# Marine Propeller - CFD Simulation

Source: https://help.sim-flow.com/tutorials/propeller
Last updated: 2026-10-14

![front-image](https://help.sim-flow.com/tutorials/images/marine-propeller.png)

## 1. Introduction

In this tutorial, we will be modeling a quarter of the propeller due to the double symmetry condition. You will also learn how to create a *Cell Zone* (sub-volume in the fluid zone), which marks the location of the rotating zone. We use the MRF model to introduce a pseudo-rotation of the propeller. The propeller will be solved in a rotating reference frame, and by this we introduce artificial motion. It is less accurate than resolving motion directly but is more efficient and allows for steady-state simulation of rotating parts. In advanced postprocessing using ParaView, we show you how to create an iso-surface of the Q-criterion.

## 2. Download SimFlow

SimFlow is a general-purpose [CFD Software](https://sim-flow.com/download/cfd-simulation-software/)

To follow this tutorial, you will need the SimFlow free version. You may download it via the following link:
[Download SimFlow](https://sim-flow.com/download-simflow/)

## 3. Create Case

Open SimFlow and create a new case named *propeller*

1. Click **New**
2. Provide name `propeller`
3. Click **Create** to open a new case

![simflow-launcher](https://help.sim-flow.com/tutorials/images/launcher-propeller.png)

## 4. Import Geometry - Propeller

After creating the case, [Download GeometryPropeller](https://help.sim-flow.com/tutorials/downloads/propeller/propeller.stl.gz)

1. Click **Import Geometry**
2. Select geometry file *propeller.stl.gz*
3. Click **Open**

![pp 2 import geometry](https://help.sim-flow.com/tutorials/images/propeller/pp-2-import-geometry.png)

## 5. Imported Geometry Units

The STL format does not contain the unit information which is defined during the geometry export. Therefore, you must manually specify the correct unit after import. If we do not know the exported unit, we can estimate it based on the total size of the model. It is displayed next to the *Geometry size* label. In our case, the default unit meter is correct.

1. To confirm default unit *meter*, press **OK**

![pp 2 unit](https://help.sim-flow.com/tutorials/images/propeller/pp-2-unit.png)

## 6. Propeller Geometry

After importing the geometry, it will appear in the 3D window.

1. Click **Fit View** to zoom the geometry

![pp 3 geometry](https://help.sim-flow.com/tutorials/images/propeller/pp-3-geometry.png)

## 7. Domain Boundary

We need to create a cylindrical boundary for the domain. For this purpose, we will create a cylindrical geometry for later use in the meshing process.

1. Click *Create Cylinder*
2. Rename *cylinder_1* to `external`
   (double-click on the name to rename it, press enter to apply)
3. Click *Properties* button if properties panel is not displayed
4. Set origin, axis, and length of the cylinder accordingly
   *Origin \({\sf [m]}\)*`-1e-03``0``0`
   *Axis \({\sf [-]}\)*`1``0``0`
   *Length \({\sf [m]}\)*`1.502`

![pp 4 domain boundary](https://help.sim-flow.com/tutorials/images/propeller/pp-4-domain-boundary.png)

## 8. Refinement Area (I)

To better resolve the flow near the propeller, we will create an area with a higher mesh resolution. To do this, we will create a new geometry by copying settings from the external geometry.

1. Click *Options* of the *external* geometry
2. Select *Duplicate* option

![pp 5 refinement area one](https://help.sim-flow.com/tutorials/images/propeller/pp-5-refinement-area-one.png)

## 9. Refinement Area (II)

1. Click *Properties* if they are not displayed
2. Rename *external_1* to `refine`
3. Set radius of the refinement geometry
   *Radius \({\sf [m]}\)*`0.3`

![pp 6 refinement area two](https://help.sim-flow.com/tutorials/images/propeller/pp-6-refinement-area-two.png)

## 10. Display Geometries

In order to see all geometries, we will decrease the opacity of the external and refine.

1. Select *external*
2. Click *Display Properties*
3. Adjust *Opacity* to *50%*
4. Adjust opacity to 50% for *refine* geometry by repeating previous steps

![pp 7 geometry one](https://help.sim-flow.com/tutorials/images/propeller/pp-7-geometry-one.png)

## 11. Meshing Parameters - External

Once the geometry is prepared, we can define the meshing properties. Meshing will be enabled for the external geometry, as it serves as the outer boundary of the analysis domain.

1. Go to *Hex Meshing* panel
2. Enable *Mesh Geometry* on *external* geometry

![pp 8 meshing parameters external](https://help.sim-flow.com/tutorials/images/propeller/pp-8-meshing-parameters-external.png)

## 12. Meshing Parameters - Propeller

To better capture the flow around the blades, we refine the mesh near the propeller geometry by defining minimum and maximum refinement levels and applying a boundary layer mesh.

1. Select *propeller* geometry
2. Enable *Mesh Geometry*
3. Enable *Create Boundary Layer Mesh*
4. Set *Refinement* to *Min 3* *Max 4*

![pp 9 meshing parameters propeller](https://help.sim-flow.com/tutorials/images/propeller/pp-9-meshing-parameters-propeller.png)

## 13. Meshing Parameters - Refine

We apply mesh refinement in the region influenced by the propeller-induced flow.

1. Select *refine* geometry
2. Enable *Mesh Geometry*
3. Set refinement *Level* to `2`

![pp 10 meshing parameters refine](https://help.sim-flow.com/tutorials/images/propeller/pp-10-meshing-parameters-refine.png)

## 14. Base Mesh

We want to create a mesh of only one blade of the propeller. For this purpose, we will create a base mesh covering only one-fourth of the geometry.

1. Go to the *Base* tab
2. Define base mesh minimum and maximum extent
   *Min \({\sf [m]}\)*`0``0``0`
   *Max \({\sf [m]}\)*`1.5``1``1`
3. Define Division along each axis
   *Division*`30``20``20`

![pp 11 base mesh](https://help.sim-flow.com/tutorials/images/propeller/pp-11-base-mesh.png)

## 15. Base Mesh Boundaries

1. 2 Define boundary names accordingly
   *X-* *inlet*
   *X+* *outlet*
   *Y-* *right*
   *Z-* *left*

![pp 12 base mesh boundaries](https://help.sim-flow.com/tutorials/images/propeller/pp-12-base-mesh-boundaries.png)

## 16. Material Point

The material point indicates which side of the geometry the mesh will be retained on. Since we are simulating water flow around the propeller, the material point must be placed outside the propeller geometry.

1. Go to *Point* tab
2. Set location of the material point
   *Material Point*`0.5``0.5``0.5`

![pp 13 material point](https://help.sim-flow.com/tutorials/images/propeller/pp-13-material-point.png)

## 17. Start Meshing Process

In this step, we will initiate the meshing process.

In the meshing panel, you may indicate how many CPUs you would like to use for this process. Please note that if you are using the SimFlow free version, you may only use serial meshing, and you may not create meshes larger than 200'000 nodes.

If you would like to test the full version [Request 30-day Trial](https://license.sim-flow.com/trial)

1. Go to *Mesh* tab
2. Start the meshing process with **Mesh** button

![pp 14 start meshing](https://help.sim-flow.com/tutorials/images/propeller/pp-14-start-meshing.png)

## 18. Mesh

After the meshing process is finished, the mesh should appear on the screen.

![pp 15 mesh](https://help.sim-flow.com/tutorials/images/propeller/pp-15-mesh.png)

## 19. Boundary Types

After creating the mesh, we have to set proper boundary types.

1. Go to *Mesh* panel
2. Change the boundary type of the *external* geometry to *patch*
3. Ensure that the remaining boundary types are selected appropriately

![pp 2 7 boundary types](https://help.sim-flow.com/tutorials/images/propeller/pp-2-7-boundary-types.png)

## 20. Boundary Interface (I)

As we will be simulating only one blade of the propeller, we have to create a boundary interface to make the model periodic.

1. Hold `CTRL` key and select *left* and *right* boundaries
2. Click *Create Arbitrary Interface* between left and right boundaries

![pp 2 8 boundary interface one](https://help.sim-flow.com/tutorials/images/propeller/pp-2-8-boundary-interface-one.png)

## 21. Boundary Interface (II)

1. Expand the interface properties
2. Change Transform type to *Rotational*
3. Define Rotation Axis
   *Rotation Axis*`1``0``0`

![pp 2 9 boundary interface two](https://help.sim-flow.com/tutorials/images/propeller/pp-2-9-boundary-interface-two.png)

## 22. Simulation Type

We want to analyze the water flow around a marine propeller. For this purpose, we will use a single-phase, steady-state simulation of incompressible turbulent flow with Multiple Reference Frame (MRF).

![Simulation Panel](https://help.sim-flow.com/assets/images/go-to-simulation-panel@2x.png)

![Step 1](https://help.sim-flow.com/assets/images/solvers-selection/simpleFoam/01_single_phase@2x.png)

![Step 2](https://help.sim-flow.com/assets/images/solvers-selection/simpleFoam/02_low_speed@2x.png)

![Step 3](https://help.sim-flow.com/assets/images/solvers-selection/simpleFoam/03_steady-state@2x.png)

![Step 4](https://help.sim-flow.com/assets/images/solvers-selection/simpleFoam/04_apply@2x.png)

## 23. Turbulence Model

For the purpose of this tutorial, we will simulate the turbulence phenomenon using the *\(Realizable \; k{-} \varepsilon\)* model.

1. Go to *Turbulence* panel
2. Select *RANS* modeling
3. Select *\(Realizable \; k{-} \varepsilon\)* turbulence model

![pp 2 2 turbulence model](https://help.sim-flow.com/tutorials/images/propeller/pp-2-2-turbulence-model.png)

## 24. Water Properties

As a fluid material, we will use water.

1. Go to *Transport Properties* panel
2. Open **Material Database**
3. Pick up *water* from the list
4. Click **Apply**

Selecting material from the *Material Database* will fill all inputs in the *Transport Properties* panel. We are still able to overwrite these values at any time.

![pp 2 3 water properties](https://help.sim-flow.com/tutorials/images/propeller/pp-2-3-water-properties.png)

## 25. Cell Zones for MRF (I)

To be able to model propeller rotation, we will take advantage of a rotating reference frame. This technique will allow modeling the propeller rotation without the need to rotate the mesh. The rotating reference frame can only be applied to a sub-region of the mesh defined by a cell zone object (a list of mesh cells). Therefore, we will first create a cell zone.

1. Go to *Mesh* panel
2. Expand list of options from the *default* region
3. Select *Add Cell Zones* from the menu

![pp 2 4 cell zones for mrf one](https://help.sim-flow.com/tutorials/images/propeller/pp-2-4-cell-zones-for-mrf-one.png)

## 26. Cell Zones for MRF (II)

For the purpose of this tutorial, we will use the whole mesh as the rotating zone. To do this, we need to create the cell zone inside the external geometry.

1. Select *external* geometry
2. Click **Create Cell Zones**

![pp 2 5 cell zones for mrf two](https://help.sim-flow.com/tutorials/images/propeller/pp-2-5-cell-zones-for-mrf-two.png)

## 27. Rotating Reference Frame

The rotating reference frame should be aligned with the negative X-axis, and all boundaries except the propeller should be treated as stationary.

1. Go to *Cell Zones* panel
2. Enable *Rotating Reference Frame* for *external* zone
3. Define Axis of the propeller
   *Axis*`-1``0``0`
4. Select boundaries that will not be defined in the rotating frame of reference
   *Static Boundaries*:
   *external*
   *inlet*
   *left*
   *outlet*
   *right*

![pp 2 6 rotating reference frame](https://help.sim-flow.com/tutorials/images/propeller/pp-2-6-rotating-reference-frame.png)

## 28. Boundary Conditions - External (Turbulence)

Next, we define the boundary conditions. Since the flow is driven by the rotating propeller, the external boundary should be set to a pressure inlet. Adjust only the turbulent intensity as follows.

1. Go to *Boundary Conditions* panel
2. Select *external* boundary
3. Select *Turbulence* tab
4. Set *Turbulence Intensity* to `1e-02`

![pp 2 10 boundary conditions external turbulence](https://help.sim-flow.com/tutorials/images/propeller/pp-2-10-boundary-conditions-external-turbulence.png)

## 29. Boundary Conditions - Inlet

We will use the same boundary conditions for inlet and external boundaries. To achieve this, we can copy settings from the external boundary to the inlet.

1. Make sure you have selected the *external* boundary
2. Click *Copy Boundary Conditions*
3. Select *inlet* boundary
4. Click **Copy**

![pp 2 11 boundary conditions inlet](https://help.sim-flow.com/tutorials/images/propeller/pp-2-11-boundary-conditions-inlet.png)

## 30. Boundary Conditions - Outlet

1. Change *outlet* character to *Outflow*

![pp 2 12 boundary conditions outlet fresh](https://help.sim-flow.com/tutorials/images/propeller/pp-2-12-boundary-conditions-outlet-fresh.png)

## 31. Monitor Forces

We will monitor the solution progress by tracking the forces acting on the propeller.

1. Go to *Monitors* panel
2. Select *Forces* tab
3. Expand *Monitored Boundaries* list and select *propeller*

![pp 2 13 monitor forces](https://help.sim-flow.com/tutorials/images/propeller/pp-2-13-monitor-forces.png)

## 32. Run - Time Control

Finally, we can start our computation.

1. Go to *Run* panel
2. Set *Number of Iterations* to `1000`

![pp 2 14 run simulation 1](https://help.sim-flow.com/tutorials/images/propeller/pp-2-14-run-simulation-1.png)

## 33. Run - CPU

To speed up the calculation process, take advantage of parallel computing and increase the number of CPUs based on your PC’s capability. The free version allows you to use only one processor (serial mode). To get the full version, you can use the contact form to [Request 30-day Trial](https://license.sim-flow.com/trial)

Estimated computation time for serial mode: 15 minutes

1. Switch to *CPU* tab
2. Click **Run Simulation** button

![run cpu serial](https://help.sim-flow.com/tutorials/images/run-cpu-serial.png)

## 34. Monitor Solution - Force

Check if a solution converges by observing stabilization of forces on the propeller boundary.

1. Click on *Forces* tab to display Force Monitor

![pp post 0 monitor solution force](https://help.sim-flow.com/tutorials/images/propeller/pp-post-0-monitor-solution-force.png)

## 35. Calculate Additional Fields

When a simulation is finished, we want to calculate an additional solution field to be used in postprocessing.

1. Go to *Calculate* panel
2. Select *Q Criterion* field
3. **Calculate** the field

Please note: After clicking the Calculate button, SimFlow will calculate the new flow variable, which will be stored in your project folder and will be accessible in ParaView.

![pp post 00 calculate](https://help.sim-flow.com/tutorials/images/propeller/pp-post-00-calculate.png)

## 36. Start Postprocessing with ParaView

After computations are finished, we can do complex visualization of our results with ParaView.

1. Go to *Postprocessing* panel
2. Run *ParaView*

![pp post 1 start paraview](https://help.sim-flow.com/tutorials/images/propeller/pp-post-1-start-paraview.png)

## 37. ParaView - Load Results

Now we are loading results into ParaView.

1. Click *Last Frame* to select the last result set
2. Click **Apply** to load results into ParaView
3. After loading results, they will be shown in the 3D graphics window

![pp post 2 paraview load results](https://help.sim-flow.com/tutorials/images/propeller/pp-post-2-paraview-load-results.png)

## 38. ParaView - Display Q Contour (I)

To show the propeller, we will now create a contour.

1. Make sure you have your case selected
2. Click *Contour*

![pp post 3 create contour](https://help.sim-flow.com/tutorials/images/propeller/pp-post-3-create-contour.png)

## 39. ParaView - Display Q Contour (II)

1. Set *Contour by* to *Q*
2. Set contour range to ` 500 ` and click enter
   (double-click to edit visible value)
3. Click **Apply** to create new contour
4. After applying changes, the contour will be shown in the 3D window

![pp post 4 create contour two](https://help.sim-flow.com/tutorials/images/propeller/pp-post-4-create-contour-two.png)

## 40. ParaView - Show Full Propeller (I)

As you can see, there is only a quarter of the propeller visible, and we would like to show the full geometry. In order to do that, we have to duplicate and transform a partial propeller.

1. Make sure you have *Contour1* selected
2. From the *Sources* Menu select *Search* option to open a search window
3. Start typing the word *transform*
4. Select *Transform* option
5. Make sure you have *Transform1* selected
6. Define *90* degree rotation about the X axis and click enter
7. Click **Apply** 2 times to create transformation

![pp post 5 transform 1](https://help.sim-flow.com/tutorials/images/propeller/pp-post-5-transform-1.png)

## 41. ParaView - Show Full Propeller (II)

We have to repeat the previous step to make another transformation - Transform1 → Transform2

1. Make sure you have *Transform1* selected
2. From the *Sources* Menu select *Search* option to open a search window
3. Start typing the word *transform*
4. Select *Transform* option
5. Make sure you have *Transform2* selected
6. Define *90* degree rotation about the X axis and click enter
7. Click **Apply** 2 times to create transformation

![pp post 6 transform 2](https://help.sim-flow.com/tutorials/images/propeller/pp-post-6-transform-2.png)

## 42. ParaView - Show Full Propeller (III)

We have to repeat the previous step to make another transformation - Transform2 → Transform3

1. Make sure you have *Transform2* selected
2. From the *Sources* Menu select *Search* option to open a search window
3. Start typing the word *transform*
4. Select *Transform* option
5. Make sure you have *Transform3* selected
6. Define *90* degree rotation about the X axis and click enter
7. Click **Apply** 2 times to create transformation

![pp post 7 transform 3](https://help.sim-flow.com/tutorials/images/propeller/pp-post-7-transform-3.png)

## 43. Display Full Propeller

To make the full geometry visible, we have to change the visibility of all geometries.

1. Make sure the contour and all its transformations are visible
2. Select *Contour1*
3. Choose pressure *p* from the coloring list
4. Click *Toggle Color Legend Visibility* and choose *Blue to Red Rainbow*
5. Choose pressure *p* for the remaining quarters

![pp 34 paraview show full propeller three 1](https://help.sim-flow.com/tutorials/images/propeller/pp-34-paraview-show-full-propeller-three-1.png)

## 44. Final Results

In the 3D view, the contour of the full propeller should appear.

![pp 35 paraview contour new](https://help.sim-flow.com/tutorials/images/propeller/pp-35-paraview-contour-new.png)

## 45. Advanced Postprocessing with ParaView

This concludes the tutorial, covering all the aspects we intended to showcase. For a finely tuned presentation of the results, you may take advantage of the more advanced features.

In ParaView, you can display streamlines, contour plots, vector fields, line or time plots, calculate volume or surface integrals and create animations.

To familiarize yourself with the ParaView capabilities, it’s worth checking out our video tutorial, *Paraview CFD Tutorial - Advanced Postprocessing in ParaView*, in which we demonstrate some of the most commonly used postprocessing techniques.

[Paraview CFD Tutorial - Advanced Postprocessing in ParaView](https://www.youtube.com/watch?v=5M6VgXyHB60&list=PLy7xPqn9xXckoD2gZgPpv8mrxillJ9PWU&index=21)