[Diger]

Is there something like an upper limit for this value suggesting to refine your mesh?

[LuckyTran]

Not really. The cell quality metrices like orthogonal quality, skewness are much better metrics.

The cell Reynolds number together with the Peclet number is used to determine what physics dominants a cell (advection vs diffusion) and therefore what discretization scheme should be employed. For upwind schemes you want this number to be high, not low. For DNS, you want this number to be <1 everywhere.

[Diger]

What does it mean "high"?
>100, >1000, >10000, >100000

[Diger]

Let me give you an example:
https://ibb.co/cZK6ty

This is a picture of the cell reynoldsnumber for the current model I tried.
It is a 1m x 1m x 1m Box and at the bottom is a pylon with a small nozzle ontop of it. It has a pinhole of 1mm and air is coming from the right with 170m/s. I want to know the mass flow through the pinhole.
Pressure is 490hPa and Temperature is 267K.

I thought that since in most of the box there is just a constant velocity which is a simple problem and therefore I used a coarse mesh leading to high cell reynolds numbers in the upper part. For the pinhole I used elementsize for the boundary surface of 0.05mm which leads to a very fine mesh near the pinhole and thus more or less low cell reynolds numbers.

I run the coupled pressure based solver with standard schemes for 50-100 iterations and then stop every 10 iterations or so to check the mass flow. The value is somewhat reasonable, but I noticed that there seems to be some oscillation in the massflow (though the pinhole) of about 10-20%.

This is what such a balance looks like:

Mass Flow Rate (g/s)
-------------------------------- --------------------
inlet 108904.3
nozzle -0.050687105
outlet -108904.84
---------------- --------------------
Net -0.58386601


Could the oscillations come from unsteady flow or have you encountered something like that?
Any suggestions regarding the mesh or setup? How would you do it?

[obscureed]

Hi Diger,

In any situation with a fast jet into a large expanse of gas, I would expect transient variation. (You wrote "in most of the box there is just a constant velocity". I agree there will be a fairly constant trend, but I would expect the jet to flap around -- a lot or a little, it's hard to predict.)

Would that transient variation would be enough to cause 10% variations in mass flowrate? -- oof, it's hard to predict.

If you apply a steady-state solver to a transient situation, you should not expect good convergence (and even if you get it, you should not completely trust it). There is no steady-state answer, so how can the solver find the answer? However, experience shows that a mostly-converged steady-state answer has some value -- it might approximate the time-based average solution. It might give you a rough idea of where the flow goes, and how significant turbulence is, etc. It makes some effort to conserve mass and momentum.

For example, suppose you find a steady-state recirculating flow pattern that returns to the vicinity of the jet, and that has a speed of order V. Suppose that this recirculating flow actually fluctuates transiently -- sometimes it hits the jet, sometimes it doesn't. That will cause a fluctuation in pressure outside the jet, and the magnitude of that fluctuation will be of order 0.5*rho*V^2. So now you can build up some kind of estimate of the level of fluctuations in mass flowrate that this transient effect might cause.

Now you need to think about why you are doing the simulation. Do you need to know the timescale/period/spectrum of the fluctuations? -- then you need to do a full transient. Do you just want the average condition, approximately? -- Well, a common assumption is that the steady-state solution will give some kind of estimate of this. Do you want the average condition accurately? You need to do a full transient for long enough to capture the whole range of behaviours -- and this is often far, far out of reach of any reasonable budget.

OK, you originally asked about mesh dependence. The rigorous way to look at mesh dependence is to try it. The pragmatic way is to look at the cell-by-cell variations, and guess whether the current mesh captures the effects you are looking for. In this context, with respectable numerics, there are no values of cell Reynolds number that intrinsically cause a serious worry. You will often find that a finer mesh captures a whole bunch of extra twiddles in the flow -- but then, they might not be important for you. CFD is still very much at the pragmatic, expense-limited stage of computing power.

A couple of practical thoughts: If the maximum speed is 170m/s (in normal air conditions), standard advice is that you need to include compressibility effects. Also, why do you "stop every 10 iterations or so to check the mass flow"? -- you should set up a report of mass flow every iteration, and plot it and write a transcript.

I hope this helps.
Ed

[Diger]

If the maximum speed is 170m/s (in normal air conditions), standard advice is that you need to include compressibility effects.

Doen that, but the maximum speed will probably somewhere around MACH1 at the nozzle.

Also, why do you "stop every 10 iterations or so to check the mass flow"? -- you should set up a report of mass flow every iteration, and plot it and write a transcript.

Actually this is the question I just asked in some other post.
I dont know how to precisely do it.
Can you explain what and how I set it up? Do you maybe mean "surface-monitors"?
PS: Probably found what you meant...


PPS: I just tried using a much more corase mesh, and it seems that the oscillations are much less pronounced. Does this mean that I do not resolve those structures or it is an artifact?

[Diger]

Now that you have seen what I'm trying to do, let me maybe ask you directly how would you do the meshing?


Would you just go for the coarse standard mesh and run the coupled pressure based solver, or would you do as I did i.e. coarse mesh, but using element size on the pinhole boundary surface or do you have any suggestions?