In this week’s blog post we will take a closer look at some settings for the EMP solver in order for you to be successful with your EMP simulation in Simcenter STAR-CCM+. The EMP solver is one of most complex and sensitive solvers that Simcenter STAR-CCM+ has in terms of convergence and stability. It is one example where the default settings for the solver is neither the best practice, nor even a real option when it comes to reaching convergence in your simulation.
The EMP solver
Let’s recap what the EMP solver in Simcenter STAR-CCM+ is, and what it does. The development of the EMP model in Simcenter STAR-CCM+ was driven by the nuclear industry. The general use of the model is for simulating dispersed flow, like bubbles in water. But in Simcenter STAR-CCM+ the development of the method has allowed for more and more flow regimes, and combinations of flow topology. Where one of the bases for the EMP solver has been population balance modeling (PBM) in Simcenter STAR-CCM+, like AMUSIG or S-Gamma [Population balance in Simcenter STAR-CCM+ – VOLUPE Software]. It is of course also possible to solve problems with another phase interaction topology [Phase interaction topology, interaction area density and length scale – VOLUPE Software], without an explicitly defined dispersed phase. You can employ a multiple flow regime topology and you can even run EMP with LSI (Large scale interface) in a similar manner to what is done for MMP.
EMP is based on a Eulerian-Eulerian formulation, in which each distinct phase has its own set of conservation equations. Phases are considered to be mixed on length scales smaller than the length scales to resolve. What this means when talking about the continuous dispersed topology of bubbles in water, for instance, is that interaction happens for bubbles smaller than the cell-size and hence require closure models to simulate.
The phases are considered to co-exist everywhere in the domain, and even in a location where you don’t have a liquid phase (e.g. above the surface in a water-air simulation) the equations for mass, momentum and energy are solved for both phases. The only field that is shared between all phases is the pressure field. The concept of co-existing phases is called “interpenetrating continua” and assumes that you are interested in the time averaged behavior of the flow, rather than the instantaneous behavior.
Settings for the EMP solver
In this section we will go over some of the solver settings that are recommended to use. Many of these settings are not only recommended settings but are also absolute requirements in order to reach convergence in your EMP case. First, we will look at settings for multiphase interaction together with boundary conditions and similar.
- For interaction length scales for continuous-dispersed phase topology, use mean diameter. If you use a population balance model use the Sauter Mean Diameter.
- When running multiple flow regime topology, the best practice is to use “gradient corrected standard” as opposed to “standard” as method of flow regime weight function under the phase interaction. The weight functions are used to decide the fractions of the different regime contributions to linearized drag and heat transfer coefficients and the gradient based modification leads to a smoother field of blending weight function than the standard method.
- Even if the fraction of a specific phase is zero, it is often a good idea to specify that phase velocity the same as the velocity of the phase actually occupying the inlet. This is especially true when you set a minimum volume fraction specification. In cases where you do not allow for the zero-fraction of any phase anywhere. Setting a minimum volume fraction is also a strong suggestion.
- Using mixture turbulence wherever it is available is a recommendation (as opposed to phasic turbulence). Both for stability reasons and because you reduce the number of equations solved at any given time. How turbulence in multiphase cases works can be read about here [Turbulence for multiphase simulations in Simcenter STAR-CCM+ – VOLUPE Software]. And mixture turbulence works the same way as turbulence for MMP, with the mixture values for density, dynamic viscosity, velocity and turbulent viscosity.
- If you experience instability, start with 1st order on all schemes (this is not only relevant for multiphase simulations).
- If you run with LSI (Large Scale Interfaces, like a water surface) use Adaptive Interface Sharpening (ADIS) as the volume fraction convection option under the Eulerian Multiphase node in the model selection.
- Turn off secondary gradients to begin with.
- RUN SIMCENTER STAR-CCM+ IN DOUBLE PRECISION (r8)!
- If needed, set the convergence tolerance for the AMG-solver tighter, with a convergence tolerance of 1e-4. Consider also increasing the number of max cycles.
Under relaxation in EMP simulations
For Eulerian multiphase there exist both an Implicit and an Explicit under relaxation factor. The product of these two gives the overall (or global) under relaxation factor. The segregated EMP Flow solver and Volume fraction solver for multiphase both have the Implicit and the explicit under relaxations. The under relaxation factors are used to improve convergence for multiphase simulations. Both in terms of simulation speed and solver robustness. The Implicit under relaxation factor improves the stability and convergence of the linear system by using the relaxation factor to increase the diagonal dominance of the matrix. The matrix referred to is the matrix representing the coefficients of the linear systems solved by the AMG solver, using one of the available relaxation schemes, like Jacobi or Gauss-Seidel. The Explicit under relaxation factor specifies the multiplier that is applied to the provisional increment of the solution. The explicit is the one generally meant, when talking about under relaxation, i.e. how much of the new solution for the subsequent step to use.
There are some different recommendations for the under relaxation factor for the EMP solver, one is to keep the implicit one at 0.8 and reduce the Explicit one. Velocity and volume fraction has both the under relaxation factors, together with S-gamma if you are using that PBM and use the same for S-gamma as for volume fraction. A good starting point for under relaxation factor can be found here:
- Implicit URF should be as large as possible, no smaller than 0.5
- Global URF for velocity 0.4
- Global URF for turbulence 0.3
- Global URF for pressure and volume fraction 0.2
Note then, that turbulence and pressure only have an overall under relaxation factor, the Explicit needs to be set to give the correct value for the overall one.
You can also create a ramp of the under relaxation and decide how many iterations to use when linearly increasing the under relaxation factor to your decided value. One suggestion is to ramp over the 200 first iterations.
Monitoring and convergence
When it comes to convergence and monitoring your EMP simulation, you really need to make sure that in each timestep (if you are running a transient simulation) convergence has been reached. All solvers need to reach convergence before the next time step. If you have an interface, it is recommended to base your timestep on a value of CFL=0.5. This can be done by creating an iso-surface and monitor the CFL on it. Monitor the minimum and maximum value of velocity, pressure, and temperature to make sure your result is physical. Measure also the convergence of each phase by looking at, density x volume fraction x volume, hence keeping track of the total volume of each phase. And as usual, create several monitor points in areas of interest and track pressure and velocity on those. Also monitor mass imbalance for each phase.
Example of EMP simulation
Just to show the capability of the EMP solver I have performed a simulation. In general, the EMP methodology can do the same as any other of the Eulerian frameworks in Simcenter STAR-CCM+, meaning that when using MMP, VOF or DMP you should also be able in theory to reproduce the result using EMP. In this simulation example a 1 m long pipe with a diameter of 0.2 m is initially filled with air. At the inlet water is sent in with 1 m/s. The full simulation time is 0.8 s, and gravity is of course included. This is done using both EMP-LSI and VOF. The figure below shows a plot of the isosurface for water at volume fraction value 0.5 for both the EMP and the VOF simulation. The models give basically the same result, hence the difference in water level is small.
The videos below show the progression of water from the inlet and for 0.8 seconds. The upper video is for EMP and the bottom one is for VOF.
I hope this has been helpful to you as you tread all the steps in the swamp that is multiphase simulations in Simcenter STAR-CCM+. As usual, reach out to support@volupe.com if you have any questions.
Author
Robin Victor
+46731473121
support@volupe.com