Not all flows have a steady-state behavior.

Otherwise the convergence history could potentially depend on mesh quality as well (orthogonality, skewness, aspect and volumetric ratios,...).

I can only guess, that you are trying to simulate this in steady-state.

Have you tried with Coupled Solver, HOTR=on, Pseudo-Transient and by increasing manually the pseudo-timestep? How is that influencing the result?

How convergence behaves, if the same flow is simulated in transient mode with statistical time-averaging of results?

Regards,

Dr. Th. Frank.

Dear Thomas Frank,

I am running a steady-state solver for now.

Here is the Mesh property:

Domain Extents:

x-coordinate: min (m) = -5.000000e-03, max (m) = 5.000000e-03

y-coordinate: min (m) = -5.000000e-03, max (m) = 5.000000e-03

z-coordinate: min (m) = -2.500000e-01, max (m) = 2.250000e+00

Volume statistics:

minimum volume (m3): 2.393006e-13

maximum volume (m3): 1.788831e-09

total volume (m3): 1.892667e-04

Face area statistics:

minimum face area (m2): 2.174882e-09

maximum face area (m2): 1.525866e-05

Checking mesh.....................................

Done.

Mesh Quality:

Minimum Orthogonal Quality = 2.12420e-01

(To improve Orthogonal quality , use "Inverse Orthogonal Quality" in Fluent Meshing,

where Inverse Orthogonal Quality = 1 - Orthogonal Quality)

Maximum Aspect Ratio = 5.44563e+02

I will try coupled solver, Pseudo transient., High order Term relaxation of 0.25 for mas flow and the rest will be set on automatic.

I will upload the results as soon as obtaining them.

Thank you Dr.Thomas Frank .

Dear Dr. Thomas Frank

I have uploaded the residual behavior of the mentioned case.

The pressure and momentum under-relaxations are 0.5.

The HOTR is turned on with a factor of 0.25 for mass flow, also the warped -face Gradient correction is enabled.

The 1st order upwind is used for all equations.

So the wiggels in the residual history are gone. But to me it seems, that the simulation has not been carried long enough forward so that the solver could finally converge. At N=500 the residuals start declining, but there the simulation run ended.

Questions:

1) What was the used (probably automatic) pseudo-timescale? You can make this printed to the Fluent transcript by setting verbosity from 0 to 1.

2) What is the characteristic throughflow time of your geometry? This can very roughly been estimated by calculating:

T_char=L_char / U_char

where l_char is the length of the main flow path through your geometry and U_char being the mean flow velocity.

Then the following relation should be satisfied:

N * dt > 5 * T_char

where N is the number of iterations (here N=500) and dt the applied pseudo-timescale of the solution method. Is that the case? The factor 5 is purely empirical. Essentially it means, that the fluid needs to pass the geometry from inlet to outlet approx. 5 times until you can expect solver convergence. It strongly depends on the geometry and the nature of your flow, recirculating and dead-water zones, areas of slowely ongoing processes, eventually the slowest physical process in your configuration detemines that number. The slowest participating process can e.g. be heat conduction in adjacent solid zones, if CHT (conjugate heat transfer) is included in your setup.

In order to accelerate the convergence you can play around with underrelaxation factors and the manually set pseudo-timescale. It could potentially work to increase the URF's from 0.5 to 0.7 or even 0.8. And you can try to manually increase the pseudo-timescale dt as long as solver stability is maintained.

Regards,

Dr. Th. Frank.

Dear Dr. Thomas Frank

The solution has converged! I had set the Dt for the fluid part as 0.05.

Furthermore, The Pseudo-timescale for the solid part was set to automatic.

The Under-relaxations for pressure and momentum was the default value (0.5).

Moreover, The first order scheme is used.

The convergence criteria were set to 1E-06 for mass, momentum, and energy and 1E-03 for turbulent parameters.

Thank you for guiding me through it. But, there is an issue. I assume that for a fully-developed flow, It might be a wrong criterion though, the velocity profile should overlap on a line perpendicular to the center of twisted-tape (at pi/2) for each full rotation of twisted tape (2pi rotation) which is not met by the results. I wonder what may be done to resolve the issue.

The geometry consists of a 25 cm long entrance tube and an outlet section of 25 cm for reducing the reverse flow problem in the outlet which there is no heat transfer in these sections. So the 45 in the second figure indicate 20 cm in the test section which is equal to 2 times the length required for twisted-tape to fully rotate

Kind Regards,

So this result looks pretty much converged now and convergence level should be deep enough.

But we have not yet spoken about mesh resolution, mesh refinement and about carrying out a mesh independence study for the obtained solution. This is just a single result on a given mesh. But how the solution will change with mesh refinement then?

And this is a flow with strong streamline curvature. I guess, that SST model is used. But has the curvature correction term option been activated to account for strong streamline curvature in the twisted geometry?

Furthermore it can only be expected that velocity profiles are identically matching, if fully developed flow conditions have been achieved. For turbulent flows this is usually the case after an L/D~30. So I would guess, that at 20cm behind the start of the twisted tape and having a tube diameter of 1cm the fully developed flow condition at this point (L/D~20) has not yet been achieved.

And are you sure that by chance you have not made a mistake with the green curve here in the diagram. If I look at the other three colors, than I can at least see a kind of an asymptotic and monotonic change, which seems to correspond to some flow development over the length of the pipe taking place. But the green curve is not matching at all. And the integral below the curves (if they are taken at an identical positioning of the twisted tape with regard to the cross-section) should be proportional to the massflow rate through the pipe at this point. Correspondingly the integral over the curves should be more or less equal because of mass conservation (same massflow rate through the cross section). This is not 100% true for a line diagram and a 3-dimensional flow (no symmetry over the 360 degree circumference), but at least an indicator for plausibility. The green curve is not plausible in that sense.

And what about near wall resolution in terms of y+ values at the walls. In which region we are in terms of y+. For flows with heat transfer one should strive for a y+~1-2 at heated walls and at least 10-15 mesh cells spend for boundary layer resolution. Is that the case here?

Regards,

Dr. Th. Frank.

Thank you again, Dr. Thomas Frank.

I will check all the hints and post the results as soon as possible.

Regards,

Dear Dr. Thomas Frank

Firstly, I do apologize for the delay.

Since I was running the case with "Outflow" for outlet boundary conditions, the solutions diverged after some iterations. By changing to "mass-flow-outlet" the issue was resolved. I have set the Pseudo time steps as 0.01s and have run the computation until the convergence criteria were met.

The Figure shows mass and momentum have converged to 1E-06. The solution method was PRESTO for pressure, QUICK for momentum, and the 2nd order for other things.

Currently, I am doing the calculation on a finer mesh to see where it leads. i will upload them as soon as possible

Convergence looks very good now. Good work.

Regards,

Dr. Th. Frank.

Dear Dr. Thomas Frank

Is it possible that this flow never becomes fully-developed?

Cause the velocity profiles still vary by far.

Regards,

Hi,

not sure about fully developed flow. I have not yet seen the geometry and I have not yet seen the details of the mesh, in particular with respect to cross-sectional resolution and resolution of boundary layers.

BTW what about the intended mesh independency study - how you intend to run this? What is the hierarchy of meshes with their mesh resolution and what are the corresponding max. y+ values? And for the chance of a fully developed solution we would need at least an L/D~35-50.

Best regards,

Dr. Th. Frank.

Hello dear Dr.Thomas Frank

Geometry details:

The tube length is 2m.

The diameter is 1cm.

The twisted-tape thickness is 1mm.

Mesh details:

The mesh is composed of 15 elements with bias 2. Then it is 20 elements and another 20 elements in the middle. And 500 number of divisions in the axial direction.

max y+ on the pipe walls and the twisted tape surface?

The "ttsurface-yplus-rfile.out" is the averaged y-plus on twisted tape and the "innerwall-yplus-rfile.out" is the y-plus on tube wall.

ANSYS Fluent 18.x is almost 4 years old. A lot of improvements have been made since then (actual version is 2020.R2).

Difficult to judge from the given information on how further improve this simulation. The mesh generally looks good (some larger jumps in cell volume observable at certain block boundaries of the structured mesh, but should not be critical). y+ in the range between 0.9 and 3 looks good to me as well. Nevertheless it would be interesting of what can be observed, if the mesh is refined by a mesh cell count of at least 4 (in total) or even 2x2x2=8, i.e. division by factor 2 in each coordinate direction. Not sure, whether your computational capabilities allow for that....

Is SST with curvature correction option acvtivated?

Regards,

Dr. Th. Frank.

Dear Dr. Thomas Frank,

Since I am using the coupled method and pseudo transient method, there is no "curvature correction" option as there is in other pressure-velocity coupling methods. However, there is a "Warped-Face gradient correction" option which I have activated in my runs.

Additionally, I will try to further reduce the mesh elements size and upload the results as soon as possible.

Furthermore, is there any lowest element size limit for mesh elements in the RANS method; By this I mean, is it possible that the reduction of mesh elements size beyond a certain value cause error?

Thank you for walking me through challenges.

Kind Regards,

Dear Mr. Eshagi,

"Curvature Correction option" is not a property of the solver or the pressure-velocity coupling scheme. It is an option in the viscous models --> k-omega models --> SST (shear-stress transport) turbulence model (checkbox on bottom left of the corresponding Fluent panel). This option exists independently from the selected solver method. And it should be activated for all flows with strong streamline curvature.

For the mesh element size there is no lower limit besides the representable number accuracy limit of a computer. With double precision floating point numbers there are 14 significant digits available. Mathematically speaking the iteration error of a discretization method of 2nd order accuracy is epsilon~O(dx^2), where dx is the length scale of the mesh element. Therefore, if the mesh elements are divided by a factor of two, than the error reduces by a factor of 4. 2nd order upwind schemes are usually not of full second order accuracy (as e.g. a central difference scheme), correspondingly the error reduction is less than the factor of 4, but better then factor of 2 (which would correspond to a 1st order discretization method).

Best regards,

Dr. Th. Frank.

Thank you,

The previous results were obtained by the RSM method. Should I instead do SST-k-omega with curvature correction?

Yes. Please give SST turbulence model with curvature correction a trial. It would depend on which of the half a dozen different RSM models in ANSYS Fluent you had activated. The most reliable in my opinion is the k-omega based BSL RSM model. But it would be good to know what SST+curv.corr. is doing for this case.

Regards,

Dr. Th. Frank.

Merry Christmas, Dr. Thomas Frank

I have run the the case by SST k-omega method using Curvature correction and low Reynolds correction. After convergence, the velocity profiles on aline perpendicular to the twisted tape in the teta=pi/2 are given in the figure,

the mass imbalance was in the order of E-14.

The outlet boundary condition was mass-outflow.

the tube consists of 25 cm of the adiabatic inlet, 200 cm of the tube with twisted-tape which the tube wall is at 350K, and there is another 25 cm of the adiabatic tube.

I wonder what is the reason for such a velocity deviation?

Hi,

without being able to analyze the CAS/DAT file directly it is almost impossible to diagnose this from the distance.

You are not giving your own interpretation here. So I can only reflect, of what I can interpret from this one single picture. The velocity profiles for cross-sections 065 until 195 seem very reasonable for me. Only the last two cross-sections at 205 and 215 seem to show non physical behavior.

Question: Have you calculated the throughflow time of the fluid flow through your flow configuration from the inlet to the outlet? Lets assume a block profile velocity at the inlet and the length of the geometry of 2.5m. How much iterations in the pseudo-transient timestep method is it taking that the fluid is passing this flow geometry at least 2-3 times? What happens to the last velocity profiles, if you run the simulation for another couple of 100*dt? Changing towards the fully developed velocity profiles at e.g. L=195? Not changing at all?

T = N * dt ~ 3 * 2.5m / U

N ~7.5m / U / dt

Have you calculated this flow at least for the resulting number of pseudo-timesteps? Or have you stopped the simulation already earlier? If yes, than this could explain, why the last 2 velocity profiles could still be affected by your settings for the flow initialization, i.e. the initial guess for the flow field, since the state of the fluid flow at T=0.0s has not yet "washed out" completely from this long geometry through the outlet cross-section.

If this is not the case, i.e. you calculated it already for a larger number of pseudo-timesteps N, than honestly I do not know from the information which I have.

Regards,

Dr. Th. Frank.

Dear Dr.Thomas Frank,

Firstly, I humbly appreciate that you are still helping me through my problem.

Secondly, the initial condition was set as the inlet condition which is a constant velocity of 1 m/s. Furthermore, the solution was converged after approximately 1750 iterations with a time-step size of 0.01s. 17 seconds should be more than 5 times of flow passage time??

Additionally, the 25cm of extended geometry, at inlet and outlets, do not have a pitch ratio. in other words, they are a tube with a straight tape extended orthogonal to the plain which the twisted tape ended (The extrude function is used in the production of this geometry).

I guess velocity profile behavior might have something to do with the damping of vortices coming out of the twisted-tape part; so the velocity profile is changed in the downstream section due to the need in the upstream which is outlet condition with a constant massflow perpendicular to the outlet.

Kind Regards,

Mahyar SeydEshaghi

Let me re-run the case with brand new geometry, maybe I have done something wrong in those steps. I will post the results as soon as it is done.

Dear Dr. Thomas Frank,

I have done a series of computations on the discussed case; however, I have replaced the working fluid, which was water, with a more viscous fluid, Ethylene Glycone.

The following meshes provided a fully-developed flow pattern. I guess the viscosity somehow dampens the turbulency and provides more accurate results.

I wonder what could be done for cases with water to refine the results?

Kind Regards,

Mahyar SeydEshaghi

By the way, In cases with water, I have tested reducing time steps to 1/10 of their value when the shear stress and outlet temperature reach a constant value, it helps to reduce the residuals and to haste convergence.