One or more Computation Directions to apply the boundary conditions may be selected.

Select the directions where flow should be simulated. To obtain the flow results for all three directions in the result file, it is necessary to choose all three directions. To some extent, checking all directions for the run of the solver prolongs computational time.

Solving linear flow with Stokes(-Brinkman) results in a 3x3 permeability matrix, which is only filled completely, if all computation directions are selected.

The Domain Boundary Conditions in Longitudinal Direction can be checked to be Periodic, Symmetric (Dirichlet), or can follow the Velocity inlet, Pressure outlet condition.

Periodic boundary conditions are recommended for periodically generated structure models and for non-periodic structures with high porosity.

Use Symmetric boundary conditions for non-periodic structures if the percentage of solid voxels is high at the inlet.  

Note, that selecting Velocity Inlet, Pressure outlet for Stokes(-Brinkman) automatically selects the SimpleFFT solver in the Solver tab. The other two solvers cannot solve the Stokes(-Brinkman) equation with velocity inlet and pressure outlet, and thus, are grayed out. The options in the Solver tab are described here.

After checking Periodic or Velocity inlet, Pressure outlet an inflow region (also called inlet) and outflow region (also called outlet) can be automatically added by checking Add implicit region and entering its size in voxels. The default added implicit inflow and outflow are 10 voxels, respectively. The inlet and outlet are essential to avoid the possibility of closing the flow channels when the structure is periodically repeated. For example, for the following structure choosing periodic boundary conditions in the direction of the flow without adding an implicit region results in the flow channels being artificially closed.

A warning appears when trying to run flow computations without adding an inflow region.

To open the channels and make the flow possible, the user should add an inlet

or choose symmetric boundary conditions.

Even so, when possible, we suggest using a periodic boundary condition, as the computational memory requirements are fairly low and therefore, the computational time is shorter.

The Velocity inlet, Pressure outlet (VinPout) boundary conditions apply a constant flow velocity in the inlet and a constant pressure drop in the outlet. The final result is influenced by the size of the inlet and outlet. Both are set with the value entered in Add implicit inflow region.

In fluid dynamics, three experiments are typical:

• Measure the mean velocity for the applied pressure drop,
• Measure the pressure drop for a given mean velocity,
• Measure the pressure drop for a given mass flow rate.

The flow properties pressure drop, or mean velocity can be entered in the Experiment Input / Output panel. Input a prescribed Pressure Drop value and obtain the calculated Mean Velocity in the result file as output. Alternatively, the input of the mean velocity results in the output of pressure drop.

The Pressure Drop is the difference between the inflow and outflow pressures, and the Mean Velocity is the average speed of the flow in the positive Z-direction. The default values are set at 0.0002 mbar, or 0.02 Pascal (1 Pa = 0.01 mbar = 10-5 bar) for pressure drop and 0.1 m/s for mean velocity.

In homogenization experiments, it is usual to input the pressure drop whereas for filtration experiments, it is the flow mean velocity, derived from the mass flow rate (g/cm3).

The Flow Rate on Flow Area in l/min per cm2 (default) or in other units, can be used to obtain the pressure drop at a given mean velocity. The volumetric flow rate per flow area is the volume of fluid which passes per unit time through a given area.

For each property, the desired unit can be selected from the pull-down menu.

It is possible to use the Mean Velocity or the Flow Rate as input because the Stokes(-Brinkman) equation is linear. Thus, the solver can prescribe a pressure drop () and compute a mean velocity (). This mean velocity is not the desired mean velocity () entered in the Experiment Input / Output panel. Therefore, the velocity and pressure field are rescaled by . Then, the pressure drop () is calculated by

For example, if the desired velocity is twice the mean velocity used by the solver, the computed pressure drop is doubled to obtain the pressure drop corresponding to the desired mean velocity.

The Domain Boundary Conditions in Transverse Directions can be checked to be Periodic, Symmetric, No-Slip, or Expert.

With the default Periodic selected, the process of periodic continuation is internally done during the run of the solver, repeatedly adding the volume structure in the directions transverse to the flow direction. Choosing the appropriate boundary condition depends on the structure’s design.

For example, imagine a structure with a cross-section as shown in (a).

• If the expected pattern of the geometry is repeated in both transverse directions (b), the flow is computed with periodic boundary conditions.
• If instead the geometry has mirror symmetry (c), symmetric boundary conditions are taken.
• If the structure is encased in a closed wall (d), the no-slip boundary conditions are used in transverse directions.

The boundary conditions in the two directions transverse to the flow can also be set to be different by checking Expert boundary conditions. For example, when the fluid is chosen to flow in the Z-direction, the boundary conditions could be chosen to be No-slip in X-direction and Symmetric in the Y-direction.

When No-Slip is used, the solver internally adds a one-voxel layer in the required direction and solves with periodic boundary conditions. That effectively is equivalent to solve the structure with casing in two ends in the direction of interest. So, the size of computation in this direction becomes n+1.

The Slip Length allows to include sliding effects in the flow simulation. Sometimes the permeability of gases can be somewhat different from the permeability of liquids in the same media. One difference is attributable to "slippage" of gas at the interface with the solid when the gas mean free path is comparable to the pore size.

The default setting No-Slip corresponds to a flow velocity of zero along the structure.

Two settings are available for the No-Slip boundary condition. Use Second Order No-Slip is activated by default. This sets the tangential velocity to zero at the center of the voxel surfaces and uses a second order approximation of the velocity field. The first order setting, which is used when the box is left unchecked uses a linear approximation (Harlow-Welch, 1965).

Use Sharp Corner can be used for digital rocks where permeability is usually overestimated or cases where voxels represent exact geometry. Activating it sets the tangential velocity to zero at the voxel corners. When the box is unchecked the default Round Corner is applied, which should be used for structures with round obstacles like fibers or grains.

Slip with a non-zero Slip Length simulates the sliding of the fluid along the solid, increasing the fluid mean flux and thus, the permeability of the structure. This option might be used when it is realistic for a given physical material. Currently, the same slip length value must be set for all materials in the structure.

In earlier releases, this feature worked correctly for axis aligned walls only, but since GeoDict 2020 the expression of the slip velocity, which assumes the slip velocity proportional to the shear stress at the surface, is reformulated for different velocity components when the angle of fiber surface is known, and reimplemented in the flow solver. Thus, direct simulation of the slip flow is possible.

Here, is the fluid flow velocity as it was introduced in Darcy's law and the Stokes equation, is the normal direction to the solid surface, is the fiber surface, is the Slip Length and is any tangential direction with . For the same pressure drop, the computed velocities for slip boundary conditions are higher than for no-slip boundary conditions. Conversely, for a given velocity or equivalently, a given mass flux, the pressure drop is lower when computed with slip boundary conditions.

For a straight channel structure, the two slip flow equations above become:

In this following example figure, the gray solid serves as a wall for a straight channel. To obtain the flow velocity along the solid () a coordinate system is defined by the solid orientation.

For a Slip Length of zero (), the graph that describes the flow velocity in dependence of the distance to the solid surface, would start at the surface of the solid. However, for a positive Slip Length () it is shifted into the solid by . Thus, the flow velocity is defined.