|
[Sponsors] |
How to use CFX own variables in user formulai |
|
LinkBack | Thread Tools | Search this Thread | Display Modes |
June 10, 2019, 12:32 |
How to use CFX own variables in user formulai
|
#1 |
Member
Abdullah Arslan
Join Date: Apr 2019
Posts: 94
Rep Power: 7 |
Hi
I would like to use CFX variables like temperature, density, mass fraction, thermal conductivity. For example, expression is Mass flux=100*T*Random (suppose) T being the temperature at that surface, line or point. So can I write in CEL expression for fluid flux like that at wall (as boundary condition) as it is? e.g. LIBRARY: CEL: EXPRESSIONS: MassFlux=100*T*Random (or 100*temperature*Random) END END END LIBRARY: CEL: EXPRESSIONS: Random=0.00007 [kg m^-2 s^-1 K^-1] END END END and CFX will incorporate temperature into this expression calculated by its solver? Thanx Last edited by Goenitz; June 10, 2019 at 13:57. Reason: explanation |
|
June 10, 2019, 18:49 |
|
#2 |
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,703
Rep Power: 143 |
As long as the units check out CFX will use it. But why didn't you just try this in CFX and find out for yourself?
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum. |
|
June 10, 2019, 20:06 |
|
#3 |
Member
Abdullah Arslan
Join Date: Apr 2019
Posts: 94
Rep Power: 7 |
I tried and Total temperature keep diverging... w/o this boundary condition, simulation works fine. However, it works till 10 iteration so I can see that expression takes T values and increase/decease mass flux at that boundary. But as solution is not converged, so I cannot say definitely.
|
|
June 11, 2019, 07:33 |
|
#4 | |
Member
Abdullah Arslan
Join Date: Apr 2019
Posts: 94
Rep Power: 7 |
Quote:
I took inspiration from tutorial 16 'reacting flow in mixing tube'. It had expressions like this. But I have less faith as when I did tutorial 21 'Combustion in can...', I changed reaction rates to zero but it didn't effect on combustion process. |
||
June 11, 2019, 19:53 |
|
#5 |
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,703
Rep Power: 143 |
Getting CFX to accept an expression and use it is a different thing to it being numerically stable and you being able to get a converged solution. It is hard to see a physical process where the flow rate is proportional to the temperature, and non-physical processes often lead to simulations which do not converge.
So the question is whether the mass flow rate condition you propose is appropriate.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum. |
|
June 12, 2019, 09:24 |
|
#6 | |
Member
Abdullah Arslan
Join Date: Apr 2019
Posts: 94
Rep Power: 7 |
Quote:
I want to set a boundary condition of Temperature on wall. it is ∂T/∂y=-(∑RHi)/λ. (R reaction rate, H enthalpy, λ thermal conductivity, w mass fraction, i specie) λ=∑wi*λi (I have CH4,CO2, H2O,... as species) So i defined the following. ThermCond=CH4.mf*CH4.cond+CO2.mf*CO2.cond+CO.mf*CO .cond+H2.mf*H2.cond+H2O.mf*H2O.cond+N2.mf*N2.cond 1. is that correct way as CFX is not recognising it. 2. How can I assign expression ∂T/∂y on a fixed wall temperature option? is that legit? |
||
June 12, 2019, 13:55 |
|
#7 |
Senior Member
Join Date: Jun 2009
Posts: 1,804
Rep Power: 32 |
It seems you are trying to impose a heat flux proportional to the reaction rate at the boundary, i.e.
q = - k dT/dn @boundary = Sum over i (H_i * R_i) There is no need for the thermal conductivity of the mixture since CFX computes it if needed, neither the temperature gradient. The only time both of those quantities are needed (K and dT/dn) is when backing out the boundary temperature once the equations are solved. On the boundary of interest, select Heat Flux in, set the Heat Flux parameter to an expression equal to the summation on the RHS of the equation above. The solution may tend to diverge if you use a large timescale, so reduce it until it converges. If you are successful at it, let us know. |
|
June 17, 2019, 09:03 |
|
#8 |
Member
Abdullah Arslan
Join Date: Apr 2019
Posts: 94
Rep Power: 7 |
Hi,
No Success yet as there are other problems. But even forcing Flux as your suggested expression, doesn't work. My expression is: LIBRARY: CEL: EXPRESSIONS: Arr= 390 [mol kg^-1 s^-1 Pa^-0.47] Eact = 43200 [J mol^-1] kconst=Arr*((CH4.p)^0.46)*((H2O.p)^0.01) Rate= kconst* e^(-Eact/R/T) END END END Will the above expression capture T and partial pressure or I have to incorporate AreaAve(CH4.p)@Surface? Another things is CH4.p for partial pressure is not recognised by CFX so I use CH4.mf*p for time being. Because Dalton Law says CH4.p=CH4.mol/mol_total*p_total. Going through reference guide, I can say that when user assigns p,T, density etc then these are bulk values. P.S I assigned Sum over i(H_i*R_i) (Sum over=areaAve=sum) but could not succeed. Actually it can operate one variable e.g. sum(p), sum(T) etc Error is: The function 'sum' referenced by parameter 'Heat Flux in' in object '/FLOW:Flow Analysis 1/DOMAIN:Fluid1/BOUNDARY:SinkF1/BOUNDARY CONDITIONS/HEAT TRANSFER' has an invalid argument, 'new'. Only arguments that consist of a single recognised variable name are supported by the solver. Last edited by Goenitz; June 17, 2019 at 11:24. |
|
June 20, 2019, 07:55 |
|
#9 |
Member
Abdullah Arslan
Join Date: Apr 2019
Posts: 94
Rep Power: 7 |
||
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
How to get multiple outputs from CFX user routine | doublestrong | CFX | 7 | April 11, 2017 11:25 |
CFX user ID error. Plz Help. | Zedd | CFX | 1 | March 14, 2017 08:05 |
HELP PLEASE! How to plot Time-Averaged variables in CFX??? | RobBanks | CFX | 7 | September 29, 2016 01:32 |
How to set environmental variables of Intel Fortran +CFX? | Christine MO | CFX | 0 | September 23, 2011 11:11 |
CFX User Subroutine Archive | David Creech | Main CFD Forum | 0 | March 17, 1999 12:41 |