Learning Forum

[Jason Sum]

[Karthik Remella]

Hello To be honest with you, the choice depends on the nature of the problem as well as how strongly (or weakly coupled) your governing equations are. If you have a stiff set of equations, you are better off using a Coupled solver. Otherwise, any segregated solver might work. If you are solving a transient problem, I would go with PISO (if I believe right). To read more about this, I'd recommend that you refer to the following link from Ansys Help.
https://ansyshelp.ansys.com/account/secured?returnurl=/Views/Secured/corp/v211/en/flu_th/flu_th_sec_uns_solve_pv.html
Karthik

[Rob]

I'd be more concerned about the mesh resolution if you're using the mesh from here /forum/discussion/29218/why-i-was-banned-to-proceed-to-setup-after-meshing-even-i-fulfilled-the-student-ver-limit-of-512k#latest it's very likely too coarse to get a decent solution. Work out your cell courant number and plug flow residence time too: this might be a very long run.

[Jason Sum]

My geometry is large in size which makes meshing coarse while fulfilling the upper limit of 512k elements.
Would you mind explaining further on how to get a better result by looking into cell courant number and flow residence time, thanks so much Rob and Karthik!
I found that when COUPLED is chosen as the solution method, under 'Control', the flow courant number is 200 now, which I know the desired value should be less then 1. What should I do to reduce the flow courant number (or just directly change it to my desired value) and what to do with the flow residence time on Fluent?

[Rob]

The default is 200, which is fine for external aero flow, and far too aggressive for anything interesting, 20-50 is more reasonable for multiphase.
The values I suggested you look at will help estimate the time step you need, then the number of time steps. It's partly to assist in choosing the settings but also allows an estimate on the total run time. With that you can decide if it's feasible in the time you have.
If you want to use multiphase you need to resolve the phase gradient. Otherwise the results may be misleading. If the system is fairly level can you use a residence time approach? Look for "mean age of air" on here as it's a method that's been abused for years in many applications.

[Jason Sum]

Sorry that I do not have much understanding on phase gradient, I am kind of newbie to Ansys Fluent! Really need your guidance ! Thanks Rob!
As my elements and nodes cannot be smaller due to the limit of student version, as you said, what I can do is working on the courant number. Am I supposed to try inputting different Time Step Size and see the global courant number shown from the console, until a trial the courant number obtained is within 20-50 as you suggested? So that I can confirm my proper Time Step Size and determine the Number of Time Steps based on how long I want it to simulate in actual world?

The following residual graph shown having set up of Number of Time Step = 200, Time Step = 0.0001, Max Iteration = 20, obtaining courant number between 1 - 2 values .
(Solution method: PISO with default setting, Control: default setting)
(Three Nitrogen gas inlet with Gauge Total Pressure of 34474Pa and Supersonic/Initial Gauge Pressure = 34400Pa)
What is this graph implying? The k and epsilon curve keep fluctuating, is this meaning a undesirable result? What should I do to obtain convergence, thanks!!!

[Rob]

With PISO you want to get the VOF courant number to be around 1. The default courant number of 200 is part of the pressure based coupled solver, and is a setting you add: which was in answer to the question above my earlier post. You have since switched to PISO which is generally better for transient applications.
The above residual plot is because you're using the transient solver. We solve for each time step, and the spike is when we increment time and move onto the next step before we then converge each step.

[Jason Sum]

Ohh! So are the residual graph attached above and my setup for this simulation (pumping N2 to pump water inside away) on the right track? Or any symptoms from the curve can be seen that my setup is inaccurate? Thanks Rob again!

[Rob]

You've run 0.003s so it may be a bit early to draw any conclusions from the results!

[Jason Sum]

While initially obtaining global courant numbers around 1-2, the simulation then terminated after 68 time steps due to the sudden excess of 250 courant number, what should I check to debug the process, should I reduce the time step size or I should modify the PISO solution settings? Thanks!

[Jason Sum]

I reduced the time step size from 1e-4 to 8e-5 and ran the calculation again, the attached is the residual graph!
Initially the residuals tended to drop and converge, but after around 1000th iteration, the graph became like this. What can I do to modify so that convergence can be obtained? Thanks for your help!!!

[Jason Sum]

It is sincerely hoped for solutions and guidance from forum experts! Many thankss.

[Rob]

Have a look at the flow field and see if there are any regions with "odd" velocity vectors or poorly resolved gradients. They're usually an indicator of where things are going wrong.

[Jason Sum]

Should I set an animation for the velocity vectors, searching for the "odd" parts from it after calculation? Is Adaptive Time Stepping more preferable in my case (multiphase) for calculation? Thanks a lot!

[Rob]

Animations can help diagnose problems, but just having a look at the flow is often enough.
I generally avoid adaptive time stepping. It's an excellent idea in principle but as it relies on the solver spotting it's diverging before it fully diverges. Depending on the flow field that may not happen!

[Jason Sum]

I am struggled on where to observe the flow field and how to figure out the "odd" parts? Am I supposed to observe the contour about velocity to see any odd parts? thanks!

[Amine Ben Hadj Ali]

Create cell registers using Field Variable and provide ranges for velocity etc to identify places where you have overshoots. Moreover: just look into 5 to 10 time steps (under Residual Monitor reduce the number of iteration to be plot) otherwise you won't figure out if you are converging in each time step or now.

Also enable the physics constraint for adaptive time stepping.

[Jason Sum]

Thanks Amine. As shown above, the epsilon curve in residual graph keep spike higher and higher. How can I identify the problematic region(s) (causing the residual not converging) after setting cell registers?
In the following photo, what range should I set for the velocity magnitude so that I can find out the error of my setup? Thanks a lot!

[Rob]

The range you choose is model dependent. Look for regions that are fast compared to the expected velocities.

[Amine Ben Hadj Ali]

Case dependent and you need to feel reasonable value range which either by boundaries or by physics or even both.

[Jason Sum]

After running calculation with 200 time steps with time step size = 4e-5 and max iterations/ time step = 40, below is the residual graph obtained:
(Figure 1. Residual graph)
As guided, I set a field variable in "Cell Register" with velocity magnitude, found that the range of velocity for the whole model = 0 - 175, while only the following part especially having velocity range of 100 - 175.
I also set Turbulent kinetic energy k in "Cell Register" as field variable and found that the following part having especially highest k value.
Does it mean that I should mesh this part with finer nodes, or any further actions I can do to obtain a converging k value in residual graph and an accurate solution? Thanks a lot!
(Figure 2. Specific part found to have "odd" velocity)
(Figure 3. The velocity magnitude range of whole model)

[Amine Ben Hadj Ali]

Are you expecting this high velocity?

[Jason Sum]

I am not sure the velocity of particular point throughout the model. just knowing that each inlet pressure is 5 psi.
I deduce the above part (Figure 2 above) is the "odd" part of my model because the cells with top 70% of velocity magnitude of the model are from this part, which seems abnormal.
Also as the k value in residual graph spike up with greater fluctuation along the iteration, I found that the suspected "odd" part (Figure 2 above) having especially higher k value from cell register.
Should I improve the meshing quality of that part and try observe the residual graph again? I am not sure am I going on the right path, thanks for your help further!!

[Amine Ben Hadj Ali]

That is a good path.
If using VOF you can set a velocity limiting to avoid this kind of "abnormal" velocities.

[Jason Sum]

Now that I targeted that "odd" part, should I step back to the meshing and mesh that part with finer elements, OR setting a velocity limiting as you proposed? How to do so? Thanks!

[Rob]

You really need a finer mesh everywhere. Refining that region will help for now but I suspect the problem will move elsewhere.

[Jason Sum]

Thanks Rob! I will try to refine the whole model first! By the way, I would like to ask for such huge model (a underground gas pipe network with ~100m long, 12'' diameter), how or any indicators to determine a proper element size of the whole model and how fine should I adjust?
Should I keep inflation meshing layer of 5, and refine the body sizing?
Will it be better if elbows are having especially finer meshing?

[Amine Ben Hadj Ali]

anyway where you expect rapid changes and steep gradients keep the resolution fine enough to avoid huge jumps!

[Jason Sum]

Okay! Thanks Amine! To obtain a desirable meshing quality, should I keep trial and error to review the residual convergence from calculation on Fluent? If convergence doesn't reach in residual graph, am I supposed to return to Meshing step to refine the model? Once convergence reached, meaning the meshing size and density are enough?

[Rob]

Sort of. You have to resolve the flow (and gradients) spatially (mesh) and temporally (time step) so it's a bit more complicated. Adding in secondary phase(s) makes it even more fun. You have a relatively small system, so we'd model with a lot of mesh: if you extend to kilometres of pipeline we'd switch to a network model. Twinbuilder or Modelica are the Ansys tools, but industrially (oil & gas) OLGA is used for that type of simulation. We may then couple into OLGA for complex components.

[Jason Sum]

Got it Rob! Now I am refining the mesh, I found some elements having extraordinary skewness (shown in red), what should I do to specifically resolve them? Thanks!

[Rob]

Have a look to understand why they're skew: I'd not expect the mesher to struggle with the CFD settings in a pipe!

[Jason Sum]

By using standard version, I have already meshed the whole pipe network with way finer body sizing meshing with 5 layers default inflation, while the elbows and tees were refined with more fined surface sizing meshing.
Body meshing element size : 3e-2
Elbows and tees element size: 5e-3
Node: 2635812
Element: 7373330
Quality Mesh Metric:
Orthogonal Quality: mainly ranging 0.75 - 0.9
Skewness: mainly ranging 0 - 0.25

Hybrid Initiation with water patched inside the pipe model
Method: PISO
Control: Default Under-relaxation factor
Boundary Conditions: 3 Inlets with each 5 psi Nitrogen gas pumping into the pipe network to simulate pumping water out of the only outlet
Time Step: 200
Time Step Size : 4e-5
Max iteration/time step : 40
1st iteration :Global Courant Number [Explicit VOF Criteria] : 5.1802
1189th iteration : Global Courant Number [Explicit VOF Criteria] : 2.24168

Below is my residual graph of calculation from 1st to 1189th iteration. Here are two questions hope for answer! Thanks!!!
I would like to ask, after refining, is the residual graph below satisfactory and is it reaching convergence?
When every time step complete, I saw it showed "solution is converged", does this indication mean my setup already having reliable simulation and obtaining residual convergence

[Rob]

Please post a couple of screen shots from the movie - I'm not permitted to open it.
If every time step is converging then there's a good chance the solution is reliable. However, you also need monitors of mass etc to confirm.

[Jason Sum]

Nearly 500 iterations

[Rob]

Looks reasonable. How are the balances, and how sensible do the results look? Note, inflation tends to result in a fairly high aspect ratio which then causes problems, you may find you need to resolve near the wall and in the streamwise directions at much the same resolution.

[Jason Sum]

Okay! I will try resolve the inflation parts.
By the way, how can I check the balance?
Also, now actual physical flow time merely = 200 x 4e-5 = 0.08s, which actually need wait for the computer to run for about 36 hours
In my case, what do you suggest so that the calculation can be way faster? (Like reduce meshing density or any other possible solution?) I am only having 6 core and GeForce GTX1650 4GB equipped. Thanks!!

[Rob]

36 hours isn't too bad, other than more parallel & faster cpu there's not much you can do. Using a coarser mesh will speed things up, but you'll just produce rubbish faster. Some models run in a few 10's of minutes, others can take several weeks or even months: CFD isn't always a quick process.
Re the balance, you need to look at the mass fluxes and volume integral: what goes in must come out or add to the volume mass.

[Jason Sum]

Two questions would like to seek for your further help:
I have set 4 parallel solver in the box before launching fluent, which made my fluent calculation faster! Now 0.08 s real world simulation only took around 12 hours! I would like to ask what parallel means, does my 6 core cpu mean that I can set max. 6 parallel solver?
Below is my calculation using 4 parallel solver:
Time step size: 3e-5
Time step: 200
Max. Iter/time step: 40
1st Iter: Global Courant Number [Explicit VOF Criteria] : 5.18633
last Iter: Global Courant Number [Explicit VOF Criteria] : 1.42208
2. I have also plot a mass imbalance graph during calculation, based on the below graph and above transient residual graph, do you think the setting is now reliable with residual convergence and I should keep this setting? Many thanks Rob!!!!!!

[Rob]

That looks promising, but you'll need to check velocity etc and that the results make sense. It's hard to give a definite answer without reviewing the case and we're not able to do that.
Re the cores. The solver has 4 cores parallel as part of the Student licence. So that's the limit. Research and commercial licences also allow access to (additional) HPC packs so you can run many cores depending on the number of packs that are bought.

[Jason Sum]

same way as monitoring above mass imbalance to monitor by plotting graph of the velocity magnitude?
in case without educational license limit, say a 6 core cpu at most can have how many parallel solver? Six? Thanks!!!

[Rob]

On your machine, with a suitable licence, 6 would be the maximum. Depending on the cpu and boards you should see good (near enough linear) speed up. To give you an idea KAUST ran on 200k cores a couple of years back: we run 2-300 cores regularly here.

[Jason Sum]

Now that the residual convergence and mass imbalance were deduced to be reasonable, for checking the velocity or other variable, should I plot to monitor them just like monitoring mass imbalance, OR just observe their range in cell register? Thanks!

[Rob]

Just monitor. In CFD we monitor residuals, monitors and fluxes. Once the computer says the model is done we also manually check the result: that is to check that the result is "correct" as the other checks are that the solver has done it's job, not that the boundary conditions etc are sensible.

[Jason Sum]

Thanks Rob! To monitor other field variables and fluxes for ensuring an accurate result, what should I select (e.g. surface/volume integral / average / mass / mass integral...) to observe relevant variables?

[Rob]

Yes! I tend to monitor velocity/temperature/phase on a point to see how much it's changing. Your case is more complex as you may have several phenomena interacting at different frequencies.

[Jason Sum]

I dont know why after the simulation, the animation of velocity magnitude contour does not shown any gradient changes on wall, only inlets showing the velocity gradient, is there anything wrong?

[Amine Ben Hadj Ali]

Check the underlying objects behind that velocity animation sequence.

[Jason Sum]

I already selected all inlets, outlet and wall of the model for the velocity magnitude,. Suppose the pipe contains some water inside, if inlets having pressure pumped inside, there should be water movement and velocity gradient changes showing, but throughout the animation stored, the wall of model keeps in blue colour. Thanks for help!!!

[Rob]

What should the fluid velocity be at the wall? Think carefully! Try the same plot with node values off.

[Amine Ben Hadj Ali]

If you select velocity contour at just inlet what do you see? Velocity is zero at walls if they do not have motion. What are your Inlet boundary conditions?

[Jason Sum]

Thanks both of you!
In the velocity contour, I saw the inlets (cross section of pipe) having velocity color gradient changes!
My boundary condition:
Three risers inlets each having 5 psi total pressure with nitrogen pump in.
I ran the calculation again by plotting a graph of Area weighted average velocity magnitude of mixture at the point circled below.
I would like to ask after obtaining the graph of velocity at a point, how can I determine it makes sense and it is a reliable result?
The point:

[Rob]

Compare the monitor with expected values. If the result is converged the value will be numerically correct, but you'll need to apply good engineering to confirm the results are physically sensible for your intended settings.
It's the old question. We test the solver, so we're confident the result is correct. What we can't say is if you put all the boundary conditions & material properties in correctly.

[Jason Sum]

Okay Rob! I will confirm the result by apply own engineering calculations and sense.
I ran a calculation with time step size of 3e-5 with 400 time steps, and max iter of 40.
The first graph below shows the 900 iteration is seemingly converging for transient, but when it keep calculation further with increasing iterations, for 2nd graph, the 0-900 iterations already not same as the 1st graph. 0-2000 iterations in 3rd graph even seems like being skewed. What's wrong with it and why? Thanks!!!

[Jason Sum]

Sincerely seeking for answer with many thanks!

[Rob]

Yesterday was Sunday: I only work for my wife on Sundays.....
It's data retention, Fluent stores the last 1000 (by default) residual points so anything beyond that may look a bit odd. Nothing to worry about.

[Jason Sum]

Ohh!! Sorry Rob! I mess up with the time difference!
thanks for your professional answer! You helped a lot! Have a good day!

[Rob]

:) Thanks, you too.