I'm running a pretty standard 2-D axisymmetric model which involves a pretty sharp and severe constriction (a larynx model), causing a jet and some backflow. When I run the model with any of several turbulent viscous models-- S-A/ RKE/ KWSST/ Reynold's Stress-- it converges, at least to a reasonable scaled amount (1e-4 -- 1e-8) .

When I run the laminar model for comparison, it completely fails to converge. Often times, it converges to 1 e-1, (overally continuity) and then begins to diverge, to some other very high value, before stabilizing. It never completely converges.

Given that the turbulent models converge, I'm confused as to why the laminar model does not. I've tried adding reasonable boundary layers, switching to second order solvers, and increasing my grid definition-- and some of these techniques have helped a little, but the overall problem of the laminar model continues. I'm thinking maybe the fact that there are interior boundary layers (from the backflow cells) could be causing some resolution issues in the laminar case.

Is there anything I can do to force my laminar model to converge in the same manner as the turbulent models do? I really need the laminar as a standard of comparison for turbulent data-- my flow is really somewhere in between.

The only way to deal with laminar simulations that do not converge using standard approach (steady solver), is to switch to unsteady formulation and run it until settling down. I personally ran into this problem many times by now and this has been a fail-proof method. Of course, this means some significant more computational effort, but be patient. The explanation for this behavior of the laminar solver is the fact that the laminar regime N-S equations are not time-averaged, so whenever a strong unsteady phenomena appears in a model, it's beeing felt immediately. Try for example to simulate Re=200 circular cylinder flow with the steady solver. Vortex shedding will never permit it to converge. The reason is simply phisical.

All the best, Razvan

switch from outflow boundary to pressure outlet, and it will not diverge.

Thanks for the suggestions. Zxaar, as to the pressure outflow, I'll try that now.

Razvan, when you say that I should use the unsteady solver, what kind of settings should do you suggest I use (time step length, total time steps, iterations per time step, etc)?

I don't think zxaar method will fix the divergence problem. I have met the similar case and I totally agree with razvan opinions. It is the underlying physics, not numerical issues. Just my opinion.

Well it all depends on the problem. It's a common mistake to use an outflow BC that's too close to geometry changes and this can cause the model to fall apart. The assumptions behind the outflow BC are pretty limiting (same thing with the Pressure-Far-Field... I know that's off topic, but you routinely see the Outflow and the PFF BCs misused on this forum). And sometimes the Outflow BC simply fails, even if the "fully developed" assumption is applicable. The Outflow BC will definitely fail if there is transient information being passed down stream in a steady state solver. And when I say it fails, I mean it can further excite the upstream effects by artificially back pressuring the system and such. If the "fully developed" solution doesn't work where the BC is applied, the Outflow BC will tend to magnify the problem.

I think Zxaar approached it from looking at what are the common mistakes, and misusing BCs in Fluent are pretty common. Razvan looked at it from a POV assuming that the setup was correct. We really don't know either way. Personally I would try Zxaar's response first (it's easier). Then if that doesn't work, I'd try Razvan's response. Both responses are valuable though.

IMHO of course.

Jason

To add to what Jason said, the problem with using outflow boundary is, unablility to force continuity when the flow enters through the outlet boundary. Usually to match the inlet flow, outflow velocities are multiplied by a factor. Now if the flow enters this could lead to unstablity. To avoid this what Fluent does is, when the flow enters the outflow, it does not enforce total continutiy (in flow = outflow). (According to their manual, the mass flux in such cases is floating or not defined). so when the flow enters and if you are not enforcing continuty, there may be cases where it diverges.

When you are using, pressure outlet, the continuity is applied in terms of pressure and hence the flow direction at outlet won't effect the stablity of solution. (this is why I said switch to pressure outlet).

I have met the similar case and I totally agree with razvan opinions.

First one persons personal experience does not necessarily applyu to every body. For example, I have never had any subsonic case diverged with Fluent. (it does not mean you can not have divereged case with fluent.

As far as getting steady solution by unsteady procedure (incompressible pressure based), could be problematic in some case. For example, flow behind a cylinder, where you have vortices. (waiting for a unique profile in such cases seems very bad idea).

It is the underlying physics, not numerical issues

It may very well be numerical issue, stablity in steady solver could be difficult. And boundary conditions play big role in it.

Compare the size of the turbulent viscosity to the constant laminar viscosity value.

Thanks for all the feedback--

Now, is there a way to use the pressure outlet BC without having to specify a species concentration? For example, I'm trying to run a species balance with flow-- and the standard outflow allows me to leave the outlet concentration unspecified (allowing the solver to calculate it). Is there any way to do the same with the pressure outlet? Every time I use pressure outlet, I'm forced to specify the outflow concentration.

[satyendra]

hi zxaar,

i am trying to solve an incompressible ideal gas problem having two mass flow inlet conditions and two pressure outlet conditions ( i cannot use outflow BC since according to chapter 7, fluent user guide this is not allowed ). hence I have set target mass flow at outlet. But the continuity is not converging. any idea where i am going wrong.

rana

[sanjeetlimbu]

Dear Sir I am trying to do laminar - species transport model

As I tried RNG viscous model- it donot give complete temperature graph.

Please suggest how to set up the laminar - model for combustion using the fluent-chemkin file for four species- N2/AR/Nc6H17/O2
I am compressing the volume by piston in 30 ms and expecting temp to rise above 766K, as I see that Temp donot rise even as piston moves and Pressure rise fro 25-30ms