[MarcelloAsciolla]

What is main the difference between "solid" and "immersed solid" when I have to choose the domain type?
Why should I choose one over the other?

I also read this limitation about the "immersed solid":
"[...] immersed solids currently affect only hydrodynamics; other immersed solid physics is not yet supported. [...]"
What does this limitation mean exactly?
Does this mean that this option uses an implementation that is valid only for simulations with "water" or does it means that it is valid for M->0 (for every fluid)?

[urosgrivc]

These are two very diferent things
What are you modeling?

Solid is used when your domain is not a fluid (heat transfer(cht), coupled fluid structure interaction...)

Imersed solid is a solid domain vhich overlaps sthe fluid domain so you can have both at the same place (mesh vise) fluid forces are tranfered to this imersed solid vhich has inertia (multidirections) and can have restricted movement or rotation (multidirections).
Imeresed solid influences the flow and vice versa
If you need good near wall treatment and results immesred solid is not wery good because of overlaping mesh.
It does not suport heat transfer

check rigid body also

But it depends vhat you are modeling

[MarcelloAsciolla]

Thank you very much,
my problem is about a little fan in a duct and the fluid is air.

I thought that both the options could be possible in this case.
The main difference that I know is that if i use "solid" I have to define also an interface solid-fluid (for "immersed solid" it not necessary).

What would you suggest best between theese two solutions?

[urosgrivc]

Well the thing is you dont need any of these.

You model a propeller like a hole in the fluid, you do not need a solid at all.

Than you slice your domain so you have stationary parts and a rotating one which encases the propeller hole.
this is called a rotating domain.
And you will need two interfaces to connect stationary domains to this rotating one.

all fluid forces, pressures, velocities and everithing are relevant only on the wals, that is why you dont need a solid.
but you do need propeller wals that is vhere the hole comes into play, you can make it vith boolean operators

[MarcelloAsciolla]

No, I can not. I need the full unsteady story of the field, because this is the start point for another analysis about the radiation of the noise. When I wrote that the fan is little I wanted to say that the whole scale of the problem is of the order of the dm and, even if the rpm is high, I have M<<1. The radius and the length of the duct are also little, so I have to choose a domain for the fan.

[urosgrivc]

OK

but why do you need a solid?

You can do steady state or transient (LES, DES..) if you want but the solid does not efect the phisics of your problem.

Are you doing omething like this?
https://drive.google.com/open?id=0Bw...lh6OGhsQ3dZMk0
there is no solid involved here

[Gert-Jan]

I strongly advice you to follow the instructions of urosgrivc. You really should not use immersed solids for this.

[MarcelloAsciolla]

OK, now I understand that solution. And yes, this could be a great idea!
I think that at the start the behavior of the fluid is a bit forced, but after a while it should work perfectly.
What about the total time of the simulation?
Are the results reliable also around t=0?

[urosgrivc]

What? no
If you are doing a transient simulation, results are as good as your initial conditions are at t=0.
if you initialize your tranzient case with your converged steady state than your results at t=0 are, well the same as for steady state solution, but than the flow develops and your results might be either wery diferent or the same depends on if your problem is actualy transient.

Total time is totaly case dependant, it can be 1000s or 0,0001s I dont know what you are triing to simulate
it depends on suroundings your initial state and other variables

I didnt exactly understand the (fluid is forced) part

[MarcelloAsciolla]

Let's suppose that I have these istants:
t0=0, t1, t2, ..., tn, ..., t_inf
At t=t0 I have the initial condition and let's suppose that this is correct.
But at the first steps (t1, t2, ..., tn) I do not think that the fluid has a correct behavior, because I am forcing the behavior adding a discontinuity to the initial condition in the velocity components.
So the situation at the start of the simulation is that the domain at rest is too much accelerated around the interface while the domain in motion is too much slowed down.
After a while (t>>tn) that discontinuity will disappear because there is a merge of the domains and the whole fluid acts as one fluid.
So I do not expect that the values calculated at t1, t2, ..., tn are correct and reliable, but they should be good from tn+1 to t_inf.
So my question is: how can I evaluate the value of tn?

[urosgrivc]

(I have the initial condition and let's suppose that this is correct)
ok what? you know the velocities and pressures of every element in the domain are corect, how?
Where did you get your initaila condition from

if a person vould know that there vould be no need for cfd

Why is your fluid flowing is the fan pushing it or some pressure change or you have some knovn velocity.
i dont understand the problem

[MarcelloAsciolla]

When I wrote <<let's suppose that in t0 the initial condition is correct>>, I wanted to mean that I am not putting the attention on t0, because I already know that it is not correct, but consider for a moment that it is the best that one can achieve.
I am focusing on the next steps, expecially on t1, because it is like I am adding another source of error passing from t0 to t1. And after this error will tend to disappear and I expect that it could be negligible from t=tn.
In other words with this method I have to take in account that I am adding this discontinuity and after I am smoothing it.

[urosgrivc]

I am sory but i dont understand the problem and am not able to help if you dont explain vhat you are doing

[Gert-Jan]

@ Marcello: What question are you trying to answer using CFD?

[MarcelloAsciolla]

I need the story of the fluid moved by the fan. This is the first step for an acoustic analysis that will be performed after with another software and it is important that the values calculated at every time step is reliable. I am not sure if at the first ones the local values around the interfaces are good enough. So I am thinking that maybe I need to make a longer simulation.

[Gert-Jan]

Maybe you can put the interfaces at a location where they do not interfere that much in your solution. Please share or sketch your geometry. Even though I think it will be very simple.

You just have to start from a frozen rotor simulation and then continue from there to obtain a transient solution. Just add a few monitoring points where you monitor velocity, pressure and tke, and then wait for a while to get a repetitive solution.
Then add your discontinuity on your inlet, whatever that may be and then monitor how it will propagate through your solution.

If you follow this approach then the local values at the interfaces will be ok. Make sure you write transient results quite often and write Velocity at Stn Frame, Pressure and other relvant variables. You could also opt for transient statistics (averages, variances etc.) to judge the validity and convergence of your solution.

[MarcelloAsciolla]

Yes, I will try to solve in this way. Thank you very much for your support and all your tips!

[Ali Di]

Hi all,

I want to simulate movement of a two-phase fluid inside an immersed solid (There are two fluid domains, the first one is the fluid that the solid is immersed in it, and the second one is the fluid inside the solid).

But, the two-phase fluid doesn't move with movement of immersed solid. Can any body help me for this matter?

Thanks in advance.

[Gert-Jan]

Non comprendo.
What kind of 2-phase-fluid do you have inside if it does not move? Isn't it s solid then?
If not, make a drawing and share it.

[Ali Di]

Originally Posted by Gert-Jan

Non comprendo.
What kind of 2-phase-fluid do you have inside if it does not move? Isn't it s solid then?
If not, make a drawing and share it.

Dear Gert,

Thank you for your reply. I attached a geometry (in a zip file) from a simulation that I talked about.