity over any length of your domain.

for 1-Dimensional problem it can be

CONPOR(SOR,0.3,CELL,1,nx,1,1,1,1)

However you can also use VPOR and check polis for further info...

Your gas generation rate is in Kg/M3*sec... so your Volume in coval is fine....however check your other numbers after volume in patch for the domain you are interested in source term....

PATCH(SOR, VOLUME, IXF, IXL, IYF, IYL, IZF, IZL, ITF, ITL)

IXF is your first node in x direction and IXL is your last node in X direction. Similarly IYX and IYF are first and last nodes in Y direction....if you are solving for 1-Dimensional problem and say you have 10 nodes, the patch command will look like

PATCH(SOR, VOLUME, 1, 10, 1, 1, 1, 1, 1, 1)

I hope your problem is not transient...if it is make argument of patch to LSTEP

Refer Patch command in Polis

Bye:

Sanjay

KALI SANJAY May 3, 2006 04:16

Re: mass generation with porosity setting
 
CONPOR(SOR,0.3,EAST,1,nx,1,1,1,1) use 'east' instead of 'cell'...it works for me and hope it will also for you....!

lily May 3, 2006 11:01

Re: mass generation with porosity setting
 
Thanks for your timely reply Sanjay:) Follow your advise,I changed my porosity setting to CONPOR(SOR,0.3,EAST,1,nx,1,1,1,1) ,and that do work for me:)

But, I am still confused by the mass generation term. As the porous media is not 100% open for flow, I think the result pressure should be diffrent with the situation that media is 30% open for flow. But through experimentations I find the porosity setting didn't affects the pressure results. I don't know why:(


Rami May 4, 2006 03:22

Re: mass generation with porosity setting
 
Lily,

As far as I know, setting the conpor type to EAST rather than CELL is used for prescribing the east face porosity (EPOR) rather than the volume porosity (VPOR), meaning you are defining and solving a different problem.

Settings of porosity has no influence on the pressure unless you explicitly define a resistance model (e.g., Darcy law, Ergun model, etc.) relating the pressure gadient to the velocity. For an explanation of the latter refer to http://www.cham.co.uk/website/new/su...atai/bcsa1.htm

lily May 8, 2006 08:36

Re: mass generation with porosity setting
 
Thanks rami

I have changed the term VPOR to diffrent values but I got same results, but EPOR worked , I don't know why. And, I am still puzzled by Generation source term setting with porous media. I always feel that this term sould be difrrent between situations there 'have' or 'no' porous media. I have define a resistance model, thanks again:)

Kali Sanjay May 9, 2006 13:37

Re: mass generation with porosity setting
 
CONPOR setting for 'EAST' from 1 to NX cells is same as 'EPOR'. CONPOR allows to specify porosity for a particular grids and EPOR is Whole-field store for East face porosity.

Kali Sanjay November 4, 2006 14:01

Re: mass generation with porosity setting
 
Dear Mike, I figured out my problem.....actually when I am giving the migration term as fluxes on east and west walls, I forgot to take in account of effective mobility (which is u/Tortuosity) at the porous/non-porous interface. That's why the flux calculated at the interface from porous side is not the same as flux calculated from non-porous side. This resulted in imbalance. However I would still like your expert coment on the CONPOR implementation. My doubt regarding the actual volume I hope is correct.

Now I want to calculate the velovity field. The problem here is to use superficial velocity. Actually I know the velocity in the porous media (The source of this velocity is due to electroosmosis, a sort of pump inside the porous media). I know the velocity field in the whole domain (actual velocity in the pores and in non-porous medium), I have pressure to atmosphere at the ends. The whole purpose of solving my pressure and velocity equations is to satisfy the continuity equation (as the velocity field I have is sort of function of x, varying). Do I just need to activate DARCY=T and solve the U1? I can just specify the U1 as source term and will solve the Pressure and U1 to satisfy continuity...will it be OK or do I need to do anything else.

Thank you in advance,

Sanjay


All times are GMT -4. The time now is 06:41.