HELP REGARDING PROPELLER THRUST SIMULATION.

[Anonymous]

Hi,

I have used a 400 odd mm dia. propeller for simulation under 0 air velocity, and created a ramp up rotating region around the propeller, and gave some parameters i have no knowledge of apart from the boundary condition and all the rest of parameters, i have yet to find a tutorial related to my project, 

*note: the propeller i am simulating is for drone (quad-copter specifically), and i have not got any result relate able  to real practical world, i have a very busy time, please if some tutorial very close to my project is provided, 

I have attached my file in rar, please look into it and give me some suggestions.

Regards

[Jon.Wilde]

Hi,

Before I dig into this, have you seen the guide here and followed it?

Rotating Regions

Thanks,

Jon

[Anonymous]

Hey thanks for that i hope i have read the rr part, yet it was refreshing so thanks for that,

And the quotes "Uniform mesh the leading and trailing edges (even on the suppressed impeller) to properly capture the flow here

The boundary between the RR and the static elements needs a uniform mesh assigned to it (useful for the CFL number - see below)


Use surface refinement - good practice for most models


Start with using 3° increments for the time-step from the start instead of using blade to blade approach. Running with 3° from the start is a good idea so that you don't need to stop and start the run to finish the analysis with 3°. Using a smaller time step also reduces chances of a divergence

Saying that - if the model is skipping more than one element at a time between the rotor and stator, use a smaller time step from the beginning. This can be visually checked with a cut plane through the model as it is running

If a uniform mesh was used, this in conjunction with the rpm and the circumference will provide an easy way to calculate how many elements pass past each other over each time step


Try to ensure that the Courant-Freidrich-Lewy criterion, where local fluid velocity x time step / mesh size < 2 is not broken"

Is not understood by me correctly can you give me a template where in i can sort of relate and understand. That would be awesome.

And please do look into the file i sent you earlier.

[Jon.Wilde]

I can share a few pointers based on your model. Everything within that document would apply here though, you really need to follow it step by step 🙂

1. Model is over constrained, have flow at inlet and P=0 at outlet, not flow on both
2. Ramp up the RR over 50 steps and then let it run for a few 1000 iterations to give you a data point. The table for the RR material should have 3 lines. One at 0, one at whatever works out to be 50 iterations and then the same speed at 100s or something so it never reaches this point 🙂
3. Your mesh looks REALLY fine, I would guess that this will not run unless you have a super machine. Consider simply using a manual mesh
4. Do you really need the holes in the hub modelled? I would think these are better closed
5. Run at 3 degrees a time step for the entire run, I am not sure what number this should be as you have a range of rotational velocities assigned
6. It might be good to run with intelligent solution control off
7. As you are using the SST turbulence model, you really need more wall layers to get a Y+ value down below 1 (see some settings below that might be a good starting point)
8. You need to enable Y+ within Result Quantities (under Solve) to be able to plot Y+ with an ISO surface once the run is complete

Hope that helps,

Jon

These are only a starting point. You need to run it and capture the converged results, check out the Y+ and then decide how to proceed. You might need to change the settings and re-run.