CEL and Variables
I'm working with CEL in Pre.
Usually you need to evaluate areaAve(<variable>)@Plane and it works. I tried areaAve(<variable1> * <variable2>)@Plane and it doesn't work......anyone knows why?!?! e.g. areaAve(p)@inlet > OK areaAve(p*T)@inlet > PROBLEMS!!!! 
Re: CEL and Variables
Hi,
Are you using CFX5.7?In Post, <font color="blue">function(variable1*variable2)@locator </font> doesn't work in version 5.7, but it works in versions 5.6 and 5.7.1.So, the same may happen in Pre. Regards, Rui 
Re: CEL and Variables
try this: PT=p*T areaAve(PT)@inlet

Re: CEL and Variables
Unfortunately, the expressions within callbacks is not supported within CFXPre and CFXSolver.
However, there is a workaround. Create an Algebraic Equation Additional Variable equal to your expression, and apply the callback function on this new variable. Good luck, Juan Carlos 
Re: CEL and Variables
I use 5.6 version!

Re: CEL and Variables
Already done. It doesn't work :(

Re: CEL and Variables
Thanks for the good idea. I tried:
LIBRARY: ADDITIONAL VARIABLE: dummy Option = Algebraic Equation Additional Variable Value = 2 * T Units = [ K ] Variable Type = Unspecified END # ADDITIONAL VARIABLE:dummy END # LIBRARY: just to try a dummy variable ( 2 * temperature) , but when I call the variable in the expression editor (e.g.: dummyAVE = areaAve(dummy)@Plane1) I've no problems. The problem is in the SOLVER, because it writes: "Error in setting: "dummyAVE" via the expression: areaAve(dummy)@Plane1 areaAve( : read successfully, and then error found at item: dummy unrecognised name Error processing expression: Expression Value = dummyAVE" Moreover in PRE, rightclicking in the expression editor I cannot find "dummy" in the variable list after I've created....how it is possible Juan? many thanks. 
Re: CEL and Variables
errata corrige: Now I find the additional variable "dummy" rightclicking in the expression editor.......but the solver don't want to recognize it....

Re: CEL and Variables
Hi,
Usually I create additional variables.For example, in CFXPre I create a new variable Source heat set the type to Unspecified and the units to [J m^3 s^1], I create an expression Sq, and when I define the Domain, in the Fluid Models tab I select the variable Source heat chose the option Algebaric Equation and set it to expression Sq. And in CFX5.6 the .ccl and the .out files are like this (which looks a little bit different from what you posted): LIBRARY : ADDITIONAL VARIABLE : Source heat Option = Definition Units = [ J m^3 s^1 ] Variable Type = Unspecified END ..... ..... CEL : EXPRESSIONS : ..... ..... Sq = Hr*Km*(Co^2)*(1alfa)^2 ..... ..... END END END FLOW : ..... ..... DOMAIN : Domain 1 ..... ..... FLUID MODELS : ..... ..... ADDITIONAL VARIABLE : Source heat Additional Variable Value = Sq Option = Algebraic Equation END END END ..... ..... ENDRegards, Rui 
Re: CEL and Variables
Many thanks Rui, but it seems that in CFXPre is impossible to evaluate a areaAve (or areaInt) of a composite variable...I will try...

Re: CEL and Variables
Hi,
I just repeated your example above, and it works for me.. Are you sure there isn't a typo that we cannot see because of the html? Is Plane 1 a boundary condition location? The CFX solver only supports callback on location that are either boundaries, subdomain, domain, monitor points or source points. Plane 1 sounds like a user defined location in the middle of a domain. Good luck, Juan Carlos 
Re: CEL and Variables
no, plane1 is a periodic boundary.
The methodology you suggest works for entities like density, temperature, but I tried with velocity and in that case the solver write "Details of error:  Error detected by routine PEEKCA CDANAM = /FLOW/GETVAR/MESH_DIR/CZIF CRESLT = NONE ++  Writing crash recovery file  ++ ++  ERROR #001100279 has occurred in subroutine ErrAction.   Message:   Stopped in routine MEMERR            ++ My problem is that I would like to write an expression of the moment source in function of the areaAve(density* vel) 
Re: CEL and Variables
Stex,
density * vel is a vector and you are using a Algebraic scalar equation. It is not what you want, I believe. Have you tried using the velocity components as  Av expression 1= density*u  Av expression 2= density*v  ... and use them individually in the momemtum source.. I am guessing here since I do not know what you are trying to do.. Perhaps the callback function are not fully supported on periodic domain interfaces..Have you tried using on WALL or INLET, just to verify your syntax is correct. Are you using 5.7.1 or 5.6? I would not continue unless you check with support and they confirm it should work on either of them. Regards, Juan Carlos 
Re: CEL and Variables
Dear Juan, now I can explain.......I did many tests. So,let's try a simple case, you can try by yourself if you don't believe me.
if you define in Pre an expression as areaAve(u)@Periodic_boundary ....it works. if you define a additional variable u_new with an algebraic equation u_new = u and then you change the expression like this... areaAve(u_new)@Periodic_boundary ....it doesn't works. Why is not possible?? 
Re: CEL and Variables
Hi Stex,
I have tried in CFX5.6: areaAve(T)@boundary and areaAve(u)@boundary work for all type of boundaries Variable T_new = T, areaAve(T_new) works for all type of boundaries Variable u_new = u, areaAve(u_new) works for all type of boundaries <u>except periodic boundaries</u>. I got the same error as you: Error detected by routine PEEKCA CDANAM = /FLOW/GETVAR/MESH_DIR/CZIF CRESLT = NONE I tried in CFX5.7.1 (with SP1): Variable u_new = u, areaAve(u_new) works for <u>all type of boundaries</u>. So it seems it was some problem that has been fixed in CFX5.7. Regards, Rui 
Re: CEL and Variables
In fact I use 5.6, and I just finish to try all the variables and boundary as you did. Thanks for all your kindness. I hope we will keep in contact.
stpieri@units.it Regards 
Re: CEL and Variables
PS: Rui, have you ever find a way to calculate massFLOW in a periodic boundary???
Thanks 
Re: CEL and Variables
Ciau Stex,
In both CFX5.6 and 5.7.1, when calculating massFlow()@inter Side1 Boundary1 (inter was defined as a Periodic Domain Interface), I got this error message:ERROR #001100279 has occurred in subroutine ErrAction. Message: An invalid request to calculate IP mass flows was found for the s ymmetry or periodic boundary named: inter Side1 Boundary1However, in CFX5.7.1 it's possible to calculate massFlowInt(var)@inter Side1 Boundary1 and massFlowAve(var)@inter Side1 Boundary1, while in CFX5.6 it isn't. To calculate the mass flow a this boundary, in CFX5.7 you can do something like areaInt(Density * Velocity dot n)@Periodic_boundary, where n is the outward normal vector. If the boundary is perpendicular to the xaxis, the mass flow would be areaInt(Density * u)@Periodic_boundary.If your fluid density is constant, in CFX5.6 you can create an expression to calculate the volume flow as Vflow = areaInt(u)@Periodic_boundary, and create another expression to calculate the mass flow as Mflow = Vflow * Density. But if the fluid density isn't constant, it seems there is no way to calculate the mass flow at a periodic boundary. But I think you should contact the CFX support and ask them how to have the mass flow through a periodic boundary available at the Solver. Regards, Rui 
Re: CEL and Variables
"ERROR #001100279 has occurred in subroutine ErrAction."
Yes, I know this ERROR... Now I've just installed 5.7 ....so right now I can calculate the massFlowAve(Temperature)@Periodic_boundary and I'm really happy about it....... I've got the last problem with the mass flow....infact I defined a Den_U=density*u variable, but I' ve the same error when I evaluate the areaInt(Den_U)@Periodic_boundary so (as you suggested) the solution is to setup a constant density and calculate the areaInt(u)@Periodic_boundary. This solution works, but is not really what I want...so I will contact CFX support. Thanks. 
All times are GMT 4. The time now is 11:03. 