Domain Setup

Domain Setup#

The domain defines the region of space that will be meshed. Different simulation types require different domain configurations. Domain setup is done in the Setup tab of your project workspace.

Domain Types#

External Flow#

For simulating flow around an object — vehicles, aircraft, buildings, bluff bodies.

Studio generates a Cartesian bounding box (wind tunnel) around your geometry with configurable padding:

Parameter

Description

Default

Upstream

Distance ahead of geometry

1.5× geometry length

Downstream

Distance behind geometry (wake capture)

3.0× geometry length

Side (left/right)

Lateral distance

1.5× geometry width

Top

Distance above

2.0× geometry height

Bottom

Distance below

0× (geometry on ground)

Options:

  • Ground plane — Places the geometry on a flat ground surface. Essential for vehicle aerodynamics where ground effect matters.

  • Symmetry plane — Meshes only half the domain and mirrors results. Halves compute cost for symmetric geometries.

Tip

For vehicle aerodynamics, use a ground plane and ensure the bottom padding is 0 so the car sits on the ground. For aircraft, increase the bottom padding to avoid ground interference.

How it works in the backend:

When you select External Flow, the mesher:

  1. Constructs the Cartesian domain bounding box from the padding parameters

  2. Loads the uploaded geometry as a closed surface

  3. Runs a fluid/solid classification step — the geometry surface defines the interior (solid) region, and the volume between the geometry and the domain box is the fluid region

  4. Applies the block AMR hierarchy to the fluid region, refining near the geometry surface using cut-cells

  5. Named selections for domain boundary faces (inlet, outlet, top, sides) are assigned automatically based on their position relative to the flow direction

Internal Flow#

For simulating flow inside a geometry — pipes, ducts, manifolds, enclosures, HVAC systems.

The domain is defined by the interior volume of your geometry. Studio automatically:

  • Identifies the fluid volume enclosed by the surfaces

  • Detects inlet and outlet faces (the open ends of the geometry)

  • Sizes the mesh based on the smallest internal dimension

How it works in the backend:

When you select Internal Flow:

  1. The mesher computes the enclosed interior volume of the uploaded geometry

  2. Inlet and outlet surfaces are identified as open faces (holes in the surface) or by named selections you assign in the Surfaces tab

  3. The Cartesian block AMR grid is constructed to fill the interior volume

  4. Cut-cells are formed where the Cartesian grid intersects the interior walls

  5. Interior wall surfaces automatically become wall-type boundary patches

Note

For internal flow geometries, the geometry must be watertight except at the intended inlet and outlet openings. Any gap in the surface other than at inlets/outlets will allow fluid to escape the domain and cause the mesher to fail to identify the correct interior.

Rotating Machinery#

For rotating equipment — fans, pumps, turbines, compressors, propellers.

This domain type creates:

  • A rotating zone around the moving geometry (MRF — Multiple Reference Frame)

  • A stationary zone for the surrounding fluid

  • An interface between the zones

Configure the rotation axis, speed (RPM), and zone dimensions in the Setup tab.

How it works in the backend:

The rotating zone is meshed as a cylindrical sub-domain, and the AMR block hierarchy is constructed independently within each zone. At the rotating/stationary interface, a non-conformal interface is created — values are interpolated across the zone boundary using an area-weighted flux exchange. This approach is used for steady-state simulations (frozen-rotor). For transient sliding mesh, the interface is updated each time step.

Conjugate Heat Transfer (CHT)#

For problems involving heat exchange between fluid and solid regions — heat sinks, cold plates, electronics cooling.

CHT domain setup requires:

  • At least two regions (one fluid, one solid)

  • Properly defined interfaces between touching regions

  • Material properties for each region

Solid Body#

For meshing the interior of a solid geometry — used for thermal analysis or structural simulations without fluid flow.

Domain Shapes#

The enclosing domain can take different shapes depending on your application:

Shape

Best For

Box

Vehicle aerodynamics, buildings, general external flow

Cylinder

Axisymmetric bodies, rotors, vertical structures

C-Domain

Airfoils and 2D-like aerodynamics

O-Domain

Cylinders, cables, circular cross-sections

Configuring the Domain#

Automatic Sizing#

When you select a domain type, Studio automatically sizes the domain based on your geometry’s bounding box. The defaults work well for most cases.

Manual Adjustment#

You can adjust the domain in two ways:

  1. Numerical input — Enter exact dimensions in the Setup panel

  2. 3D viewer — Drag the domain box handles directly in the viewer

Domain Visualization#

The domain boundary appears as a semi-transparent box in the 3D viewer. You can:

  • See the geometry positioned within the domain

  • Verify adequate clearance on all sides

  • Check that the domain is large enough to avoid boundary interference

Domain Size Guidelines

Too small: Boundary effects contaminate the solution. Flow doesn’t develop properly before hitting the outlet.

Too large: Wastes cells on far-field regions, increasing compute cost without improving accuracy near the geometry.

The defaults strike a good balance for most applications. Increase downstream distance for bluff bodies with large wakes.

Named Selections#

Named selections (also called boundary patches) are how Studio identifies different surface regions for boundary condition assignment. When you generate a mesh, every face on the domain boundary belongs to a named selection.

Studio automatically creates named selections for domain boundaries:

Named Selection

External Flow

Internal Flow

inlet

Upstream face of the domain box

Open inlet face(s) of the geometry

outlet

Downstream face of the domain box

Open outlet face(s) of the geometry

top

Top face of the domain box

—

side_left, side_right

Side faces

—

ground

Bottom face (if ground plane enabled)

—

symmetry

Symmetry cut plane (if enabled)

—

Geometry surfaces

Automatically from CAD face names

Interior walls

You can view and rename all named selections in the Surfaces tab. See Surfaces for full details.

Meshing Time#

Once you click Generate Mesh, the job is dispatched to cloud GPUs. Typical generation times:

Mesh Size

Typical Time

< 5 million cells

1 – 3 minutes

5 – 20 million cells

3 – 8 minutes

20 – 100 million cells

8 – 30 minutes

> 100 million cells

30 minutes – 1 hour

These are approximate. Actual time depends on:

  • Geometry complexity — More surface features and curvature require more cut-cell processing

  • AMR depth — More refinement levels increase both cell count and the number of block classification operations

  • Number of refinement zones — Each zone adds an additional refinement pass

  • Domain size — Larger domains with more coarse-level blocks take longer to initialize

Tip

For a rough estimate: expect 1–10 million cells per minute of meshing time, with complex high-AMR meshes at the lower end and simple geometries at the upper end.

You can monitor meshing progress and intermediate cell counts in the Logs panel.

Contents