[kalyan106]

Hello everyone,

I have a question on CFX particle tracking and would like your valuable insights on that.

I am running an unsteady RANS simulation of an axial flow compressor with a sliding mesh. The simulation consists of (1) aerothermal calculations to obtain the flow field and (2) particle tracking, in which particles are injected and tracked through one-way coupling with the flow. The aerothermal calculation is very expensive; particle tracking is cheaper, but I need to study many kinds of particles (think of a parametric study). Also, during particle tracking, I want the flow field to keep changing. I can think of two ways to achieve this:

One, keep solving for the fluid on the fly as particles are injected and travel through the domain. However, this is very expensive.

Two, perform the aerothermal calculation once, save the flow field at different timesteps, and then perform particle tracking by loading the saved unsteady solutions as particles are tracked.

Challenge: I found that it is possible to turn the fluid solver off while particles are tracked. So, after the simulation is initiated, the flow field in the first time step is loaded. As time goes, particles are tracked, and the rotor also rotates. However, the flow field is not updated.

Solution: Is it possible to update the flow field as particles are tracked? If this is not possible within the software, can a workaround be developed? Like PyAnsys?

For example, let’s say I have a fluid time step of 1 s and saved the flow fields at t = 1, 2, …, N s in a previous aerothermal calculation (time step of 1 s). Can I build a script to (a) initiate the simulation using flow solution at t=1s, (b) track particles till time reaches 2 s (end of 1st time step), (c) reinitialize/change flow field using the saved flow solution at t = 2s and continue particle tracking? This process is repeated every time step.

P.S. - In step (c), if particles cannot be continuously tracked from the previous step, I can also inject particles using their information at t= 2s and restart the tracking process.

Thank you!

[ghorrocks]

What are the different flow fields you want to do this with? Are they a transient simulation? Or are they totally different conditions (different flow rate or pressure)?

[kalyan106]

Thank you for answer. Here is what I would like to do:

Before particle tracking: Yes, the flow fields come from different timesteps in a transient simulation. I have all the timesteps saved as .trn files, example, 1_full.trn, 2_full.trn,.....,10_full.trn for a transient fluid simulation (initial and boundary conditions fixed) for 10 timesteps. These timesteps also contain 10 different angular positions of the rotating domains, say rotor 1.

When particle tracking starts: I would like to initialize the fluid using say 1_full.trn, and then do the particle tracking for 9 timesteps, with the fluid solver turned off and the rotating parts still rotating ((using expert parameters)) What I would also like is to be able to load the files 2_full.trn,.....,10_full.trn during the particle tracking, so that the particles see different flow fields as they travel across the domain, without solving for the fluid in real time.

Let me know if you need any other information.

[ghorrocks]

What you describe is easily done by:
* Do a transient simulation and generate the trn files at the time points you want the particle tracking done
* Do particle tracking simulations at each time point, using the trn files as initial conditions and using expert parameters to turn the fluids and thermal solvers off.

This approach only works if the particle time scale (ie: time taken for a particle to go from inlet to outlet) is small relative to the fluid time scale (ie: time taken for the transient flow features). If they are of similar time scales this approach will not work and you will have to do a normal transient fluids/thermal simulation with particle tracking as well.

I am confused why you say you want to do the particle tracking for 9 timesteps. Can't you just do it in a single time step?

[kalyan106]

Thanks for your reply. To answer your question at the end, I would inject particles only at the end of the 1st time step and let them travel throughout the domain. I want to see the effect of the changing state of the fluid on the particle trajectories. I would not like track the particles in one single timestep, otherwise they would see a "frozen" state of the fluid as they travel across the domain.
To give you an idea of the time scale differences, here is what I have to say. I have a rotor with a pitch of 15 degrees, and I want to choose a fluid timestep so that each pitch contains 100 timesteps (to capture the unsteadiness). This gives me a fluid timestep of ~ 1e-7 s. If I now consider the no. of such timesteps required for the particles to travel from inlet to outlet, it is around 9k timesteps. I want to write a script or CCL, so that after the initialization, once the particle tracking starts, CFX keeps changing the fluid state after each timestep the particles are tracked for. And this should come from the already saved .trn files, not solving for the fluid again.
I hope that gives you a better picture. The solution you gave in the beginning makes sense, but I want to automate it. Let me know if you think this is feasible or have any other questions.

[ghorrocks]

OK, so you are saying the particle time scale and the flow time scales are similar. In that case you have to run a transient simulation with particle tracking. You cannot use a series of pre-generated flow fields (not easily at least).

[kalyan106]

Yes you are right, it is not straightforward in the CFX GUI, so I was wondering if I could do it using either User Fortran, Junction Box Routine or PyAnsys. I looked up the CFX documentation and other online sources, but haven't had any luck yet.
Maybe it is possible in Fluent, but for some reason I have to use CFX.

[ghorrocks]

Yes, it can be done in user fortran. But it is not easy, hence my comment. CFX user fortran is complex and not well documented so it is challenging.

I have no idea on Fluent, I am not an expert on that one.

[kalyan106]

Your comment "Yes, it can be done in user fortran." gives me some confidence. I have used it before for implementing a lot of user defined stuff in CFX, so I know how to write one. But I wasn't sure if my problem can also be solved using this. Let me try doing it with user fortran. I will update if I have any luck, thanks!

[ghorrocks]

Sounds good, good luck! I suggest it sounds like a junction box routine which overwrites the flow field every time step with a flow field loaded in from the trn files. Junction box routines are more complex than the CEL function, but if you have some experience with CFX fortran you have a head start.