Boundary Conditions

Initial Condition

Analysis > Boundary Conditions > Initial Condition

Initial condition is used to define and create the fluid (liquid and gas) regions inside the container. This is useful when the CAD or FE model does not have a separate body for the fluids. The fluid option will be displayed based on single-phase (one fluid) and multiphase (two fluids) options in the Solution panel.

The fluids can be generated using By plane, By % of "Fluid1" in total volume, or By "Fluid1" volume in liters.

Body Force

Analysis > Boundary Conditions > Body Force

This option is used to define body force for a simulation. For Global Acceleration, the vector and magnitude must be specified. By default, the magnitude is 9.81 m/s². It can be specified in the desired direction using a vector.

Figure 2. Global acceleration definition

For the Time Dependent body force with different acceleration terms, a time versus acceleration table must be established. This table can be defined within the Create Table window or imported from an external source in the form of a predefined *.txt file.

Figure 3. Definition of Time Dependent body force with different acceleration terms

Domain

Analysis > Boundary Conditions > Domain

This tool is used to define the domain and global parameters of the nanoFluidX case. For a typical drivetrain simulation, if the simulation is of a closed geometry (a gearbox) nanoFluidX will automatically calculate the domain dimensions, so it does not need to be specified.

For other cases, especially those with open boundaries, the domain size and/or reference values should be specified.

Define Domain Manually: If the simulation has an open boundary, or if there are periodic boundary conditions associated with the domain, it is necessary to manually prescribe the size of the domain (bounding box). In this case the padding around the particles should be set to 3*dx.
Boundary Conditions: These domain parameters are used to define the boundary conditions at minimum and maximum boundary. Boundary options supported are Periodic and Simple Outlet (default).
Other options: A free text box where additional parameters can be specified.

Motion

Analysis > Boundary Conditions > Motion

Wall boundary particles can be moved during a simulation with a prescribed motion. The principal concept is to define a motion for a specific phase/body and apply this motion within a given time frame.

Motion types that can be specified in tank sloshing simulations are Translational, Rotational, Passive Rigid Body and Oscillatory motion.

Define motion in SimLab: Oscillatory motion is defined as translational oscillation motion based on cosine function and initial body position.; Passive rigid body motion defines a 6-DOF rigid body freely interacting with the fluid. Constraints, forces, and damping are available for each translation and rotation component.; Like phases, different motions are defined consecutively. It is possible to combine motion types to realize more complex motions.
Note: Only certain combinations of motions are supported.
For the most complex motions a custom motion can be defined. This allows import of a time history file from the multibody dynamics solver to define any kind of arbitrary motion.; MotionSolve and Inspire Motion export this file natively. Other solvers may be able to produce the file required.

Inlet

Analysis ribbon > Boundary Conditions > Inlet

An Inlet region is an (fluid) inlet without back flow. Inlet regions can be defined anywhere inside the domain using rectangular, circular, or custom shapes. The only limitation to the inlet regions is that they must be planar, even in the custom shape or arbitrary orientation scenario.

Figure 4. Circular and Circular Arbor inlet region definitions. (left) front view, flowing into page, (right) side view, flowing from left to right. Spawn particles (brown), particles affected by the extension (magenta), free particles (cyan). Continuous lines show extension borders.

Inlet regions consist of two parts:

Stencil spawn surface
Extension (optional)

Inlet Stencil

Inlet stencil is created for the inlet region which behaves as a source of particles and will be exported as a .txt file for the inlet region containing the x-, y-, and z- coordinates of the particles which are to be inserted into the domain.

The spacing of the stencil must match the dx value used for the rest of the simulation.

Important: When the stencil is generated, it will be placed in a model named InletRegionsProbes.gda. The stencils must remain in the model. Otherwise, they will not be exported correctly. This model is always exported to the .cfg, regardless of whether it is displayed during export.

Check the stencil against the wall particles to ensure there are no overlaps or penetrations. The figure below shows an example of a misaligned stencil and conduit.

As the fluid particles leave the extension, the distance between fluid-fluid particles and fluid-wall particles are not similar. This results in a pressure rise on the side where fluid particles are closer to the wall. Depending on the severity of the misalignment, this may result in undesired secondary flows.

Inlet Extension

The extension imposes the inlet velocity and ensures the distance between different spawn layers remaining at dx. As a result, extension is an important component of the Inlet region.

The extension covers up to half dx, further in each direction than the definitions given in the *.cfg to ensure all spawned Inlet region particles are covered. The fluid particles within the extension have the same velocity as the inlet region. It is important that the spawn area is not disturbed by other fluid particles. The extension only applies to the fluid phase specified for that specific inlet region.

While possible, disabling the extension is generally not recommended unless it is guaranteed that the spawn area will remain undisturbed during the active interval of the Inlet region. Moving Inlet regions always requires an extension to function properly.

Care must be taken to ensure that any change in profile or shape of the conduit downstream of the Inlet region does not conflict with the extension. If there is a conflict, the extension will push the particles through the conduit wall. It is not guaranteed that the particles will be out of the wall at the end of the extension.

Define Inlet in SimLab

In SimLab, inlet region can be created inside the domain by using combination of inlet shapes and inlet types. After the inlet name is defined, from the material selection menu, users can define which fluid phase is going to be used for the inlet. Inlet shape can be rectangular, circular or custom. For Inlet Type, Constant or Time dependent inflow can be defined based on Velocity, Mass or Volume flow.

Name: Inlet region name.
Material: Specifies the phase of the fluid spawned by the inlet region.
Inlet Shape: Specifies the shape of the inlet region.
Inlet Type: Specifies the type of the inlet region. Inflow can be defined via Velocity, Mass or Volume flow and can be constant and time dependent.
Start Time/ End Time: Specifies the start and finish times which define the window where the Inlet region is active.
Ramp up Time/ Ramp down Time: This parameter specifies a time window for the acceleration and deceleration of the fluid. At the start time, the flow will ramp up from zero to the specified value over this time. If ramp down is specified, the velocity will ramp back down to zero prior to the end time. This minimizes pressure fluctuations and instabilities caused by instantaneous changes in velocity.
Prefilled: To be activated if fluid particles coinciding with stencil positions are present when inlet region becomes active.
Moving body motion to follow: If active, user has to select moving body that would be followed by inlet region.
Other Options: A free text box where additional parameters can be specified.

Inlet Temperature Treatment

After having the Heat Transfer Coefficient (HTC) calculations available in nanoFluidX, it becomes necessary to apply simple temperature boundary conditions to inlet regions. Inlet fluid temperatures may be specified for each inlet region via the other options text box in the Inlet Regions dialog menu, without the need to define a separate fluid phase. Specified temperature will stay constant within the inlet region and inlet extensions.

Note:

The temperature value remains constant throughout the simulation and does not offer any ramp or time-series input. When discharging fluids of different temperatures into a bulk, please choose a suitable initial bulk temperature to avoid extreme differences in temperature.
Constant temperature is enforced within the extensions if the extension is active. This means that if inletregion_extpre and/or inletregion_extpst are set to true, the temperature control within the extension is maintained before and/or after the inlet region’s active particle spawn interval.

Outlet

Analysis ribbon > Boundary Conditions > Outlet

Outlet regions use a combination of removal and extension regions to allow particles of any phase to be removed from anywhere within the computational domain. Every particle that enters an outlet region will be removed from the simulation permanently.

Currently there are 3 shapes available:

Spherical
Cylindrical
Cuboidal

Cylindrical and cuboidal outlet regions can optionally have an extension region, like inlet region extensions, which can define either velocity or acceleration within its volume.

An extension is an extended region in the opposite direction of the outlet region's normal where a constant particle velocity or acceleration in the normal direction is enforced. When used without extensions, outlet regions act as pseudo zero pressure and zero stress boundaries with no back flow. Although it must be noted that since the particles are missing neighbors (incomplete support), these conditions are not strictly met, hence pseudo.

When used with an extension and provided that the extension is well populated, the behavior depends on the type of extension.

Spherical outlet region cannot have an extension and acts as a simple particle sink.

Define Outlet in SimLab

In SimLab, outlet region can be created inside the domain by using combination of outlet shapes and extension types.

Name: Outlet region name.
Outlet Shape: Specifies the shape of the outlet region.
Extension Type: Specifies the type of the outlet extension type:
- Velocity - When using the velocity extension type, the extension sets the normal component of particle velocity to the specified value. The particle velocity is free to evolve in directions perpendicular to the Outlet regions normal directions. The particles immediately outside of the extension will see this as some form of constant velocity outlet boundary. This is a loose form of boundary condition and the velocity felt by the particles immediately outside of the extension is not exactly equal to the Outlet region velocity. The pressure immediately outside the extension will adjust itself to support the flow through the extension. Applying zero velocity in velocity type extension will result in a clogged Outlet region.
- Acceleration - When using acceleration extension type, the extension sets the normal component of particle acceleration to the specified value. The particle acceleration is free to evolve in directions perpendicular to the Outlet regions normal direction. For particles immediately outside of the extension, the particles in the extension represent a form of outlet boundary with constant acceleration. The pressure immediately outside the extension will adjust itself to support the flow through the extension.
Start Time / End Time: Specifies the start and finish times which define the window where the Outlet region is active.
Ramp Up / Down Time: This parameter specifies a time window for the acceleration and deceleration of the fluid. At the start time, the flow will ramp up from zero to the specified value over this time. If ramp down is specified, the velocity will ramp back down to zero prior to the end time. This minimizes pressure fluctuations and instabilities caused by instantaneous changes in velocity.
Extendent Length (dx): The length of the extended region in terms of particle spacing.
Material: Outlet regions can be set to apply only to specific phases. For example, removing one fluid only. It is also possible to specify wall phases. In this situation, an opening can be created in the wall by the Outlet region.
Other Options: A free text box where additional parameters can be specified.

Regions

Define any number of regions to alter/prescribe velocity, acceleration, porous media or temperature.

Velocity

Analysis > Boundary Conditions > Regions > Velocity

The Imposed Velocity tool is used to define an arbitrary number of regions to define fluid velocity.

The fluid velocity region can be specified in a rectangular or spherical shape, and it hard-imposes a velocity on all fluid particles which are within the prescribed region. The easiest analogy is a pump mechanism (momentum source), except that there are no moving parts involved.

Create Impose Velocity Region in SimLab

Name: Impose velocity region name.
Region Type: Specifies the type of the impose velocity region.
Velocity Type:
- Constant - Imposed velocity inside the region.
- Time Series - Defines variable velocity inside the imposed region.
Parabolic velocity: Enables a parabolic velocity profile when cylindrical imposed velocity regions are used.
Cylinder cap: Controls adding hemispherical caps on the cylinder bases (resulting in a pill-shape geometry). The caps are added to both sides of the cylinder.
Start Time/ End Time: Specifies the start and finish times which define the window where the impose region is active.
Damping Time: This parameter specifies a time window for the acceleration of the fluid. At the start time the velocity will ramp up from zero to the specified value over this time. This minimizes pressure fluctuations and instabilities caused by instantaneous changes in velocity.
Advanced Options:
- Mode - Defines the mode of the impose region, are the specified values added or set inside the impose region. Options are SET, ADD.
- Constraint - Defines the constraint of the impose region, are the specified values strictly or loosely imposed in the region. Options are: LOOSE, STRICT.
- Moving body motion to follow - Impose regions can follow a MOVINGWALL phase with a predefined motion.

Impose Acceleration

Analysis > Boundary Conditions > Regions > Acceleration

Imposes a defined acceleration on all the particles which are within the defined region. It also can be thought of as a momentum source region, except that by defining the acceleration instead of hard setting the velocity of the particles, the region is likely to behave more stable.

The fluid acceleration region can be specified in a cuboid (parallelepiped), or cylindrical shape and it hard-imposes acceleration on all particles which are within the prescribed region.

Create Impose Acceleration Region in SimLab

Name: Impose acceleration region name.
Region Type: Specifies the type of the impose acceleration region.
Acceleration Type:
- Constant - Imposed acceleration inside the region.
- Time Series - Defines variable acceleration inside the imposed region.
Cylinder cap: Controls adding hemispherical caps on the cylinder bases (resulting in a pill-shape geometry). The caps are added to both sides of the cylinder.
Start Time/ End Time: Specifies the start and finish times which define the window where the impose region is active.
Damping Time: Damping time of the prescribed acceleration.
Advanced Options:
- Mode - Defines the mode of the impose region, are the specified values added or set inside the impose region. Options are SET, ADD.
- Constraint - Defines the constraint of the impose region, are the specified values strictly or loosely imposed in the region. Options are: LOOSE, STRICT.
- Moving body motion to follow - Impose regions can follow a MOVINGWALL phase with a predefined motion.
Other Options: A free text box where additional parameters can be specified.

Impose Porous

Analysis > Boundary Conditions > Regions > Porous

Porous media definition follows the well-known Darcy-Forchheimer model and allows for definition of volume averaged isotropic or non-isotropic porous media.

It is generally assumed (default) that the principal axes of the porous region align with the base simulation X, Y, and Z coordinates (inertial reference frame). If that is not the case, a separate coordinate system can be defined and the values defining porosity will be considered in that new coordinate system.

There are two parameters which define the volume averaged porosity of the region:

porous_inert: This command defines the diagonal inertial coefficients in the Darcy-Forchheimer porosity model. If the values of this vector are all set to 0.0 and all the components of porous_visc are set to non-zero, then the used porosity model effectively becomes the Darcy model/equation. Given that nanoFluidX supports non-isotropic porous media, this coefficient is a 3-component vector value of the form X Y Z.
porous_visc: This command defines the diagonal inertial component coefficient in the Darcy-Forchheimer porosity model.
Given that nanoFluidX supports non-isotropic porous media, this coefficient is a 3-component vector value of the form X Y Z.

Create Impose Porous region in SimLab

Name: Impose porous region name.
Region Type: Specifies the type of porous region.
Start Time/ End Time: Specifies the start and finish times which define the window where the impose region is active.
Advanced Options: Moving body motion to follow - Impose regions can follow a MOVINGWALL phase with a predefined motion.
Other Options: A free text box where additional parameters can be specified.