[Upa_upitas]

Hey!

I'm working on determining the mixing time of a bioreactor at different rpm. To achieve this, a tracer injection (scalar additional variable) is simulated while monitoring its concentration. I work in CFX.

Due to the geometry of my fluid domain, steady-state simulations don't converge, so everything is done as a transient simulation, even to establish the velocity fields.

It works fine when the tracer injection is solved simultaneously with the establishment of the fluid and turbulence fields in a single simulation.

However, when using a Frozen Field approach, it doesn't work: all equations for the tracer remain at 0 in the solver step, as if it is never injected or calculated (even though the same injection mechanism works in a simultaneous simulation). For a Frozen Field approach, I'm following this procedure:

1. Perform a transient simulation (15s) of the reactor stirred at the desired speed. There is no tracer injection, and the tracer concentration (initial conditions) is 0 throughout the entire domain.
2. Add the tracer injection to the same .def file. Using Expert parameters, turn off the equations for the fluid and turbulence while activating the scalar equations.
3. In the solver, use the file from step 2 and solve with double precision, using the results file from step 1 as initial values.

This procedure doesn't cause the solver to crash, but the tracer equation (the only one being solved now) remains at 0 (see picture attached).

Do you have any idea why this might be happening? What am I doing wrong when moving from a simultaneous simulation to a Frozen Field approach?

Thanks for your help!

[ghorrocks]

Using a transient model with a Frozen Rotor MFR model does not make sense to me. If you are modelling it transient then you should use a proper Transient Rotor/Stator model, ie: model the correct motion of the device.

Your problem may be linked to this - try running it transient rotor/stator and resolve the rotor motion.

[Upa_upitas]

Originally Posted by ghorrocks

Using a transient model with a Frozen Rotor MFR model does not make sense to me. If you are modelling it transient then you should use a proper Transient Rotor/Stator model, ie: model the correct motion of the device.

Your problem may be linked to this - try running it transient rotor/stator and resolve the rotor motion.

Thank you for the answer

Are you talking about the interface "Frame change/Mixing model"? There is an option "Transient Motor Stator".

Once changed this option, how would you continue to model the tracer injection and mixing time? Two-step Frozen field or just one step simultaneously solving the fluid/turbulence field with the scalar?


My main concern right now, is that doing it simultaneously makes it impossible to use the right time step corresponding to 5º rotation of the impeller/time step--> the required time step is extremely small and the solving process take more several days and the solver always ends being crashed by the system. No .res file are generated.

Many thanks

[Gert-Jan]

Please share your output file with all the settings.
To upload a file, use "Go Advanced"

[Upa_upitas]

Originally Posted by Gert-Jan

Please share your output file with all the settings.
To upload a file, use "Go Advanced"

Hey,

the .out file is to heavy even using Go advanced settings. Which part of the definition or solver are you interested in?

If using transient rotor/stator should I use Pitch change in somehow?

It's computationally impossible to set a time step which ensures 5º rotation

Thanks

[Gert-Jan]

Only the top part with the settings.
Everthing Between LIBRARY: and COMMAND FILE:

[Upa_upitas]

------------------------

[Upa_upitas]

------------------------------

[Upa_upitas]

------------------------------------------------

[Gert-Jan]

Why don't you upload a text file?

[Upa_upitas]

Originally Posted by Gert-Jan

Why don't you upload a text file?

Here you are

I'm new in the forum sorry

[ghorrocks]

Frozen rotor is not intended to be run in a transient simulation, especially one where you turn equations off.

While running it as a full transient simulation, with the interface as transient rotor/stator will take longer it is physically correct and will converge. So if this approach takes too long then you need more computing power.

[Upa_upitas]

Originally Posted by ghorrocks

Frozen rotor is not intended to be run in a transient simulation, especially one where you turn equations off.

While running it as a full transient simulation, with the interface as transient rotor/stator will take longer it is physically correct and will converge. So if this approach takes too long then you need more computing power.

Thanks

So I should run it in a full transient with a Transient Motor Stator as mixing model in the interfaces and Pitch set at "none". I'm afraid that using the right 5º-time step won't be computationally possible so I will use larger time step while discussing it on the MSc Theso¡s report.

Just to check we are on the same page, when I said "Frozen Field approach" I didn't refer to the interface mixing model "Frozen Rotator". I was thinking on using a v-established fluid and turbulence results file as a initial values for the simulation solving for the scalar.

Many thanks

[Gert-Jan]

You have a Frozen Rotor simulation setup in which you want to solve the transient tracer, while you don't solve the flow as Fluids=f.
Then what do you use as Flow field? Do you use the flow filed from the transient calculation as initial guess (through interpolation)?

Not sure but I guess this is not enough. Apparently, a interpolated solution is not used as flow field for your tracer. I guess that you should at least solve the flow for a microsecond.

So, I would add a step in between where you solve the flow with Frozen rotor for a single timestep of 1 microsecond. In that case CFX sets everything right. And then continue with the transient calculation of the passive tracer.

[Gert-Jan]

As Glenn mentioned:
Remember that the Scalar will be solved in the variable "Velocity", in both Transient simulations with Transient Rotor-stator interactions and in Steady state calculations with Frozen Rotor.
In Transient calculations, this leads to realistic results since the tracer is convected by the variable Velocity AND moved by the rotation of the rotating domain.
In steady state calculations, with Frozen Rotor, the rotating domain is not rotating. So, in the simulation the tracer will only be convected by the variable Velocity. The tracer will not move by the rotating domain since it frozen. As a result, the tracer will move in the wrong direction in the rotating domain. It will be discontinuous over the interface because the variable Velocity is also discontinuous.

So, you make an error here when using frozen rotor. If the rotating domain is small compared to the mxing tank, this might be acceptable. Alternatively follow Glenn's advice.

I asked ANSYS to allow me to convect the tracer with the variable Velocity in Stn Frame in a frozen rotor setup, since this variable is continuous over the interface. That would give not perfect but more realistic results. At least, the discontinuity in the interface would disappear. Unfortunately, ANSYS doesn't listen to me.

I tested Fluent and Star-CCM+. They have the same problem. And both don't have an option to mix the tracer in the variable Velocity in Stn Frame.

[ghorrocks]

So I should run it in a full transient with a Transient Motor Stator as mixing model in the interfaces and Pitch set at "none".

Yes, correct.

I'm afraid that using the right 5º-time step won't be computationally possible so I will use larger time step while discussing it on the MSc Theso¡s report.

You should use a time step size determined by a sensitivity analysis. I suspect a 5° time step will be way too large.

Just to check we are on the same page, when I said "Frozen Field approach" I didn't refer to the interface mixing model "Frozen Rotator". I was thinking on using a v-established fluid and turbulence results file as a initial values for the simulation solving for the scalar.

Your output file has this for the domain interface: Bottom:
FRAME CHANGE:
Option = Frozen Rotor
END

This is the Frozen Rotor I am referring to.

[Upa_upitas]

Originally Posted by ghorrocks

You should use a time step size determined by a sensitivity analysis. I suspect a 5° time step will be way too large.

The time step necessary for 5º is extremely small (ie 1,6 to 0,4 ms depending on the rpm) and it takes several days to be solved in a full transient process. The university cluster where I sent the simulations just kills the simulation for being too long and heavy. Cannot go to this range of time step and requires to move to rotations larger than 5º.

Therefore, I'm interested in only solving for the scalar with the right time step using the v-established flow & turbulence results file...

Everything using the Transient Motor Stator as mixing model

1000 thanks for your answers !!!!!