# Boundary condtions, variable temperature and derivative

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

February 14, 2020, 07:49
Boundary condtions, variable temperature and derivative
#1
Member

Abdullah Arslan
Join Date: Apr 2019
Posts: 87
Rep Power: 2
Good day all,

i need to apply this boundary condition on wall.

w_(CH4_wall )=((-Rate×Molar mass) Δy/(ρD_i ))+w_(CH4_fluid )

where w is mass fraction [no unit]
Rate is in mol/m2/s
Δy is derivative distance of wall/fluid transition
D_i is diffusivity coefficient

Preciously, I was putting it as just mass flux [-Rate x Molar mass]. How I can put the above boundary condition? Plus it has no units so as Total source or as Flux, How can I convert above equation?

Similarly, how can I use variable temperature in CFX?
T_wall=((-Rate×Enthalpy) Δy/λ)+T_fluid

λ thermal conductivity
I was using Rate X Enthalpy before as heat flux.

Attached are the boundary conditions and geometry which clears what is Δy.
Does the computed mass fraction near wall is of fluid or of wall (attached image)?

Thank you for your previous help and in advance for future ones.

[For attached image
i is specie variable like CH4, H2
v_i is stochiometric coefficient of reactant'/product"
eff is just effective
ΔT= T_wall - T_fluid
Δw= w_wall - w_fluid
Attached Images
 Paper BCs.png (32.6 KB, 12 views) CH4 mass fraction contour.png (25.9 KB, 13 views)

Last edited by Goenitz; February 14, 2020 at 07:59. Reason: explanation

 February 14, 2020, 09:29 #2 Senior Member   Join Date: Jun 2009 Posts: 1,127 Rep Power: 22 It is always best to understand where that equation is coming from instead of using a discretized version for another method into the software. ANSYS CFX is not a finite difference code, and it is not a cell-centered finite volume code either; therefore, those formulas will only be valid on very specific scenarios. From what I can guess, the formula used to say: Mass Fraction Flux = Rate * Molar Mass where Mass Fraction Flux is given by Mass Fraction Flux = rho * D * grad (Mass Fraction) . Normal Trying to replace a flux condition which depends on the solution (normal gradient) as it converges by a Dirichlet condition is a recipe for convergence problems. In addition, ANSYS CFX only supports "zero flux" conditions on walls. For an accurate representation of non-zero flux condition, or Dirichlet condition on walls, you need to not account for the flux on the equation of interest but also the contributions to the mass conservation and energy equation as well. Recall that the sum of all the species equations add up the mass conservation equation; therefore, the sum of all the fluxes around the boundary better conserve mass either way. __________________ Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.

 February 14, 2020, 10:06 #3 Member   Abdullah Arslan Join Date: Apr 2019 Posts: 87 Rep Power: 2 1. Mass is conserved as species generation and consumption is proportional (conserved) 2. I am using catalyst as Wall and adding sources of heat and mass fluxes. Should I take it as Opening? I will try. 3. Adding sources at wall didn't cause convergence problem but accuracy (80% off than original.), using point 5 equations. 4. I will try to find out how to see if energy is conserved. 5.Mass Fraction Flux = Rate * Molar Mass is coming from some other publication. 6. The equations (in OP) I described above are used in paper for ANSYS CFX 15. 7. Paper link https://www.scopus.com/record/displa...a8ba1432b24f33 8. Can I use variable temperature using CCL or Fortran?

 February 14, 2020, 16:26 #4 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 16,061 Rep Power: 123 You can set a variable to a value using a source term and a source term coefficient: Source term = -C(v-v(setpoint)) Source term coefficient = -C Where v is the variable you are setting (mass fraction, velocity, temperature etc) v(setpoint) is the value you want it to have and C is a large number relative to the variable values, maybe 1E6. That's how you do it. Note you should not have convergence problems or linearisation problems with this approach as it is properly linearised and taken account of in the residuals and imbalances calculations. Whether it is a good idea is another question. __________________ Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.

February 17, 2020, 08:43
#5
Member

Abdullah Arslan
Join Date: Apr 2019
Posts: 87
Rep Power: 2
Quote:
 Originally Posted by ghorrocks You can set a variable to a value using a source term and a source term coefficient: Source term = -C(v-v(setpoint)) Source term coefficient = -C Where v is the variable you are setting (mass fraction, velocity, temperature etc) v(setpoint) is the value you want it to have and C is a large number relative to the variable values, maybe 1E6. That's how you do it. Note you should not have convergence problems or linearisation problems with this approach as it is properly linearised and taken account of in the residuals and imbalances calculations. Whether it is a good idea is another question.
My mixture is multicomponent fluid containing CH4, CO, H2O,H2 and N2. As their component model is "Transport Equation" so they are available as 'sources' under 'boundary sources'. However, they can only be added as Flux (Quantity*kg/m2/s) or as Total Source (Quantity*kg/s).

This is also true if I define my own variable and use "Transport equation" or "Diffusive Transport Equation". So basically, I cannot use Temperature unless I multiply it with Flux or Total Source (which I don't know how as wall velocity is zero).

The source coefficient appears, when I use subdomain. However, my reaction is surface reaction. So 'Flux Coefficient' or 'Total source coefficient' is available.

There is another option adding 'Source point', which requires adding sources at certain user points. But my geometry is too big for that.
Attached Images
 Sources under boundary sources at boundary (wall).png (21.4 KB, 4 views) Subdomain sources.png (22.0 KB, 4 views)

 February 17, 2020, 09:20 Differential #6 Member   Abdullah Arslan Join Date: Apr 2019 Posts: 87 Rep Power: 2 For the expression ΔT/Δy= -Rate×Enthalpy/λ some authors used -Rate×Enthalpy as Flux (makes sense as we just taking λ to LHS of equation) and some used T_wall=((-Rate×Enthalpy) Δy/λ)+T_fluid where ΔT=T_wall - T_fluid I guess T_fluid is T in ANSYS CFX-Pre. But how can I determine Δy which I think is distance between boundary cells and boundary? For now I am just taking 300th of channel height.

 February 17, 2020, 09:48 #7 Senior Member   Join Date: Jun 2009 Posts: 1,127 Rep Power: 22 Would you mind pointing to the publication you are using? Something is off for the energy equation boundary condition. The boundary condition for heat transfer at a catalytic wall is not trivial, and definitely not just a flux formula. Boundary energy flux = conductive flux + "radiation flux if active" + "energy release if catalytic" Then, you pick the option for your boundary energy flux: flux specified? Temperature specified? Transfer coefficient? and solve for which temperature value the wall should have. If the wall is catalytic, there is no way to know the temperature at the wall ahead of time unless you are modeling some other physics outside that can be represented as an isothermal wall (say phase change for example). __________________ Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.

February 17, 2020, 10:30
#8
Member

Abdullah Arslan
Join Date: Apr 2019
Posts: 87
Rep Power: 2
Quote:
 Originally Posted by Opaque Would you mind pointing to the publication you are using?
This is the paper which uses in their own code T_wall function
https://www.sciencedirect.com/scienc...96890418310343

This is the paper who uses ANSYS CFX11 but didn't tell how they put boundary conditions
https://www.scopus.com/record/displa...a8ba1432b24f33

This is the paper which uses more or less same condition and equation and uses fluxes for mass and energy
https://www.sciencedirect.com/scienc...60319918329045

No radiation, NO CONDUCTION in wall but heat transfer occurs between gas and wall. Though no HTC is given, but gas λ.
Also no temperature or flux or HT coefficient is specified. Wall Temperature is given as function of rate, SMR enthalpy and thermal conductivity. rate depends upon partial pressure and temperature of gas.

February 17, 2020, 11:14
#9
Senior Member

Join Date: Jun 2009
Posts: 1,127
Rep Power: 22
This link seems to be incomplete

Quote:
 Originally Posted by Goenitz This is the paper who uses ANSYS CFX11 but didn't tell how they put boundary conditions https://www.scopus.com/record/displa...a8ba1432b24f33
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.

February 17, 2020, 11:23
#10
Member

Abdullah Arslan
Join Date: Apr 2019
Posts: 87
Rep Power: 2
Quote:
 Originally Posted by Opaque This link seems to be incomplete
this is working
https://www.jstage.jst.go.jp/article...7_633/_article

February 17, 2020, 17:17
#12
Super Moderator

Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 16,061
Rep Power: 123
Quote:
 My mixture is multicomponent fluid containing CH4, CO, H2O,H2 and N2. As their component model is "Transport Equation" so they are available as 'sources' under 'boundary sources'. However, they can only be added as Flux (Quantity*kg/m2/s) or as Total Source (Quantity*kg/s).
The source term I was talking about is a total source and you set the units of the term C to suit.

And of course, Opaque's comments about the underlying physics you are trying to implement are important as well.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.

February 24, 2020, 07:32
#13
Member

Abdullah Arslan
Join Date: Apr 2019
Posts: 87
Rep Power: 2
Quote:
Thank you for the detailed reply. I was going through (for past week) it and thought in CFX, may be I have to add sources in continuity equation. However, it acts like an inlet with mass flow rate, velocity and temperature along species in/out fractions. Here I could set both mass fractions and variable temperature as it is (without any gradient or flux terms, so that was success at least).

Anyway, I found out that Stefan velocity vanishes at steady state, and my reaction is steady state reaction from beginning.

Regards