FLUENT V5 - How to calculate mixing or blending time with the Multiple Reference Frame model


Given is a simulation of a stirred tank using multiple reference frames. Now, the blend time is to be calculated. How to do?

After a fluid flow simulation for a stirred tank has been done, often
the flow field is to be used for a transient simulation of the
transport of a (dissolved) tracer species. This is the numerical
simulation of a well-known experimental method to determine the
so-called blending or mixing time: The tracer is added locally at time
t=0, and from then on the tracer concentration is followed over time
by appropriate probes at one or several locations in the tank. The
blending time is then defined as the time after which the measured
concentration(s) for the last time enter(s) a certain range around the
equilibrium concentration.

If this is to be done in FLUENT5.x, some important points should be
noticed, as described in the second Resolution (press [>>]).

The blend time is defined as the time from the addition of a trace pulse until a certain degree of homogeneity in the stirred mixture is reached. This is essentially the instruction how to proceed:

1.: Switch off the calculation of all equations (flow, turbulence, energy,...) under Solve--Controls--Solution.
2.: Switch on multiple species (no volume reactions) under Define--Models--Species.
3.: Define two different fluid materials (species) that have exactly the same properties as the fluid that the fluid flow simulation has been performed with.
4.: Create a "mixture" material that consists of these to components. Choose this "mixture" material to be active under Define--Models--Species.
5.: Under Define--Models--Solver, switch on unsteady calculation, choose 2nd order implicit unsteady formulation.
6.: Under Solve--Controls--Solution, verify that only the trace species equation is on, set its underrelaxation factor to 1.0 and choose the second order convection discretisation scheme for it(!).
7.: Mark a small part of the domain using Adapt--Region, enter coordinates, press "Mark" (NOT "Adapt").
8.: Patch a mass fraction for the tracer species of 0.2 into the whole domain (all fluid zones). Then, patch a mass fraction (for the same trace species) of 0.8 only into the mark register from the previous step.
9.: Define several "probe positions" by creating Point Surfaces (Surface--Point) at various locations. Define Surface Monitors for these "probes"; plot and write (to a file) the (average of the) tracer species mass fraction once every time step.
10.: Run the unsteady simulation. Set the time step size so that the fluid crosses no more than ONE cell per time step everywhere in the domain. Each time step should converge (constant monitors, species residual around 10^-5 or less) within 10 to 20 iterations. If it doesn't, reduce the time step size. (This is very important!). The time-dependent trace concentrations at the various probe locations will be monitored (and written to their respective files).

The blend time can now be defined as the time it takes for the concentration at any (or all of the) probe(s) to enter a certain deviation margin around the terminal concentration, which will be reached after infinite blending.gf

NOTE: If you re-patch the same initial conditions and run a new tracer transport solution, very strange things may (will!) happen due to a bug in Fluent6 (6.0.20). Please see Solution 514 for details. Preparing and setting up the solution in FLUENT 5.x

1. First, do a simple fluid flow simulation for the stirred tank as
usual. You may use fixed velocity data, multiple reference frames
or sliding meshes to accound for the impeller in the simulation.
(For particular comments on numerical tracer experiments in the
latter two cases, please see below.)
2. As the very first step of the set-up of the numerical tracer
experiment, go to Solve--Controls--Solution and switch off the
solution of fluid flow and turbulence. Make sure this is done at
first.
3. Create a second fluid material that has identical
properties to the one you used as the stirred liquid, but with a
different name. Switch on Multiple Species
(Define--Models--Species), without reactions or any other model.
Then create a mixture material that consists of the two liquid
materials you used/created for this analysis. Activate this
mixture material in the Species panel. (Don't forget this! --
After this step, you can switch off the Energy transport model,
which will have been enabled by FLUENT when you enabled multiple
[non-reacting] species.)
4. Enable transient simulations (Define--Models--Solver: unsteady).
Choose second order time discretisation. Also, go to
Solve--Controls--Solution again and enable second order
discretisation for the species transport equation. (You may use
QUICK if this is available.)
5. Mark a small part of the tank volume using any of the tools in
the Adapt menu. Don't really adapt (if you pressed the "Adapt"
button, just reply "No" in the confirmation box that will
appear). Then use Solve--Initialize--Patch to patch a certain
tracer concentration in the newly created register.
6. For the transient simulation, you have to choose a proper time
step size. Use the so-called Courant criterion: The time step
should be sufficiently small, so that in no cell the flow goes
longer than across one cell within every time step. In addition,
every time step should converge in 20 iterations maximum.
Convergence should be monitored using surface monitors plotting
the tracer concentration on a Point Surface (generate using
Surface--Point in the menu). It will probably not become constant
before the scaled residuals go down to approx. 1.e-5 or less. Too
small time steps (e.g. in parts of the volume where there are
very small flow velocities) usually do very little harm.

Interpreting Visualised Results - Tracer Transport in Rotating Zones

If you started from a flow field that was calculated using multiple
reference frames or sliding meshes, and if you then visualise the
tracer transport by a nice animation, you will find that the
rotational movement of the tracer "blob" will go against the direction
of the impeller rotation, when the tracer enters the rotating frame of
reference / moving mesh zone. This is necessary - the tracer transport
simulation must be done in the same numerical way as the fluid flow
simulation is. (This is an inherent constrain of the finite volume
technique.) For this, in the inner frame of reference / moving zone
relative velocities must be used, as they are seen by an observers who
rotates at the same speed as the shaft (and impeller[s]) does. (Only
by this, mass conservation of the trace is guaranteed.) In spite of
the apparently unrealistic simulation approach, resulting blending
times have been proven to agree very well with reality.

Using the absolute frame of reference

If this is really desired, it is even possible to do the complete
simulation in the absolute frame of reference. This will cause the
tracer "blob" to rotate in the same direction throughout the
computational domain. But by this, it will collide severely with the
impeller blades, not penetrating them (which would be necessary for
mass conservation), but disappearing out of the calculation as it is
pushed against the blade surface by the flow. This will lead to severe
tracer loss, so that the monitored tracer concentration will never
reach the expected equilibrium value. (The extent of this loss depends
on many factors, amongst them the size of the impeller.)

If you really want to do the tracer transport simulation in the
absolute frame of reference for the whole computational domain,
proceed as follows:
Before you start the unsteady simulation, create three custom field
functions. Each of them should be defined to be identical to one of
the velocity components (U, V, W). Now use "Solve--Initialize--Patch"
to patch each of the velocity components in the complete domain (all
fluid cell zones) using the corresponding custom field function.
(Enable the button "Use Custom Field Function".) This should
apparently exchange the current flow field by itself, i.e. change
nothing. But as the custom field function will give the absolute
velocities (NOT relative the any rotating frame of reference), this
operation feeds the absolute velocity information into the solver's
data fields, so that these data will be used for the transient tracer
transport simulation. --- Remember to switch of the solution of the
Flow (and turbulence) equation at the very beginning!





Show Form
No comments yet. Be the first to add a comment!