[juliom]

Thanks Glenn for the clarification!

[Guille1811]

* You have viscous work on. Unless you intend to model viscous heating turn it off. I can't see how viscous heating is significant here.

I turned it on because cfx pre gived me a warning message that when using total energy option (ill explain why i used this option later) you have to active viscous work.

* Why are you modelling the solid? This makes this a CHT simulation which is much more complex. I cannot see why you need to model the solid.

Im modelling the solid because in the real world scenario the volume and position of the engine affects the direction and positions from which the air is being sucked by the momentum source. That being said, because the air is at different temperatures in different heights i thought this fenomenon would be important to incorporate in the simulation

* You have modelled the blower as a rotating domain. It would be MUCH simpler to have one stationary domain for the whole simulation and model the blower as a rotating momentum source. By this I just mean the X,Y and Z components of the momentum source are varied as a function of time to make it a rotating blower.

Well actually there are those to settings being used. If you look at the definition of the momentum source you would see a parameter "phi" which varies over time and represents the angle of rotation. If you mean that i could just simply make the domain stationary (while using the "phi" setting) my question is how can i make it work considering the cilindrical geometry of that domain. In other words, if i make it stationary and then the angle phi varies, the outflow wont be parallel to the cilindrical axis by no means and that would not be the real life scenario.

* You have the total energy option selected. Why do you need that? A thermal energy model will be much simpler and robust and I suspect will have enough physics for this case.

I thought the same as you but i did an experiment and started a run on total energy and another one on thermal energy and funny enough the thermal energy one gived an even smaller timestep, which didnt grow even a bit after 2 days.

* You have the frame change model as frozen rotor. If you want to model the rotation of the blower then shouldn't that be Transient Rotor Stator?

That setting i literally just followed the advise of a friend, my mistake.

* What is the purpose of the porous model? This is yet another model which will add complexity.

The purpose of the porous model is that the air from the momentum source hit these vinetrees and pass throw them, so i modelled that domain as a porous one, with soft wood being the solid, porosity 0.7, permeability 1E-9 and 0 resitance coeff (because of lacking data)

Thanks a lot for your time btw!!

[Guille1811]

I add to the second point you mentioned that made the solid adiabatic, if it changes anything to said...

[ghorrocks]

Based on your comments I recommend:

* Changing to Thermal energy model. You don't need a full total energy model. Also turn viscous heating off. This will simplify your physics.

* If you think the inlet/outlet ducting is important then you model the ducting as a region cut out from your domain, not as a solid. Have a look at the tutorial examples of how they model butterfly valves and rotating machinery. You do not model the solid as a body unless you want to model heat transfer inside the body.

* Fix the GGI option, it should be TRS.

* Have a look at the porous model. It will be adding significant convergence difficulties to your model (and the whole point of this thread is that you are having convergence difficulties). Have a look at how it is working - is significant flow going through it? If no flow appears to be going through then just replace it with a wall as it won't make much difference to the result. If the flow passes through without doing anything then just leave them out entirely. I would only model the porous region if the flow is passing through it and being significantly affected by it.

In general - only add physics when you know you need it. So use the simplest physics to model what is necessary. Do sensitivity analysis on the different physics models so you know what is significant and what is not - and then don't model stuff which is not important.

[Guille1811]

Glenn, I implemented all of your recommendations but sadly the timestep size behaves exactly the same after almost 2 entire days of running. I even made an extremelly simplified version of the simulation, with no oscilation and no "engine volume", bigger domain and much better mesh and the timestep size behavious is almost exactly the same.

The first picture attached is a monitor of the timestep size given by the addaptive timestep on the standard simulation (with your changes implemented of course) and the second picture attached is the same monitor but for the oversimplified case.

I really just dont know what to do at this point, what could be the explanation for this extremely low timestep size?

[ghorrocks]

The explanation is the same as all along - the solver is having trouble converging so it requires a very small time step to converge.

From here I would recommend:
* Look at the results files in detail. Do a few time steps where you output a results file every time step. Look closely at the results for things like oscillations, unstable flow and things jiggling about.
* If you find any oscillations, instabilities or jiggles then think about whether it is likely to be real. Note that large scale flow oscillations are common in jet flows, so I think it quite likely you will find something.
* Put the residuals in the results file. Use the post processor to find where the area of highest residuals are, as this is the region which is holding back convergence.

If you can post some images of what you see as you check these things that will help.