open TELEMAC-MASCARET The mathematically superior suite of solvers

Hello,

in a rather simple case, rectangular 25 m long channel, with v7p1r1 and k-e model, MURD scheme (4) for velocities, k and e, I'm not able to get a steady state flow field. It is really weird and I tried a lot of different options.. time step, boundary conditions for turbulence, etc. I cannot figure out what is going on. And the strange thing: v6p3r2 converges very well with the same steering file, (besides some different names for some keywords)

Enclosed the test case and I would be very glad for any hints.

Best regards,
Clemens

Hello Clemens,

I had a quick look at your case, which runs without problem (with the trunk version) and seems to converge, at least if you look the discharges at the entrance and at the exit, which tend to be the same. Could you then explain what is the hint that tells you that it has not converged. A remark is that very often the solvers converge in 0 iterations (especially the k and epsilon diffusion equations), which is a hint that either you converged, or your time step is too small or the requested accuracy is not enough.

My only similar experience was a long time ago with a backward facing step. The k-epsilon model did some vortex shedding after the step and never reached a steady state. This is also obviously the case with bridge piers. It is however strange with a straight channel. A possibility is that there is a longitudinal resonance that takes time to fade away or which is somehow maintained by the boundary conditions (maintaining a steady discharge at the entrance while the elevation may change freely is perhaps not a real behaviour).

Of course all this does not explain the differences between different versions.

With best regards,

Jean-Michel Hervouet

Hello Jean-Michel,

thank you for the answer.
To explain: with convergence I mean the convergence to a steady state for all the variables involved.
Indeed I had the same idea and tried the trunk version, and it worked, like v6p3r2! So what I figured out: when I use a liquid boundary file with a ramp function for the discharge, v7p1r1 doesn't reach a steady state. Turning off the liquid boundary file solves somehow the problem! Other remark maybe related to this: using the liquid boundary file, in the first iterations I get such messages in the listing:
GRACJG (BIEF) : SOLUTION X=0 BECAUSE L2-NORM OF B VERY SMALL: 0.000000
which disappear with increasing discharge after some time.
However it is to say that I get this message also with v6p3r2 and the trunk version.

Other observation: turning on the computation of k and epsilon at the inlet via a linear profile over the depth, both the versions v7p1r1 and the trunk version cannot reach a steady state, independently of the usage of the liquid boundary file or not. I don't know why since in other very similar cases it worked like a charm. Maybe it is related to the number of vertical layers.

Best regards,
Clemens

Hello again,

reviving this flume case:
when I turn on the computation of k and epsilon at the inlet via a linear profile over the depth: OPTION FOR THE BOUNDARY CONDITIONS OF K-EPSILON =2, no steady state is reached, independently of the time step used.
Decreasing the relative accuracy of k-eps from the default value of 1.E-6 to 1.E-12: ACCURACY FOR DIFFUSION OF K-EPSILON = 1.E-12 solves the problem and a steady state can be reached!
Interestingly I can reach a steady state when using the min values for k and eps at the inlet OPTION FOR THE BOUNDARY CONDITIONS OF K-EPSILON =1, using the default accuracy for k and eps.
However I cannot figure out what are the reasons for this different behaviour. Maybe it is related to the really small absolute threshold values for k and eps but in terms of the relative accuracy it shouldn't matter?

Best regards,
Clemens

Hello Clemens,

Yes, I am also working on a case without tidal flats and TREATMENT OF NEGATIVE DEPTHS = 2 triggers a crash when there is not enough accuracy. Logic becomes very fuzzy when accuracy is too rough... In my case the approximate velocities create wrong free surface gradients when the continuity equation is redone at machine accuracy.

JMH

Hello Jean-Michel,

indeed the combination of the threshold values / limiters and the specified accuracy is quite tricky. So also my previous post was apparently not the end of the story. What I observed was that the simulations using the default limiters for k and eps, KMIN and EMIN, induce some spurious turbulence at the inlet, in terms of turbulent viscosities. With the default KMIN and EMIN values the calculated turb. viscosity is higher than the laminar viscosity. Especially near the inlet, the simulation, in terms of k and eps, didn't converge. Changing the accuracy for k-eps didn't help that much.

I did some tests with the limiters and I propose to change the minimum value KMIN from 1.E-10 to 1.E-20. The simulation converged perfectly in every node. This sounds plausible since with KMIN=1.E-20 the computed turb. viscosity is much lower (=9.E-26) than the laminar viscosity which, in my view, should be the case in a node with KMIN and EMIN.


Best regards,
Clemens

Hello Clemens,

Waow ! 1.E-20 ! what happens with the term epsilon/k in the equation of epsilon ? It will create a lot of epsilon ? Actually the problem is also with tidal flats and we would need a lot of cases to be sure. I will see a specialist next Friday and will ask him what to do. I am afraid that nobody really knows how k-epsilon can work with the size of our elements, with large aspect ratio and with dry nodes... we are in terra incognita.

Regards,

JMH

Hello Jean-Michel,

hm, at least in this case it works, with epsilon not flying away.

To reformulate it: I propose to test the lower KMIN value on other cases.

Furthermore related to such testing it would be interesting to revisit the boundary condition treatments of the k-e model in Telemac-3D.
I have to say that with the latter proposal I don't want to say that the k-e model in Tel3D performs "bad". Actually it works really good in terms of the computed k, eps and viscosities compared to analytical formulas and other CFD packages.

Best regards,
Clemens

Hello,

maybe my suggestion to lower KMIN to 1.E-20 was really a little bit over-hasty.
But my viewpoint stands: the default values for the limiters KMIN and EMIN create spurious oscillations at the inlet zone and there is no way to get rid of them, besides changing those limiters. And for a user this can be very annoying.
I tested the combination of KMIN = 1.E-12 and EMIN = 1.E-14 (which give neglible turbulent viscosity at the inlet) with some different setups and Telemac does a really good job.

Best regards,
Clemens