# Incompressible Navier–Stokes solver with Phase Change Jump Condition

We wish to approximate numerically the incompressible, variable-density Navier–Stokes equations with phase change \displaystyle \partial_t\mathbf{u}+\nabla\cdot(\mathbf{u}\otimes\mathbf{u}) = \frac{1}{\rho}\left[-\nabla p + \nabla\cdot(2\mu\mathbf{D})\right] + \mathbf{a} \displaystyle \nabla\cdot\mathbf{u} = 0 with the deformation tensor \mathbf{D}=[\nabla\mathbf{u} + (\nabla\mathbf{u})^T]/2.

The scheme implemented here is close to that used in Gerris (Popinet, 2003, Popinet, 2009, Lagrée et al, 2011).

We will use the generic time loop, a CFL-limited timestep, the Bell-Collela-Glaz advection scheme and the implicit viscosity solver. If embedded boundaries are used, a different scheme is used for viscosity.

We extend this scheme by including the velocity jump due to the phase change: \displaystyle \left(\mathbf{u}_g - \mathbf{u}_l\right)\cdot\mathbf{n}_\Gamma = \dot{m}\left(\dfrac{1}{\rho_g} - \dfrac{1}{\rho_l}\right) which is introduced into the velocity field directly, according to the ghost velocity approach proposed by Nguyen et al. 2001, that was modified by Tanguy et al. 2007 for droplet evaporation problems, and by Tanguy et al. 2014 for boiling simulations.

The idea is to set the velocity jump in the “ghost regions” by exploiting the jump condition: \displaystyle \mathbf{u}^{ghost}_l = \mathbf{u}_g - \dot{m}\left(\dfrac{1}{\rho_g} - \dfrac{1}{\rho_l}\right)\mathbf{n}_\Gamma

\displaystyle \mathbf{u}^{ghost}_g = \mathbf{u}_l + \dot{m}\left(\dfrac{1}{\rho_g} - \dfrac{1}{\rho_l}\right)\mathbf{n}_\Gamma Two different momentum equations for the gas and liquid phase velocities are solved, but a single projection step is used to update the velocities at the new time step. Additional projection steps are used to obtain a divergence-free velocity for the advection of the volume fraction field.

This is a modified version of the method discussed by Long et al. 2024 for phase change using the EBIT approach, and implemented in basilisk by Tian Long. Unlike the previous version, this approach has mainly been tested on evaporation problems rather than on boiling simulations, and it was designed for VOF simulations.

The main advantage with respect to the navier-stokes/centered-evaporation.h approach is that we avoid the oscillations that arise due to the introduction of the localized expansion term as a volumetric source in the projection step.

#define VELOCITY_JUMP

#include "run.h"
#include "timestep.h"
#include "bcg.h"
#if EMBED
# include "viscosity-embed.h"
#else
# include "viscosity.h"
#endif
#include "aslam.h"

The primary variables are the centered pressure field p and the centered velocity field \mathbf{u}. The centered vector field \mathbf{g} will contain pressure gradients and acceleration terms.

We will also need an auxilliary face velocity field \mathbf{u}_f and the associated centered pressure field p_f.

scalar p[];
vector u[], g[];
scalar pf[];
face vector uf[];

Other variables specific to this algorithm.

vector u1[], u2[], uext[], u1g[], u2g[];
face vector uf1[], uf2[], ufext[], uf1g[], uf2g[];
scalar mEvapTot1[], mEvapTot2[];
scalar ls1[], ls2[];
scalar pg[];
vector n[];
scalar ps[];
face vector nf[];

extern scalar f;
extern scalar mEvapTot;
extern scalar rho1v, rho2v;

In the case of variable density, the user will need to define both the face and centered specific volume fields (\alpha and \alpha_c respectively) i.e. 1/\rho. If not specified by the user, these fields are set to one i.e. the density is unity.

Viscosity is set by defining the face dynamic viscosity \mu; default is zero.

The face field \mathbf{a} defines the acceleration term; default is zero.

The statistics for the (multigrid) solution of the pressure Poisson problems and implicit viscosity are stored in mgp, mgpf, mgu respectively.

If stokes is set to true, the velocity advection term \nabla\cdot(\mathbf{u}\otimes\mathbf{u}) is omitted. This is a reference to Stokes flows for which inertia is negligible compared to viscosity.

(const) face vector mu = zerof, a = zerof, alpha = unityf;
(const) scalar rho = unity;
mgstats mgp, mgpf, mgu;
bool stokes = false;

The volume expansion term is declared in evaporation.h.

extern scalar stefanflow;
scalar drhodt[], drhodtext[];

## Helper functions

We define the function that performs the projection step with the volume expansion term due to the phase change.

trace
mgstats project_sf_ghost (face vector uf, face vector ufg, scalar p,
(const) face vector alpha = unityf,
double dt = 1.,
int nrelax = 4)
{

We allocate a local scalar field and compute the divergence of \mathbf{u}_f. The divergence is scaled by dt so that the pressure has the correct dimension.

  scalar div[];
foreach() {
div[] = 0.;
foreach_dimension()
div[] += uf.x[1] - uf.x[];
div[] /= dt*Delta;
}

foreach()
div[] += drhodtext[]/dt;

We solve the Poisson problem. The tolerance (set with TOLERANCE) is the maximum relative change in volume of a cell (due to the divergence of the flow) during one timestep i.e. the non-dimensional quantity \displaystyle |\nabla\cdot\mathbf{u}_f|\Delta t Given the scaling of the divergence above, this gives

  mgstats mgp = poisson (p, div, alpha,
tolerance = TOLERANCE/sq(dt), nrelax = nrelax);

And compute \mathbf{u}_f^{n+1} using \mathbf{u}_f and p.

  foreach_face()
ufg.x[] = uf.x[] - dt*alpha.x[]*face_gradient_x (p, 0);

return mgp;
}

trace
mgstats project_extended (face vector uf, face vector ufs, scalar p,
(const) face vector alpha = unityf,
double dt = 1.,
int nrelax = 4)
{

We allocate a local scalar field and compute the divergence of \mathbf{u}_f. The divergence is scaled by dt so that the pressure has the correct dimension.

  scalar div[];
foreach() {
div[] = 0.;
foreach_dimension()
div[] += ufs.x[1] - ufs.x[];
div[] /= dt*Delta;
}

foreach()
div[] += drhodtext[]/dt;

We solve the Poisson problem. The tolerance (set with TOLERANCE) is the maximum relative change in volume of a cell (due to the divergence of the flow) during one timestep i.e. the non-dimensional quantity \displaystyle |\nabla\cdot\mathbf{u}_f|\Delta t Given the scaling of the divergence above, this gives

  mgstats mgp = poisson (p, div, alpha,
tolerance = TOLERANCE/sq(dt), nrelax = nrelax);

And compute \mathbf{u}_f^{n+1} using \mathbf{u}_f and p.

  foreach_face()
uf.x[] = ufs.x[] - dt*alpha.x[]*face_gradient_x (p, 0);

return mgp;
}

trace
mgstats project_sf_twofield (face vector uf1, face vector uf2, scalar p,
(const) face vector alpha = unityf,
double dt = 1.,
int nrelax = 4)
{

We allocate a local scalar field and compute the divergence of \mathbf{u}_f. The divergence is scaled by dt so that the pressure has the correct dimension.

  scalar div[];
foreach() {
div[] = 0.;
double div1 = 0., div2 = 0.;
foreach_dimension() {
div1 += uf1.x[1] - uf1.x[];
div2 += uf2.x[1] - uf2.x[];
}
div[] = (ls1[] < 0.) ? div1 : div2;
div[] /= dt*Delta;
}

We add the density lagrangian derivative.

  foreach()
div[] += drhodt[]/dt;

We solve the Poisson problem. The tolerance (set with TOLERANCE) is the maximum relative change in volume of a cell (due to the divergence of the flow) during one timestep i.e. the non-dimensional quantity \displaystyle |\nabla\cdot\mathbf{u}_f|\Delta t Given the scaling of the divergence above, this gives

  mgstats mgp = poisson (p, div, alpha,
tolerance = TOLERANCE/sq(dt), nrelax = nrelax);

And compute \mathbf{u}_f^{n+1} using \mathbf{u}_f and p.

  foreach_face() {
#ifndef DECOUPLED
#endif
}

return mgp;
}

## Boundary conditions

For the default symmetric boundary conditions, we need to ensure that the normal component of the velocity is zero after projection. This means that, at the boundary, the acceleration \mathbf{a} must be balanced by the pressure gradient. Taking care of boundary orientation and staggering of \mathbf{a}, this can be written

#if EMBED
# define neumann_pressure(i) (alpha.n[i] ? a.n[i]*fm.n[i]/alpha.n[i] :  \
a.n[i]*rho[]/(cm[] + SEPS))
#else
# define neumann_pressure(i) (a.n[i]*fm.n[i]/alpha.n[i])
#endif

p[right] = neumann (neumann_pressure(ghost));
p[left]  = neumann (- neumann_pressure(0));
ps[right] = neumann (neumann_pressure(ghost));
ps[left]  = neumann (- neumann_pressure(0));
pg[right] = neumann (neumann_pressure(ghost));
pg[left]  = neumann (- neumann_pressure(0));

#if AXI
uf.n[bottom] = 0.;
uf.t[bottom] = dirichlet(0); // since uf is multiplied by the metric which
// is zero on the axis of symmetry
uf1.n[bottom] = 0.;
uf1.t[bottom] = dirichlet(0); // since uf is multiplied by the metric which
// is zero on the axis of symmetry
uf2.n[bottom] = 0.;
uf2.t[bottom] = dirichlet(0); // since uf is multiplied by the metric which
// is zero on the axis of symmetry
p[top]    = neumann (neumann_pressure(ghost));
ps[top]    = neumann (neumann_pressure(ghost));
pg[top]    = neumann (neumann_pressure(ghost));
#else // !AXI
#  if dimension > 1
p[top]    = neumann (neumann_pressure(ghost));
p[bottom] = neumann (- neumann_pressure(0));
ps[top]    = neumann (neumann_pressure(ghost));
ps[bottom] = neumann (- neumann_pressure(0));
pg[top]    = neumann (neumann_pressure(ghost));
pg[bottom] = neumann (- neumann_pressure(0));
#  endif
#  if dimension > 2
p[front]  = neumann (neumann_pressure(ghost));
p[back]   = neumann (- neumann_pressure(0));
ps[front]  = neumann (neumann_pressure(ghost));
ps[back]   = neumann (- neumann_pressure(0));
pg[front]  = neumann (neumann_pressure(ghost));
pg[back]   = neumann (- neumann_pressure(0));
#  endif
#endif // !AXI

For embedded boundaries on trees, we need to define the pressure gradient for prolongation of pressure close to embedded boundaries.

#if TREE && EMBED
void pressure_embed_gradient (Point point, scalar p, coord * g)
{
foreach_dimension()
g->x = rho[]/(cm[] + SEPS)*(a.x[] + a.x[1])/2.;
}
#endif // TREE && EMBED

## Initial conditions

#define NOSHIFTING
#ifdef BOILING_SETUP
# define BYRHOGAS
# define CONSISTENTPHASE2
#endif

event defaults (i = 0)
{

CFL = 0.8;

The pressures are never dumped.

  p.nodump = pf.nodump = true;
ps.nodump = pg.nodump = true;

The default density field is set to unity (times the metric).

  if (alpha.x.i == unityf.x.i) {
alpha = fm;
rho = cm;
}
else if (!is_constant(alpha.x)) {
face vector alphav = alpha;
foreach_face()
alphav.x[] = fm.x[];
}

On trees, refinement of the face-centered velocity field needs to preserve the divergence-free condition.

#if TREE
uf.x.refine = refine_face_solenoidal;
uf1.x.refine = refine_face_solenoidal;
uf2.x.refine = refine_face_solenoidal;

When using embedded boundaries, the restriction and prolongation operators need to take the boundary into account.

#if EMBED
uf.x.refine = refine_face;
uf1.x.refine = refine_face;
foreach_dimension() {
uf.x.prolongation = refine_embed_face_x;
uf1.x.prolongation = refine_embed_face_x;
uf2.x.prolongation = refine_embed_face_x;
}
for (scalar s in {p, pf, u, g, u1, u2}) {
s.restriction = restriction_embed_linear;
s.refine = s.prolongation = refine_embed_linear;
}
for (scalar s in {p, pf, ps, pg})
#endif // EMBED
#endif // TREE
}

We had some objects to display by default.

event default_display (i = 0)
display ("squares (color = 'u.x', spread = -1);");

After user initialisation, we initialise the face velocity and fluid properties.

double dtmax;

event init (i = 0)
{
trash ({uf1, uf2, uf});
foreach_face() {
uf.x[] = fm.x[]*face_value (u.x, 0);
uf1.x[] = fm.x[]*face_value (u1.x, 0);
uf2.x[] = fm.x[]*face_value (u2.x, 0);
}

We update fluid properties.

  event ("properties");

We set the initial timestep (this is useful only when restoring from a previous run).

  dtmax = DT;
event ("stability");

We set the default divergence source term to zero (for the liquid phase)

  foreach() {
drhodt[] = 0.;
drhodtext[] = 0.;
}
}

## Time integration

The timestep for this iteration is controlled by the CFL condition, applied to the face centered velocity field \mathbf{u}_f; and the timing of upcoming events.

event set_dtmax (i++,last) dtmax = DT;

event stability (i++,last) {
dt = dtnext (stokes ? dtmax : min (timestep (uf1, dtmax), timestep
(uf2, dtmax)));
}

## Extrapolations

We use PDE-based Aslam’s extrapolations, to extrapolate the vaporization rate \dot{m}, from the interface to the liquid and gas phases.

void extrapolations (void)
{

First, we store the liquid and gas phase volume fractions.

  scalar faslam1[], faslam2[];
foreach() {
faslam1[] = f[];
faslam2[] = 1. - f[];
}

We convert the volume fraction in level set. This step can be expensive, and it should be skipped if the CLSVOF method is used.

#ifdef CLSVOF
extern scalar d;
foreach() {
ls1[] = d[];
ls2[] = -d[];
}
#else
vof_to_ls (f, ls1, imax = 5);
foreach()
ls2[] = -ls1[];
#endif

The interface normals are computed using the level set. By doing so the normals are naturally defined over the whole domain.

  gradients ({ls1}, {n});
foreach() {
double maggf = 0.;
foreach_dimension()
maggf += sq (n.x[]);
maggf = sqrt (maggf);
foreach_dimension()
n.x[] /= (maggf + 1.e-10);
}

Update the interface normal vectors on the faces.

  foreach_face()
nf.x[] = 0.5*(n.x[] + n.x[-1]);

We store the extrapolated vaporization rate \hat{m} on the fields mEvapTot1 and mEvapTot2. Using constant_extrapolations the liquid and gas phase cells are populated with the vaporization rate without changing its values.

#ifndef DIFFUSIVE
foreach() {
double rhojump = (rho1v[] > 0. && rho2v[] > 0.) ?
(1./rho2v[] - 1./rho1v[]) : 0.;

mEvapTot1[] = mEvapTot[]*rhojump;
mEvapTot2[] = mEvapTot[]*rhojump;
}

constant_extrapolation (mEvapTot1, ls1, 0.5, 20, c=faslam1, nl=0,
nointerface=true);
constant_extrapolation (mEvapTot1, ls2, 0.5, 20, c=faslam2, nl=0,
nointerface=true);

foreach()
mEvapTot2[] = mEvapTot1[];
#endif
}

We perform the extrapolations after the phasechange event in evaporation.h.

event phasechange (i++,last) {
extrapolations();
}

If we are using VOF or diffuse tracers, we need to advance them (to time t+\Delta t/2) here. Note that this assumes that tracer fields are defined at time t-\Delta t/2 i.e. are lagging the velocity/pressure fields by half a timestep.

event vof (i++,last);
event tracer_diffusion (i++,last);

The fluid properties such as specific volume (fields \alpha and \alpha_c) or dynamic viscosity (face field \mu_f) – at time t+\Delta t/2 – can be defined by overloading this event.

event properties (i++,last);

## Initialize Velocities

We set the initial ghost velocities for the first iteration. For droplet evaporation problems we use the jump condition to update the gas phase ghost velocity:

\displaystyle \mathbf{u}^{ghost}_g = \mathbf{u}_l - \dot{m}\left(\dfrac{1}{\rho_g} - \dfrac{1}{\rho_l}\right)\mathbf{n}_\Gamma

while the initial liquid ghost velocity is set to zero. For boiling problems we set to zero the initial gas ghost velocity, while we use the jump condition to set the value of the liquid phase ghost velocity:

\displaystyle \mathbf{u}^{ghost}_l = \mathbf{u}_g + \dot{m}\left(\dfrac{1}{\rho_g} - \dfrac{1}{\rho_l}\right)\mathbf{n}_\Gamma

void update_ghost_velocities (void) {
foreach() {
foreach_dimension() {
#ifdef BOILING_SETUP
u2g.x[] = u2g.x[];
u1g.x[] = u2.x[] + mEvapTot1[]*n.x[];
#else
u1g.x[] = u1g.x[];
u2g.x[] = u1.x[] - mEvapTot2[]*n.x[];
#endif
u1.x[] = (ls1[] < 0.) ? u1.x[] : u1g.x[];
u2.x[] = (ls1[] > 0.) ? u2.x[] : u2g.x[];
}
}

foreach_face() {
#ifdef BOILING_SETUP
double mEvapTot1f = 0.5*(mEvapTot1[] + mEvapTot1[-1]);
uf2g.x[] = uf2g.x[];
uf1g.x[] = uf2.x[] + mEvapTot1f*nf.x[]*fm.x[];
#else
double mEvapTot2f = 0.5*(mEvapTot2[] + mEvapTot2[-1]);
uf1g.x[] = uf1g.x[];
uf2g.x[] = uf1.x[] - mEvapTot2f*nf.x[]*fm.x[];
#endif
double lsf = 0.5*(ls1[] + ls1[-1]);
uf1.x[] = (lsf < 0.) ? uf1.x[] : uf1g.x[];
uf2.x[] = (lsf > 0.) ? uf2.x[] : uf2g.x[];
}
}

event init_ghost (i = 0, last)
{

We compute the value of the centered ghost velocities.

  foreach() {
foreach_dimension() {
#ifdef BOILING_SETUP
u2g.x[] = 0.;
u1g.x[] = u2.x[] + mEvapTot1[]*n.x[];
#else
u1g.x[] = 0.;
u2g.x[] = u1.x[] - mEvapTot2[]*n.x[];
#endif
}
}

We compute the value of the face ghost velocities. The interface normal on the face is computed using the level set.

  foreach_face() {
#ifdef BOILING_SETUP
double mEvapTot1f = 0.5*(mEvapTot1[] + mEvapTot1[-1]);
uf2g.x[] = 0.;
uf1g.x[] = uf2.x[] + mEvapTot1f*nf.x[]*fm.x[];
#else
double mEvapTot2f = 0.5*(mEvapTot2[] + mEvapTot2[-1]);
uf1g.x[] = 0.;
uf2g.x[] = uf1.x[] - mEvapTot2f*nf.x[]*fm.x[];
#endif
}
}

At the beginning of every iteration we initialize the liquid and gas phase velocities using the ghost values:

\displaystyle \mathbf{u}_l = \begin{cases} \mathbf{u}_l & \text{if } \phi < 0 \\ \mathbf{u}_l^{ghost} & \text{if } \phi > 0 \end{cases}

\displaystyle \mathbf{u}_g = \begin{cases} \mathbf{u}_g & \text{if } \phi > 0 \\ \mathbf{u}_g^{ghost} & \text{if } \phi < 0 \end{cases}

Where the level set \phi is negative in the liquid phase and positive in the gas phase.

event init_velocities (i++, last)
{
foreach() {
foreach_dimension() {
u1.x[] = (ls1[] < 0.) ? u1.x[] : u1g.x[];
u2.x[] = (ls1[] > 0.) ? u2.x[] : u2g.x[];
}
}

foreach_face() {
double lsf = 0.5*(ls1[] + ls1[-1]);
uf1.x[] = (lsf < 0.) ? uf1.x[] : uf1g.x[];
uf2.x[] = (lsf > 0.) ? uf2.x[] : uf2g.x[];
}
}

### Predicted face velocity field

For second-order in time integration of the velocity advection term \nabla\cdot(\mathbf{u}\otimes\mathbf{u}), we need to define the face velocity field \mathbf{u}_f at time t+\Delta t/2. We use a version of the Bell-Collela-Glaz advection scheme and the pressure gradient and acceleration terms at time t (stored in vector \mathbf{g}).

void prediction(vector u, face vector uf)
{
vector du;
foreach_dimension() {
scalar s = new scalar;
du.x = s;
}

foreach()
foreach_dimension() {
#if EMBED
if (!fs.x[] || !fs.x[1])
du.x[] = 0.;
else
#endif
du.x[] = u.x.gradient (u.x[-1], u.x[], u.x[1])/Delta;
}
else
foreach()
foreach_dimension() {
#if EMBED
if (!fs.x[] || !fs.x[1])
du.x[] = 0.;
else
#endif
du.x[] = (u.x[1] - u.x[-1])/(2.*Delta);
}

trash ({uf});
foreach_face() {
double un = dt*(u.x[] + u.x[-1])/(2.*Delta), s = sign(un);
int i = -(s + 1.)/2.;
uf.x[] = u.x[i] + (g.x[] + g.x[-1])*dt/4. + s*(1. - s*un)*du.x[i]*Delta/2.;
#if dimension > 1
if (fm.y[i,0] && fm.y[i,1]) {
double fyy = u.y[i] < 0. ? u.x[i,1] - u.x[i] : u.x[i] - u.x[i,-1];
uf.x[] -= dt*u.y[i]*fyy/(2.*Delta);
}
#endif
#if dimension > 2
if (fm.z[i,0,0] && fm.z[i,0,1]) {
double fzz = u.z[i] < 0. ? u.x[i,0,1] - u.x[i] : u.x[i] - u.x[i,0,-1];
uf.x[] -= dt*u.z[i]*fzz/(2.*Delta);
}
#endif
uf.x[] *= fm.x[];
}

delete ((scalar *){du});
}

We solve the advection equations for \mathbf{u}_l and \mathbf{u}_g.

void advection_div (scalar * tracers, face vector u, double dt,
scalar * src = NULL)
{

If src is not provided we set all the source terms to zero.

  scalar * psrc = src;
if (!src)
for (scalar s in tracers) {
const scalar zero[] = 0.;
src = list_append (src, zero);
}
assert (list_len (tracers) == list_len (src));

scalar f, source;
for (f,source in tracers,src) {
face vector flux[];
tracer_fluxes (f, u, flux, dt, source);
#if !EMBED
foreach() {
double fold = f[];
#endif
foreach_dimension()
f[] += dt*(flux.x[] - flux.x[1] + fold*(u.x[1] - u.x[]))/(Delta*cm[]);
#else
f[] += dt*(flux.x[] - flux.x[1])/(Delta*cm[]);
#endif
}
#else // EMBED
update_tracer (f, u, flux, dt);
#endif // EMBED
}

if (!psrc)
free (src);
}

{
if (!stokes) {
prediction (u1, uf1);
prediction (u2, uf2);
mgpf = project_sf_twofield (uf1, uf2, pf, alpha, dt/2., mgpf.nrelax);
advection_div ((scalar *){u1}, uf1, dt, (scalar *){g});
advection_div ((scalar *){u2}, uf2, dt, (scalar *){g});
}
}

### Viscous term

We first define a function which adds the pressure gradient and acceleration terms.

static void correction (vector u, double dt)
{
foreach()
foreach_dimension()
u.x[] += dt*g.x[];
}

Solving the viscous term we obtain the temporary velocities \mathbf{u}_l^* and \mathbf{u}_g^*.

event viscous_term (i++, last)
{
if (constant(mu.x) != 0.) {
correction (u1, dt);
correction (u2, dt);
mgu = viscosity (u1, mu, rho, dt, mgu.nrelax);
mgu = viscosity (u2, mu, rho, dt, mgu.nrelax);
correction (u1, -dt);
correction (u2, -dt);
}

We reset the acceleration field (if it is not a constant).

  if (!is_constant(a.x)) {
face vector af = a;
trash ({af});
foreach_face()
af.x[] = 0.;
}
}

### Acceleration term

The acceleration term \mathbf{a} needs careful treatment as many equilibrium solutions depend on exact balance between the acceleration term and the pressure gradient: for example Laplace’s balance for surface tension or hydrostatic pressure in the presence of gravity.

To ensure a consistent discretisation, the acceleration term is defined on faces as are pressure gradients and the centered combined acceleration and pressure gradient term \mathbf{g} is obtained by averaging.

The (provisionary) face velocity field at time t+\Delta t is obtained by interpolation from the centered velocity field. The acceleration term is added.

event acceleration (i++,last)
{
trash ({uf1,uf2});
foreach_face() {
uf1.x[] = fm.x[]*(face_value (u1.x, 0) + dt*a.x[]);
uf2.x[] = fm.x[]*(face_value (u2.x, 0) + dt*a.x[]);
}
}

## Approximate projection

This function constructs the centered pressure gradient and acceleration field g using the face-centered acceleration field a and the cell-centered pressure field p.

void centered_gradient (scalar p, vector g)
{

We first compute a face field \mathbf{g}_f combining both acceleration and pressure gradient.

  face vector gf[];
foreach_face()
gf.x[] = fm.x[]*a.x[] - alpha.x[]*(p[] - p[-1])/Delta;

We average these face values to obtain the centered, combined acceleration and pressure gradient field.

  trash ({g});
foreach()
foreach_dimension()
g.x[] = (gf.x[] + gf.x[1])/(fm.x[] + fm.x[1] + SEPS);
}

## Projection

To get the pressure field at time t + \Delta t we project the face velocity field (which will also be used for tracer advection at the next timestep). Then compute the centered gradient field g.

event projection (i++,last)
{

For boiling problems, we obtain a ghost pressure p^{ghost} using the following projection step: \displaystyle \nabla\cdot\left(\dfrac{1}{\rho}\nabla p^{ghost}\right) = \dfrac{\nabla\cdot\mathbf{u}_g^*}{\Delta t} from which we obtain the updated gas ghost velocity: \displaystyle \mathbf{u}_g^{ghost} = \mathbf{u}_g^* - \dfrac{\Delta t}{\rho}\nabla p^{ghost}

For evaporation problems, we solve the ghost pressure using the divergence of the liquid velocity: \displaystyle \nabla\cdot\left(\dfrac{1}{\rho}\nabla p^{ghost}\right) = \dfrac{\nabla\cdot\mathbf{u}_l^*}{\Delta t} and we use this pressure to update the liquid ghost velocity: \displaystyle \mathbf{u}_l^{ghost} = \mathbf{u}_l^* - \dfrac{\Delta t}{\rho}\nabla p^{ghost}

#ifdef BOILING_SETUP
project_sf_ghost (uf2, uf2g, pg, alpha, dt, mgpf.nrelax);

vector gpg[];
foreach()
foreach_dimension()
u2g.x[] = u2.x[] + dt*gpg.x[];
#else
project_sf_ghost (uf1, uf1g, pg, alpha, dt, mgpf.nrelax);

vector gpg[];
foreach()
foreach_dimension()
u1g.x[] = u1.x[] + dt*gpg.x[];
#endif

The one-field pressure of the system is obtained from the following projection step: \displaystyle \nabla\cdot\left(\dfrac{1}{\rho}\nabla p^{ghost}\right) = \dfrac{\nabla\cdot\mathbf{u}^*}{\Delta t}

where the divergence is computed based on the level set field: \displaystyle \nabla\cdot\mathbf{u}^* = \begin{cases} \nabla\cdot\mathbf{u}_l^* & \text{if } \phi < 0 \\ \nabla\cdot\mathbf{u}_g^* & \text{if } \phi > 0 \end{cases}

and the two velocities are computed from the one-field pressure and update at the new time step as:

\displaystyle \mathbf{u}_l^{n+1} = \mathbf{u}_l^* - \dfrac{\Delta t}{\rho} \nabla p \displaystyle \mathbf{u}_g^{n+1} = \mathbf{u}_g^* - \dfrac{\Delta t}{\rho} \nabla p

  mgp = project_sf_twofield (uf1, uf2, p, alpha, dt, mgp.nrelax);

correction (u1, dt);
correction (u2, dt);
}

We update the centered and face velocity values.

event update_ghost (i++, last) {
foreach() {
foreach_dimension() {
#ifdef BOILING_SETUP
u2g.x[] = u2g.x[];
u1g.x[] = u2.x[] + mEvapTot1[]*n.x[];
#else
u1g.x[] = u1g.x[];
u2g.x[] = u1.x[] - mEvapTot2[]*n.x[];
#endif
}
}

foreach_face() {
#ifdef BOILING_SETUP
double mEvapTot1f = 0.5*(mEvapTot1[] + mEvapTot1[-1]);
uf2g.x[] = uf2g.x[];
uf1g.x[] = uf2.x[] + mEvapTot1f*nf.x[]*fm.x[];
#else
double mEvapTot2f = 0.5*(mEvapTot2[] + mEvapTot2[-1]);
uf1g.x[] = uf1g.x[];
uf2g.x[] = uf1.x[] - mEvapTot2f*nf.x[]*fm.x[];
#endif
}
}

## Extended Velocity

According to Tanguy et al. 2007, an additional projection step is required in evaporation problems to ensure that the liquid velocity is conservative. This step could be skipped for boiling problems. We define a velocity \mathbf{u}^S as: \displaystyle \mathbf{u}^S = \begin{cases} \mathbf{u}_l^{n+1} & \text{if } \phi < 0 \\ \mathbf{u}_l^{ghost} & \text{if } \phi > 0 \end{cases}

And we solve an additional Poisson equation: \displaystyle \nabla\cdot\left(\dfrac{1}{\rho}\nabla\psi\right) = \dfrac{\nabla\cdot\mathbf{u}^S}{\Delta t} from which we correct the liquid velocity ensuring that it respects the divergence-free constraint: \displaystyle \mathbf{u}_l^{n+1} = \mathbf{u}^S - \dfrac{\Delta t}{\rho}\nabla \psi

If we perform this step also for boiling problems we need to do the same operation replacing \mathbf{u}_l with \mathbf{u}_g, assuming that the VOF field is advected using the gas phase velocity.

event extended_velocity (i++, last) {
#ifdef BOILING_SETUP
face vector ufs[];
foreach_face() {
double lsf = 0.5*(ls1[] + ls1[-1]);
ufs.x[] = (lsf > 0.) ? uf2.x[] : uf2g.x[];
}
project_extended (uf2, ufs, ps, alpha, dt, mgp.nrelax);

foreach_face()
uf2g.x[] = uf2.x[];
#else
face vector ufs[];
foreach_face() {
double lsf = 0.5*(ls1[] + ls1[-1]);
ufs.x[] = (lsf < 0.) ? uf1.x[] : uf1g.x[];
}
project_extended (uf1, ufs, ps, alpha, dt, mgp.nrelax);

foreach_face()
uf1g.x[] = uf1.x[];
#endif
}

## Reconstructions

We reconstruct \mathbf{u}_l^{n+1} and \mathbf{u}_g^{n+1} using the ghost liquid and gas phase velocities, for the next time step. The one-field velocity \mathbf{u} is simply reconstructed from a volume average, just for visualization purposes.

We also set the value of the extended velocity \mathbf{u}^E, used for the VOF advection equation.

event reconstructions (i++, last) {
foreach() {
foreach_dimension() {
u1.x[] = (ls1[] < 0.) ? u1.x[] : u1g.x[];
u2.x[] = (ls1[] > 0.) ? u2.x[] : u2g.x[];
}
}

foreach_face() {
double lsf = 0.5*(ls1[] + ls1[-1]);
uf1.x[] = (lsf < 0.) ? uf1.x[] : uf1g.x[];
uf2.x[] = (lsf > 0.) ? uf2.x[] : uf2g.x[];
#ifdef BOILING_SETUP
ufext.x[] = uf2.x[];
#else
ufext.x[] = uf1.x[];
#endif
}

foreach()
foreach_dimension()
u.x[] = u1.x[]*f[] + u2.x[]*(1. - f[]);

foreach_face() {
double ff = 0.5*(f[] + f[-1]);
uf.x[] = uf1.x[]*ff + uf2.x[]*(1. - ff);
}
}

Some derived solvers need to hook themselves at the end of the timestep.

event end_timestep (i++, last);

After mesh adaptation fluid properties need to be updated. When using embedded boundaries the fluid fractions and face fluxes need to be checked for inconsistencies.

#if TREE
#endif