[dickes]

Hallo everyone,

I am modeling the bottling process of non-carbonated beverages using the inhomogenuous MUSIG Modell for bubbles and air-entainment. When I Change the drag cofficient in the Fluid Pair Modells Tab for the liquid/gas from a constant drag coefficient to an Expression found in a paper, I get the following error in the first iteration of the solver:

| Writing transient file 0_full.trn |
| Name : Transient Results 1 |
| Type : Standard |
| Option : Every Timestep |
+--------------------------------------------------------------------+

Details of error:-
----------------
Error detected by routine PSHDIR
CDRNAM = /FLOW/GETVAR/PHYS_ZONE_DIR/MULTIFLUID_MODELS/ /SIZGRP
CRESLT = NONE

Current Directory : /FLOW/SOLUTION/TSTEP0/CLOOP0/ZN1/VERTICES

+--------------------------------------------------------------------+
| ERROR #001100279 has occurred in subroutine ErrAction. |
| Message: |
| Stopped in routine MEMERR |
| |
| |
| |
| |
| |
+--------------------------------------------------------------------+


The Simulation is transient. I already raised the Memory allocation factor from 1 to 3 but the error prevails.

The expressions I use are from the paper Hänsch et al 2012 A multi-field two-fluid concept for transitions between different scales of interfacial structures

Thanks in advance!

[ghorrocks]

CFX error messages are not very helpful. It appears to be suggesting it is looking for a size group (or the size distribution from MUSIG?) while it is writing the results file but not finding it so crashing. So check your MUSIG setup to make sure the size groups are properly defined, and stay well defined at the limits of the ranges you expect to see.

[Opaque]

Would you mind sharing the expression for the variable drag coefficient?

It seems the expression is not being resolved correctly.

[dickes]

Originally Posted by Opaque

Would you mind sharing the expression for the variable drag coefficient?

It seems the expression is not being resolved correctly.

There are several equations interconnected inside the Drag Coefficient. I was able to reduce the problem to the use of the variable: Group I Diameter. When I apply a constant to this variable, the next error is due to a 0 in the denominator of the expression of C_D,sphere.

My expressions for the drag coefficients are the following:


Cd bubb = max(Cd sphere,min(Cd elipse,Cd cap))

Cd cap = 8/3

Cd cg = (1 - phi morph)*Cd bubb + phi morph * Cd cont

Cd cont = max(phi fs * Cd fs,(1 - phi fs)*Cd drop)

Cd drop = 0.44

Cd elipse = 2/3 * (Eo)^0.5

Cd fs = 0.01

Cd sphere = 24 / Re particle* (1 + 0.1 * Re particle^0.75)

Eo = (water.Density - gas.Density) * 9.81 [m s^-2] * dG1^2 / surface \
tension

Re particle = water.Density * slip velocity * dG1 / water.Dynamic \
Viscosity

a fs = 100

ab = 20

alpha cg crit = 0.3

dG1 = Group I Diameter

dx = 2 [mm]

mag gas vf gradient = (gas.Volume Fraction.Gradient X^2 + gas.Volume \ Fraction.Gradient Y^2 + gas.Volume Fraction.Gradient Z^2)^0.5

mag water vf gradient = (water.Volume Fraction.Gradient_x^2 + \
water.Volume Fraction.Gradient_y^2 + water.Volume \
Fraction.Gradient_z^2)^0.5

mag water vf gradient post = (water.Conservative Volume \
Fraction.Gradient X^2 + water.Conservative Volume Fraction.Gradient \
Y^2 + water.Conservative Volume Fraction.Gradient Z^2)^0.5

n = 4

nabla alpha cg crit = 1/(n*dx)

phi fs = 0.5 * tanh(a fs * dx * (mag gas vf gradient-nabla alpha cg \
crit)) + 0.5

phi morph = 0.5 * tanh(ab*(gas.Volume Fraction - alpha cg crit)) + 0.5

slip velocity = (((gasDisp.Velocity_x * gasDisp.Volume \
Fraction)/(gasDisp.Volume Fraction)-water.Velocity_x )^2 +((gasDisp.Velocity_y * \
gasDisp.Volume Fraction )/(gasDisp.Volume Fraction)-water.Velocity_y )^2 \
+((gasDisp.Velocity_z * gasDisp.Volume Fraction)/(gasDisp.Volume Fraction)-water.Velocity_z )^2)^0.5

surface tension = 0.073 [N m^-1]

[dickes]

Originally Posted by ghorrocks

CFX error messages are not very helpful. It appears to be suggesting it is looking for a size group (or the size distribution from MUSIG?) while it is writing the results file but not finding it so crashing. So check your MUSIG setup to make sure the size groups are properly defined, and stay well defined at the limits of the ranges you expect to see.

The out File lists the following information:

| MUSIG Size Group Information |
+--------------------------------------------------------------------+

Domain name : fluid

MUSIG fluid : continuous

Group Polydispersed Fluid Diameter Mass
Group 1 gas 8.5000E-03 3.8104E-07

Domain name : fluid

MUSIG fluid : bubbles

Group Polydispersed Fluid Diameter Mass
Group 1 gasDisp 1.5000E-03 2.0941E-09
Group 2 gasDisp 2.5000E-03 9.6948E-09
Group 3 gasDisp 3.5000E-03 2.6602E-08
Group 4 gasDisp 4.5000E-03 5.6540E-08
Group 5 gasDisp 5.5000E-03 1.0323E-07
Group 6 gasDisp 6.5000E-03 1.7040E-07
Group 7 gasDisp 7.5000E-03 2.6176E-07

So I am not sure why the solver is not able to find the variable. Any further help is useful!

[Gert-Jan]

According to your first post, you get the error while writing a full transient file 0_full.trn at iteration 0. That is before any iteration/calculation has started.
(Normally this is only used to check if the initial guess/initial condition is setup correctly.)

Do you also get the error if you do not write a trn-file at iteration 0? What if you write a trn-file at different iterations?
Is this question related to your previous question regarding DIAMCLIP_FL1?

[dickes]

Originally Posted by Gert-Jan

According to your first post, you get the error while writing a full transient file 0_full.trn at iteration 0. That is before any iteration/calculation has started.
(Normally this is only used to check if the initial guess/initial condition is setup correctly.)

Do you also get the error if you do not write a trn-file at iteration 0? What if you write a trn-file at different iterations?
Is this question related to your previous question regarding DIAMCLIP_FL1?

The error remains when I skip writing the first transient file.

My question regarding DIAMCLIP_FL1 is in the same simulation. I am trying to activate the different expressions from the paper
Hänsch et al 2012 A multi-field two-fluid concept for transitions between different scales of interfacial structures

To narrow the error message down I activate the different expressions one by one. The variable Drag Coefficient (Cd cg) is activated in the FLUID PAIR MODELS tab for momentum transfer. The Interfacial Area Density (Ad cg) is activated for Interphase Transfer (when the Error DIAMCLIP_FL appears). When I use both expressions at the same time the error MEMERR remains.

Update: The DIAMCLIP_FL error is solved! MEMERR from the Group I Diameter prevails.

[Opaque]

In your expressions there is a variable that is missing the "MUSIG FLUID" prefix, <Musig Fluid>.<variable>

Not sure which one in particular.