Chemical Vapor Deposition Help

[igergian]

Hi all,

I am very new to Code_Saturne, just a month, and I am trying to implement a case of a chemical vapor deposition reactor. The reactor is tubular with a temperatur profile imposed on the boundaries.
The questions that I have and have not found any informations are
1) How can you define multi-species gas inlet (in my case carrier gas and precursor)
2) How can you define a surface reaction?

Any help or reference would be great. Thank you

[Yvan Fournier]

Hello,

There are very few examples for this, but I attach a setup (using version 2.0) of the "ECHO" test case, which uses a mix of Helium and CO2. In that case, inlets are separate, but this is not essential to the setup.

I will try to add a case description by tomorrow.

To define a surface reaction, I do not know if your reaction is 0D (based on variable values at/near the surface), or if it requires the resolution of a linear system on the whole surface. In the first case, things should be feasible, though you will have to be careful with boundary layer effects. The best would be to look through the code, for examples from specific physics, and I could give you a few pointers to possibly relevant code.

Best regards,

Yvan

[igergian]

Hello and thank you for the immediate response
I believe the first part of multi species inlet is very straightforward and easy to implement.

As for the surface reaction, the equation that calculates the deposition rate (which I want to measure) is based on concentration of precursor and the byproducts of the reaction. The problem that I am thinking of is that if I use the concentration of species which are at the boundary layer cell I am not going to have a surface reaction but volumetric.

Also, is it possible for my case to use the gas combustion module?

Thank you in advance.

[igergian]

Hello again
I have set up a test case where I have 3 species (scalars) that I want them to react by this equation
1 A ----> 0.7 B + 0.3 C (mass fractions)
I am trying to make the surface reaction by creating a flux boundary condition for the scalars.
So, in the inlet I have 10% of species A of the total massflow and 0% of species B and C. On the walls I have put a flux boundary condition as it is shown

call getfbr('31 and x<0', nlelt, lstelt)
!==========
do ilelt = 1, nlelt

ifac = lstelt(ilelt)

! CAUTION: the value of itypfb must be different from
! iparoi, ientre, isymet, isolib, iindef,
! greater than or equal to 1, and
! less than or equal to ntypmx;
! these integers are defined in paramx.h
do iphas = 1, nphas
itypfb(ifac,iphas) = iparoi
enddo

wallflx = 1.8 * 10**-10
! Species1 wall flux
icodcl(ifac,isca(4) ) = 3
rcodcl(ifac,isca(4),1) = 0.
rcodcl(ifac,isca(4),2) = rinfin
rcodcl(ifac,isca(4),3) = wallflx

! Species2 and Species3 wall flux
icodcl(ifac,isca(3) ) = 3
rcodcl(ifac,isca(3),1) = 0.
rcodcl(ifac,isca(3),2) = rinfin
rcodcl(ifac,isca(3),3) = -wallflx * 0.7

icodcl(ifac,isca(2) ) = 3
rcodcl(ifac,isca(2),1) = 0.
rcodcl(ifac,isca(2),2) = rinfin
rcodcl(ifac,isca(2),3) = -wallflx * 0.3

enddo

I also put some monitoring points near the wall and in the outlet but the output files show me that there is no increase in the scalars for species B and C.
Any ideas?

[Yvan Fournier]

Hello,

Your value of base wall flux density seems very small (wallflx = 1.8 * 10**-10), so I would expect the increase in scalars to be very very slow.

Can you test with a higher value (not so high that you crash the calculation, but using a value so that the flux density/(specific heat equivalent * density) is closer to 1 ?

Best regards,

Yvan

[igergian]

Hi again,

as you said I used a greater value 5e-6 and it worked.

Thank you very much

[igergian]

Hi again,

a new problem arise if I want to use this line in the usclim.f90

ATIconc = rtp(iel,isca(2)) * propfb(iel, ipprob(irom))/0.2042668

the error I receive in the compil.log is


ATIconc = rtp(iel,isca(2)) * propfb(iel, ipprob(irom))!/0.2042668
1
Error: Incompatible ranks 0 and 1 in assignment at (1)
gfortran -I/serveurVega/logiciels/saturne/cs-2.0/include -x f95-cpp-input -Wall -Wno-unused -D_CS_LANG_FR -D_CS_FC_HAVE_FLUSH -O -c /home/igergian/tmp_Saturne/3dCVD.FINAL.06051504/src_saturne/usclim.f90
gfortran -I/serveurVega/logiciels/saturne/cs-2.0/include -x f95-cpp-input -Wall -Wno-unused -D_CS_LANG_FR -D_CS_FC_HAVE_FLUSH -O -c /home/igergian/tmp_Saturne/3dCVD.FINAL.06051504/src_saturne/usphyv.f90

Is it impossible to use physical variables in the boundary condition files?

Thank you

[Yvan Fournier]

Hello,

No, you can use physical varibles, but there may be a missing (or an excess) dimension in one of your terms. I would guess at irom(iphas), with iphas = 1.

Starting with version 2.1, iphas has been removed, but in version 2.0, you need to set iphas = 1 and index variables with iphas just about everywhere...

Regards,

Yvan

[igergian]

That was it..
Thank you again