Unbounded advection discretisation
 

I am new to both CFX and, in general, CFD and am working on a multi-component flow simulation. I have a fluid pair of nitrogen and a custom fluid "Mixture", which consists of hydrogen peroxide and water. The fluid Mixture was defined as a variable composition mixture.

The premise is to simulate an injection of 8% hydrogen peroxide into a large vessel, which also experiences nitrogen sparging, and to then run a transient simulation to see how long it will take for the vessel to be a uniform 8% peroxide (initial conditions of 0% peroxide, 100% water). I had been using an upwind advection scheme in order to produce converged results. However, I have been having problems converging and recently read that the upwind scheme may be the reason if a mesh is too refined. I then tried to switch to a specified blend factor of 0.8, but got the below error when running the simulation in -Solver:

"An unbounded advection discretisation scheme was specified for the transport equation of a bounded variable. The advection scheme is changed to a bounded scheme." The "Effective adv. scheme" was subsequently switched to High Resolution

I didn't see an explanation for this in the help files and would appreciate any thoughts.

Thank you.

Hi,

First order upwinding is very diffusive and can give erroneous results. That is why it is not recommended for almost all applications. They are however very easy to converge so can make good initial guesses. Second order schemes are much less diffusive but have boundedness problems. To counter this problem CFX has a hybrid scheme where you can use a bit of first order to stabilise it. An alternative approach in CFX is to use the high-res differencing scheme which has a limiter built-in to try to reduce boundedness issues.

Looks like you are having convergence problems when you move from upwinding (easy to converge but inaccurate) to second order (hard to converge but more accurate). Try smaller timesteps and/or tighter convergence and lots of other things but we'll do those first.

Glenn Horrocks

Thanks for the additional information. Two more questions:

1.) Irregardless (for the purposes of this question) of my convergence problems, why was I unable to use the Specified Blend Factor advection scheme for my multi-component flow? When switching from upwind, I had initially specified a blend factor of 0.8, but -Solver immediately switched me into the High-Res scheme (see error message from original post). Is there something about multi-component flow that does not allow use of the specified blend factor?

2.) I have been playing around with reducing the timestep, etc, and am now in a place where my transient solution converges under the High Resolution scheme to RMS<1e-4 in 6 coefficient loops with a timestep on the order of 0.002sec. Unfortunately, I am looking to run at least an hour of this transient simulation, which will take weeks if things continue at this rate (my domain is ~3 million elements). Is there any information on what precisely is "inaccurate" about the upwind advection scheme? Essentially, I am looking to find out if there are any areas in my domain that are not mixed as well as others. If I can obtain this information using the upwind scheme, I can likely get there a lot faster. Or, is upwind so inaccurate that even general solutions are not usable?

Specified blend is not bounded, mean that you can have numerical wiggles. E.g. mass fraction can get smaller than zero or larger than one resulting in unphysical states. Clipping can not heal that in any case. At my phd times I struggled a lot with that issue in my inhouse code.

Possibly there is upper limit for the blending within highres. Have look at help or ask the support. Please post if you find something.

Hi,

Any decent CFD text should discuss the pitfalls of first order upwinding. The classic text on CFD accuracy is "Computational Fluid Dynamics" by Roache - this text discusses accuracy issues far beyond first order upwinding.

If you use upwinding for the mass fractions you will get additional mixing effects caused by the diffusive nature of the first order scheme. Whether that is a problem or not depends on what you are trying to do. If you need concentration gradients to remain sharp then upwinding will not work. From reading your description above the mixing rate is the key parameter in the simulation so that means upwinding will be very inaccurate.

You got convergence problems with the hybrid scheme using a blend of 0.8 because it is using 80% second order and 20% first order differencing and the second order differencing is unbounded and (in your case) causing convergence problems. That's why I recommend the high res scheme as it keeps boundedness - but it is still less stable than upwinding so will be harder to converge.

The simulation run time looks long? Welcome to CFD - that's why CFD uses supercomputers. I suspect if you use adaptive timestepping after the initial transient is done it will be able to speed the simulation up, but still I would count on a very long simulation.

Glenn Horrocks