Segregated or Coupled flow?
 

Hey everyone,

I have a query. What is the difference between segregated flow model and the coupled flow model? I mean I read the technical details in the guide but which one is better? do they have specific uses or is there a difference in the computation time or the accuracy ?

I am asking this because I meshed my geometry once with tetrahedra and once with polyhedra cells. The tetrahedra mesh works fine with segregated model and crashes when i use a coupled flow model with it.

and its the other way round for the polyhedra mesh. it works fine with coupled flow and not with the segregated model. is there a problem with my mesh or are these physics-models mesh specific?

thanks,
hamza

Coupled flow needs more resources like memory and computational time as it solves coupled equations for pressure and velocities. But that also means, it's more stable in cases with high density fluctuations like supersonic flow with shocks etc. My experience is, it's not the best choice for a standard case as it might be unstable unless you reduce the courant number a lot.
And in theory the number of steps it takes to solve a mesh doesn't depend on the cell count. Practically it still might need a huge number of steps until you get a solution.

Segregated flow is a good choice for most cases. It runs fast, but can have problems with supersonic flows. And the bigger the mesh, the more steps you need as some information has to cross the domain several times.

So far this should be nothing new, it's all in the user guide. But anyway I'm feeling like a Tibetan prayer wheel. I have to repeat again and again: Which one is the better depends on your application! Just think: What's better, a heavy lorry or a Ferrari? Depends on if you want to race your friend or if you have to bring 20 tons of beer to a party...

For sure there's nothing like "coupled for polys, segregated for tetras". Both solvers are working with both mesh types. It just depends on your physical phenomena and your solver settings. For example, a courant number of 5 (default on the coupled solver) might be too high to start with and the coupled solver also needs a reasonable initialization.

But what I can't understand is why you are using a tetrahedral mesh.

Thanks for the information adbul.

I made the tetrahedral mesh using another software(Ansa). My company asked me to do so and I just wanted to do some meshing with starccm so I generated a polyhedra mesh of similar fineness, just to see the effect of mesh-type on the simulation.

Although I faced a real tough time trying to repair the mesh in starccm. I was trying to bring the maximum skewness angle in the entire mesh below 85 and I also had some problems with some pierced edges. Thats the reason I asked could it be because of the mesh quality that one of the models doesnt work.

What type of mesh do you recommend for an egr system?

Okay, a customers requirement is a good reason to use a tetrahedral mesh - although it's not the best requirement they could dictate.

Well, bad cells could be problematic with any solver, although the segregated solver is more robust in my experience.
No matter which solver you are using, it's nearly always worth to invest more time to get a better mesh. (Better means better quality, not necessarily a finer mesh)

For most cases I would recommend a polyhedral mesh, that's suitable for most cases. A tetrahedal mesh doesn't provide any advantage further than the shorter time for meshing. A polyhedral mesh needs less cells for the same geometry and is better for numerics.
In some cases it might be good to have a trimmed mesh, for example when you've got a flow strongly aligned to the mesh lines or when morphing is involved. But as I mentioned before, for most cases is polyhedral mesh is fine.

Cheers

Thanks abdul!

As i said I had problems generating a good polyhedra because of the high skewness angle and I was facing some problems repairing it so I increased the fineness of the mesh. Anyways thats not the main problem that I am facing right now.

Its the residuals. They are just way too high. The simulation runs good for as many cycles I want but the residuals are of the order 10^7 for tke and sdr...

I tried playing with the turbulence length scale. I reduced it to .2 mm from 2 mm. It only reduced the fluctuations from one iteration to the other.

The residuals remain pretty much constant but they are too high. what could the problem be?

If you want more details about my mesh and physics model let me know...

thanks,
Hamza

Well, the quality of a mesh always depends on (but not only) user input. When the mesh quality gets much better with a refined mesh, that's an indicator for bad values (e.g. too big surface sizes etc.) in many cases.

Residuals in CCM+ are normalized within the first 5 iterations. Therefore the level of the residuals depends on the initialization values and the solution itself. A high level for residuals doesn't necessarily mean, your solution is bad.
When you would use the current solution as initialization and keep on running the simulation, your residuals would be normalized to the current values and therefore be pretty much around 1, but the solution itself would be the same. So what's the point? Lower residuals don't necessarily mean, the result is better - at least as long as the residuals are normalized.

Don't give too much on residuals. More important to check your results carefully. Check for unrealistic values, monitor some engineering data and compare it to reliable simulations or experimental data. The highest residual doesn't harm when you've got a perfect solution. And the lowest residual is pointless when you"ve got a fluid velocity above the speed of light or a perpetuum mobile...

Hey Abdul,

Thanks for the reply man. I did try playing with the initial values and I did get the residual to come down a little...still i have the tke and sdr values in some thousands...

I always monitor the massflow at the inlets and outlets and there is no problem with that..

I was only worried that since residuals denote the magnitude of error in the solution, so a high value would mean that the solution is useless....

That would be right when the residuals wouldn't be normalized. But as they are, the level of the residuals is more or less meaningless while the history is more important (especially in unsteady simulations, to check whether a time step is fine or needs further iteration). But even that shouldn't cause headache, as all depends on inital values.