CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   CFX (http://www.cfd-online.com/Forums/cfx/)
-   -   Error in subroutine FNDVAR (http://www.cfd-online.com/Forums/cfx/22849-error-subroutine-fndvar.html)

Mickel July 16, 2006 20:39

Error in subroutine FNDVAR
 
Hello! Does anyone knows how to fix this error or what it refers to? In my problem, there three domains(stator ,rotor,stator).I want to simulation the cavitation phenonmena occured in the rotor domain by selecting two materials. error message: +--------------------------------------------------------------------+ | Reference Pressure Information | +--------------------------------------------------------------------+

Domain Group: R1

Pressure has not been set at any boundary conditions.

The pressure will be set to 0.00000E+00 at the following location:

Domain : R1

Node : 1 (equation 1)

Coordinates : ( 7.35912E-02,-1.25240E-01, 1.33895E-01).

Domain Group: S2

Pressure has not been set at any boundary conditions.

The pressure will be set to 0.00000E+00 at the following location:

Domain : S2

Node : 1 (equation 1)

Coordinates : ( 1.96447E-01, 8.61126E-02, 1.31548E+00). ---------------------------------- Error in subroutine FNDVAR : Error finding variable DENSITY_FL2 GETVAR originally called by subroutine GET_MFLOIP_ZIF .

Thanks in advanced!


Mickel July 16, 2006 20:46

Re: Error in subroutine FNDVAR
 
All domains are at a reference pressure of 1 atm. The boundary conditions are setting with total pressure inlet and mass flow rate outlet

Mike July 17, 2006 08:13

Re: Error in subroutine FNDVAR
 
It looks like it is not setup correctly. Possibly there are no Domain Interfaces? Maybe the fluids are not consistent between the domains? Have you completed the Rotor-Stator and the Cavitation tutorials? Mike

Mickel July 18, 2006 03:42

Re: Error in subroutine FNDVAR
 
Hi Mike.Thanks for your concern. 1.for the first advice: I had checked the out file in the solver manager and got two frozen interfaces and three pair periodic interfaces. 2.the second: in order to shun error for inconsistent materials between the domains, I created a file named cfx5rc.txt. In the txt file, he first line is: "CFX5_NO_CONSTANT_PHYSICS=1", and second line is: "export CFX5_NO_CONSTANT_PHYSICS". Then I copied the file to C:\Documents and Settings\user\.cfx\10.0 for setting up system environment.

3.As you knowed, my simulation resemble the axial Rotor-Stator and the Cavitation tutorials and I had got a lot of good guidance from the two example. I will study them repeatly.


opaque July 18, 2006 08:28

Re: Error in subroutine FNDVAR
 
Dear Mickel,

Using the CFX5_NO_CONSTANT_PHYSICS enviroment is for a case at a time.. As soon as the enviroment is set, some of the physics checking/copying functionality is disabled (not enabled) and physics can become inconsistent across domains, i.e. domain interfaces. That is why is not the default behavior.

Perhaps the fluid on both sides of the domain interface is not the same (in your case), or the physical models are way different..

Good luck, Opaque

Mike July 18, 2006 08:43

Re: Error in subroutine FNDVAR
 
Hi Mickel, you can't have different materials in different connected fluid domains. I expect your stator-rotor-stator are connected fluid domains, so you must have the same materials list in all three. If the fluid domains were isolated from one another (maybe by a CHT solid, or a gap in the computational domain) then you could use different materials. Mike

Mickel July 19, 2006 00:48

Re: Error in subroutine FNDVAR
 
Hi Mike, what the "connected fluid domains" means? Does it mean that CFX can't create interface between stator and rotor for different materials? If it does, then how can I simulate the cavitation phenomena occured in pump with diffuser?

opaque July 19, 2006 08:15

Re: Error in subroutine FNDVAR
 
Dear Mickel,

How would a material change when crossing the rotor-stator interface? Perhaps the definitions of material, fluid and multiphase flow that CFX uses are not clear..

As far as I recall, you need a multiphase setup to run the cavitation model. Therefore, you need two fluids: one of the may not exist (however, it must be defined) until the cavitation region starts to form.

I would contact the CFX help desk and ask for some guidance; otherwise, you may be wasting some of your valuable time.

Good luck,

Opaque


All times are GMT -4. The time now is 15:42.