[Pumba]

Hey guys,

i'm trying to make my own drag model for a multiphase application with varying morphology.

Anyhow, i need the cell volume, so i used the 'volcvol' variable in one of my equations for the drag. This leads to the following error:

 ======================================================================
 OUTER LOOP ITERATION =    1                    CPU SECONDS = 3.844E+01
 ----------------------------------------------------------------------
 |       Equation       | Rate | RMS Res | Max Res |  Linear Solution |
 +----------------------+------+---------+---------+------------------+
 | Wallscale-Bulk       | 0.00 | 1.9E-06 | 4.5E-04 | 10.3  3.0E-02  OK|
 +----------------------+------+---------+---------+------------------+
 ----------------------------------
 Error in subroutine  cal_CVVOL :
 Error calculating control volume volumes
 GETVAR originally called by subroutine  cal_CAB_MOM
 
 +--------------------------------------------------------------------+
 | ERROR #001100279 has occurred in subroutine ErrAction.             |
 | Message:                                                           |
 | Stopped in routine GV_ERROR                                        |
 |                                                                    |
 |                                                                    |
 |                                                                    |
 |                                                                    |
 |                                                                    |
 +--------------------------------------------------------------------+

I'm using volcvol for the damping of the turbulence at the free surface as well and it works fine there. Is there some workaround for this?

I have no experience with user fortran at all, so i'm using only CEL for my model.

[Opaque]

If you look at the discretization theory for ANSYS CFX, the source terms are evaluated on the sector of the elements of the mesh, not on the control volumes.

The variable volume of control volumes cannot be used for expressions that are evaluated on elements of the mesh.

It is odd (to me) a source term is a function of the mesh size. Wonder if there is a confusion on how the source terms are implemented.

Hope the above helps,

[Pumba]

Yes, you are correct, i actually got a response from the ANSYS Support today. It's necessary to add an algebraic additional variable for volcvol. But it only works if you add "Under Relaxation Factor = 1.0" in the CCL of the AV.
This additional variable interpolates volcvol onto the cell faces.

I don't think there is any confusion, i just made a function that is '1' at the free surface and '0' everywhere else. I'm sure there must be a better way but it seems to work so far.