Slice Output

Slice Output#

Slice Output in Flow360 allows you to visualize flow field variables on 2D cutting planes through the computational domain. The data is interpolated from the three-dimensional flow solution field onto the two-dimensional slice plane. This provides detailed insight into flow features at specific locations, while generating much smaller files than full volume outputs.

Available Options#

Option

Description

Applicable

Output fields

Flow variables to include in the output

always

Output format

Format for saving output data

always

Save interval

When to save outputs

always

Frequency

How often to save outputs

when Save interval is Custom

Frequency offset

The time step at which to start the output

when Save interval is Custom

Assigned slices

Define one or more slice planes by specifying their origin and normal vector

always

Global Time Stepping in Child Cases#

When working with child cases (cases forked from a parent simulation), it’s important to understand that the Frequency and Frequency offset parameters refer to the global time step, which is transferred from the parent case.

Example: If the parent case finished at time_step=174, the child case will start from time_step=175. If Frequency=100 is set in the child case, the output will be saved at global time steps 200 (25 time steps into the child simulation), 300 (125 time steps into the child simulation), etc. Frequency offset also refers to the global time step, meaning that if in the previously mentioned child case, Frequency offset=50 was set (with Frequency=100), the output would be saved at global time steps 250 (75 time steps into the child simulation), 350 (175 time steps into the child simulation), etc.

Detailed Descriptions#

Output fields#

Select the flow variables to include in the output files.

  • Default: None (must select at least one)

  • Example: Cp, Mach, velocity

Note: See complete list of available fields below.

Output format#

The file format for saving the slice data.

  • Default: paraview

  • Options:

    • paraview

    • tecplot

    • both

Notes:

  • Choose the format that best suits your post-processing workflow.

  • Select paraview for .vtu format, tecplot for .plt format, or both to save in both formats.

Save interval#

Choose the points in the simulation where the results are saved.

  • Default: Save at end

  • Options:

    • Save at end

    • Custom (only available when Time stepping is Unsteady)

Notes:

  • Choose Save at end to save only the final results of the simulation.

  • Choose Custom to save the results in given intervals.

Frequency#

How often to save outputs, measured in number of physical time steps.

  • Default: -1 (only at the end of simulation)

  • Example: 100 — saves output every 100 physical time steps.

    • Standalone case: If you start a simulation from time_step=0 with frequency=100, outputs are saved at time steps 100, 200, 300, etc.

    • Parent-child case: If the parent finished at time_step=174, the child starts from time_step=175. With frequency=100 in the child, outputs are saved at global time steps 200 (25 steps into child), 300 (125 steps into child), 400 (225 steps into child), etc.

Notes:

  • For steady simulations, use -1 to save only at end of run. For unsteady simulations, set a positive value to create the data required for an animation.

  • Important for child cases - this parameter refers to the global time step (see Global Time Stepping).

  • This setting is only applicable for unsteady cases.

Frequency offset#

The time step at which to start the output animation.

  • Default: 0 (beginning of simulation)

  • Example: 1000 — with frequency=100, outputs are saved at time steps 1000, 1100, 1200, etc.

    • Standalone case: If you start a simulation from time_step=0 with frequency=100 and frequency_offset=1000, outputs are saved at time steps 1000, 1100, 1200, etc.

    • Parent-child case: If the parent finished at time_step=174, the child starts from time_step=175. With frequency=100 and frequency_offset=200 in the child, outputs are saved at global time steps 200 (25 steps into child), 300 (125 steps into child), 400 (225 steps into child), etc.

Notes:

  • Useful for skipping initial transient phases in unsteady simulations.

  • Important for child cases - this parameter refers to the global time step (see Global Time Stepping).

  • This setting is only applicable for unsteady cases.

Assigned slices#

Define one or more slice planes through the computational domain.

  • Definition parameters:

    • Name: A unique identifier for the slice

    • Origin: The 3D coordinates of a point on the slice plane

    • Normal: The normal vector to the slice plane (does not need to be normalized)

  • Example:

    Name: "Midspan"
Origin: (0, 5, 0)
Normal: (0, 1, 0)

Note: Multiple slices can be defined, each with unique name, origin, and normal.

Available Output Fields#

Variables from Available Output Fields and the following specific variables

Volume-Specific Variables#

  • betMetrics - BET Metrics

  • betMetricsPerDisk - BET Metrics per Disk

  • linearResidualNavierStokes - Linear residual of Navier-Stokes solver

  • linearResidualTurbulence - Linear residual of turbulence solver

  • linearResidualTransition - Linear residual of transition solver

  • SpalartAllmaras_hybridModel - Hybrid RANS-LES output for Spalart-Allmaras solver (supports both DDES and ZDES)

  • kOmegaSST_hybridModel - Hybrid RANS-LES output for kOmegaSST solver (supports both DDES and ZDES)

  • localCFL - Local CFL number

Hybrid RANS-LES Output Variables#

For detailed information about the SpalartAllmaras_hybridModel and kOmegaSST_hybridModel output fields and their DDES and ZDES variables, see the Hybrid RANS-LES Output Variables section in Volume Output.

💡 Tips

Key Output Fields for Slice Analysis#

  • Total Pressure Coefficient (Cpt)

    • Effectively shows boundary layer development and growth

    • Clearly reveals flow separation regions

    • Highlights wakes behind objects

    • Indicates regions of energy loss in the flow

    • Can be used to identify vortices and other flow structures

    To calculate the dimensional total pressure from Cpt:

    p_t (N/m²) = Cpt × (1/2)ρ∞ × U_ref² + p_t∞

  • Mach Number and Velocity Fields

    • Excellent for visualizing shock waves

    • Shows expansion regions

    • Reveals flow acceleration and deceleration zones

    • Indicates boundary layer thickness

Common Slice Orientations#

  • XY Plane: Normal = (0, 0, 1)

  • YZ Plane: Normal = (1, 0, 0)

  • XZ Plane: Normal = (0, 1, 0)

Strategic Slice Placement#

Place slices at these key locations for maximum insight:

  • Leading and trailing edges of aerodynamic surfaces

  • Maximum thickness locations on wings or bodies

  • Wing-body junctions to visualize corner flow

  • Wake regions behind objects (at various downstream distances)

  • Boundary layer regions (parallel to surface)

  • Shock wave locations (approximately perpendicular to flow)

Visualization Recommendations#

  • For boundary layer analysis: Use Cpt with a color scale that highlights low values

  • For shock detection: Use Mach or pressure with carefully adjusted color scales

  • For vortex visualization: Use vorticityMagnitude or velocity vector plots

  • For separation detection: Look for reversal in velocity vectors or negative streamwise velocity

  • For BET analysis: Position slices at specific radial positions of the rotor disk

❓ Frequently Asked Questions

  • How many slices can I create in a single simulation?

    There is no hard limit on the number of slices, but each additional slice increases the output file size and computational overhead. For best performance, limit slices to key areas of interest.

  • Can I create slices at angles that aren’t aligned with the coordinate axes?

    Yes, by setting the appropriate normal vector. For example, a 45° plane between X and Y axes would use normal = (1, 1, 0).

  • What’s the difference between paraview and tecplot formats?

    Paraview format (.vtu) is for the open-source ParaView visualization tool, while Tecplot format (.plt) is for the commercial Tecplot software. Choose based on your preferred visualization tool.

🐍 Python Example Usage

The following example demonstrates how to configure slice outputs in your simulation using the Flow360 Python API.

import flow360 as fl
from flow360 import u

# Create a simulation setup
simulation = fl.SimulationParams(
    # Other simulation parameters...
)

# Define slice outputs
simulation.outputs.append(
    fl.SliceOutput(
        name="Wing Slices",
        entities=[
            fl.Slice(
                name="Wing Root",
                origin=(0, 0, 0) * u.m,
                normal=(0, 1, 0)
            ),
            fl.Slice(
                name="Midspan", 
                origin=(0, 5, 0) * u.m,
                normal=(0, 1, 0)
            ),
            fl.Slice(
                name="Wingtip",
                origin=(0, 10, 0) * u.m,
                normal=(0, 1, 0)
            )
        ],
        output_format="paraview",
        output_fields=["Mach", "pressure", "vorticity"],
        frequency=100,  # Save every 100 time steps
        frequency_offset=0  # Start saving from beginning of simulation
    )
)

# Create time-averaged slice output
simulation.outputs.append(
    fl.TimeAverageSliceOutput(
        name="Time Averaged Wake",
        entities=[
            fl.Slice(
                name="Wake Slice",
                origin=(2, 0, 0) * u.m,
                normal=(1, 0, 0)  # Normal to flow direction
            )
        ],
        output_fields=["velocity", "Cp", "turbulence"],
        start_step=1000,  # Start averaging from time step 1000
        frequency=500,    # Save every 500 time steps
        frequency_offset=1500  # Start saving from time step 1500
    )
)

Note: For information on time-averaging slice output for unsteady simulations, see Time-Averaged Slice Output.

Contents