# Internal Pipe Flow - CFD Simulation

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

![front-image](https://help.sim-flow.com/tutorials/images/t-joint-connection.png)

## 1. Introduction

The Pipe Flow tutorial serves as an excellent introduction to SimFlow. It primarily concentrates on explaining the fundamental aspects of the software. In this tutorial, we will present the simulation of internal flow through a simple T-pipe geometry (created directly in SimFlow). This simulation will feature a single-phase, incompressible flow, consisting of two inlets and one common outlet.

## 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 *pipe flow*

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

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

## 4. Create Geometry - Cylinder 1

To build a "Pipe" geometry for the simulation, we will make use of SimFlow’s basic geometry module. This module allows for creating and editing primitive geometries (box, cylinder, and sphere).

SimFlow also supports importing complex geometries in well-known formats such as STEP, STL, IGES, and others. However, in this case, we will use a simple pipe geometry.

For this operation, we will need to create two cylinders, which we will unite in further steps into a pipe. Our initial step will involve adding the first cylinder.

1. Go to *Geometry* panel
2. Select *Create Cylinder*
3. Set the cylinder dimensions:
   *Length \({\sf [m]}\)*`0.4`
   *Radius \({\sf [m]}\)*`0.05`

![image](https://help.sim-flow.com/tutorials/images/t-pipe-connection/t-pipe-02-geometry-cylinder1.png)

## 5. Create Geometry - Cylinder 2

In this step, we will create the second cylinder.

1. Select *Create Cylinder*
2. Set the origin and axis:
   *Origin \({\sf [m]}\)*`0``-0.4``0`
   *Axis \({\sf [-]}\)*`0``1``0`
3. Set the cylinder dimensions:
   *Length \({\sf [m]}\)*`1.5`
   *Radius \({\sf [m]}\)*`0.075`

![image](https://help.sim-flow.com/tutorials/images/t-pipe-connection/t-pipe-03-geometry-cylinder2.png)

## 6. Unite Geometries

In this step, we will create a pipe geometry by joining the two cylinders created in prior steps. For this task, we will use a unite tool. This is a geometric boolean operation that will result in a single solid geometry.

1. Select both cylinders with `CTRL` key pressed
2. Click *Unite Geometries*
3. The new geometry will be listed below the cylinders. Double-click on its name and change it from *unite* to `pipe`

![image](https://help.sim-flow.com/tutorials/images/t-pipe-connection/t-pipe-04-unite-geometry.png)

## 7. Geometry - Pipe

The resulting geometry will be displayed in the graphics window.

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

![image](https://help.sim-flow.com/tutorials/images/t-pipe-connection/t-pipe-05-geometry.png)

## 8. Creating Face Group - Inlet 1

In this simulation, we are dealing with an internal flow problem. The imported geometry determines the bounds of the fluid domain. To inform the program where the boundaries of the inlet and outlet mesh should be created, we will use the *Face Groups*.

A *Face Group* is a set of faces that should be distinguished within a geometry. When the geometry containing the face group is used for meshing, an additional boundary is created. The boundary represents the respective face group and inherits its name.

1. Select the first inlet face by holding `CTRL` key and clicking on the geometry face in a 3D view. The selection should be marked in red
2. Click on the *Face Group* button in the graphics context toolbar
3. Press `Esc` or click the **X** button to exit selection mode

![image](https://help.sim-flow.com/tutorials/images/t-pipe-connection/t-pipe-06-face-group-inlet1.png)

## 9. Creating Face Group - Inlet 2

In this step, we will create a face group for the second inlet.

1. Select the second inlet. Press `CTRL` key and click on the face as shown on the slide below
2. Click on the *Face Group* button in the graphics toolbar
3. Press `Esc` or click the **X** button to exit selection mode

![image](https://help.sim-flow.com/tutorials/images/t-pipe-connection/t-pipe-07-face-group-inlet2.png)

## 10. Creating Face Group - Outlet

In order to choose the outlet, we need to rotate the view so that the other end of the geometry becomes visible.

1. Select the outlet face. Press `CTRL` key and click on the face
2. Click on the *Face Group* button in the context toolbar
3. Press `Esc` or click the **X** button to exit selection mode

![image](https://help.sim-flow.com/tutorials/images/t-pipe-connection/t-pipe-08-face-group-outlet.png)

## 11. Rename Face Groups

In the *Geometry Panel*, we can find four *Face Groups* under the *pipe* geometry. The first group, named default, contains all non-selected surfaces. These surfaces will become the pipe walls.

The three additional groups represent the inlets and the outlet of the fluid domain. We will rename those groups to make the resulting boundary names more readable.

1. Select *pipe* geometry
2. Expand *Geometry Faces*
3. Change face group names accordingly (double-click on a group name to start editing)
   *group_1* \(\rightarrow\) `inlet1`
   *group_2* \(\rightarrow\) `inlet2`
   *group_3* \(\rightarrow\) `outlet`

![image](https://help.sim-flow.com/tutorials/images/t-pipe-connection/t-pipe-09-face-group-name.png)

## 12. Meshing Parameters - Pipe

In order to create the mesh, we need to specify the meshing options used for a given geometry. For the pipe, we will add the boundary layer and refine the mesh near edges by level 1.

1. Go to *Hex Meshing* panel
2. Select the *pipe* component
3. Enable *Mesh Geometry*
4. Enable *Create Boundary Layer Mesh*
5. Set surface *Refinement* to *Min 0* *Max 1*

![image](https://help.sim-flow.com/tutorials/images/t-pipe-connection/t-pipe-10-hex-meshing.png)

## 13. Base Mesh - Domain

For the base mesh, we will use a box geometry. As we would like to create the mesh inside the pipe geometry, we need to make the box size a little bigger than the pipe.

1. Go to *Base* tab
2. Click on **Autosize** to adapt box to visible geometries
3. Define the number of divisions
   *Division*`25``200``60`

![image](https://help.sim-flow.com/tutorials/images/t-pipe-connection/t-pipe-11-base-mesh.png)

## 14. Material Point

Material Point tells the meshing algorithm on which side of the geometry the mesh is to be retained.

Since we are considering flow inside the pipe, we need to place the material point inside the geometry. In this case, we do not need to modify the coordinates of the material point, since the default location is already inside the pipe.

![t pipe 11 point](https://help.sim-flow.com/tutorials/images/t-pipe-connection/t-pipe-11-point.png)

## 15. Start Meshing

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

![image](https://help.sim-flow.com/tutorials/images/t-pipe-connection/t-pipe-12-meshing.png)

## 16. Mesh

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

![image](https://help.sim-flow.com/tutorials/images/t-pipe-connection/t-pipe-13-mesh.png)

## 17. Boundaries

To be able to assign inlet and outlet boundary conditions, we have to assign the proper boundary types.

1. Define boundary types accordingly
   *pipe* *wall*
   *pipe_inlet1* *patch*
   *pipe_inlet2* *patch*
   *pipe_outlet* *patch*

![image](https://help.sim-flow.com/tutorials/images/t-pipe-connection/t-pipe-14-mesh-boundaries.png)

## 18. Simulation Type

We want to analyze the water flow through a pipeline. For this purpose, we will use a single-phase, steady-state simulation of incompressible turbulent flow.

![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)

## 19. Turbulence

We are going to use the standard \(k{-}\omega \; SST\) model to resolve turbulence.

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

![image](https://help.sim-flow.com/tutorials/images/t-pipe-connection/t-pipe-16-turbulence.png)

## 20. Transport Properties - Water

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.

![image](https://help.sim-flow.com/tutorials/images/t-pipe-connection/t-pipe-17-transport-properties.png)

## 21. Boundary Conditions - Inlet 1

Now, we will define the inlet and outlet boundary conditions. At the first inlet, we will set constant water velocity.

1. Go to *Boundary Conditions* panel
2. Select *pipe_inlet1* boundary
3. Set the *Velocity Inlet* character
4. Set the inlet velocity
   *U* *Reference Value \({\sf [m/s]}\)*`0.8`

![image](https://help.sim-flow.com/tutorials/images/t-pipe-connection/t-pipe-18-bc-inlet1.png)

## 22. Boundary Conditions - Inlet 2

The second inlet will be defined using a pressure inlet condition. For the pressure value, we will use 1 [kPa].

Note that for the incompressible solver, we operate using kinematic properties. And thus instead of using dynamic pressure, we are going to set a value divided by reference density – kinematic pressure \(m^2/s^2\).

1. Select *pipe_inlet2*
2. Set the total pressure value
   *\(p_0\) \({\sf [m^2 / s^2]}\)*`1`

![image](https://help.sim-flow.com/tutorials/images/t-pipe-connection/t-pipe-19-bc-inlet2.png)

## 23. Boundary Conditions - Outlet

At the outlet, we will apply the pressure outlet character. The pressure value we will leave at the default of 0. For the incompressible flow, pressure is always relative, and we can add any constant (1 atm for example) after computation.

1. Select *pipe_outlet*
2. Set the *Pressure Outlet* character

![image](https://help.sim-flow.com/tutorials/images/t-pipe-connection/t-pipe-20-bc-outlet.png)

## 24. Monitors – Sampling (I)

During calculation, we can observe intermediate results on a section plane. To sample data on a plane, we need to define the plane and also select fields that will be sampled. Note that runtime postprocessing can only be configured before starting calculations and cannot be changed later on.

1. Go to *Monitors* panel
2. Switch to *Sampling* tab
3. Select *Create Slice*
4. Set slice plane normal vector
   *Normal \({\sf [-]}\)*`1``0``0`

![image](https://help.sim-flow.com/tutorials/images/t-pipe-connection/t-pipe-21-monitors-slice.png)

## 25. Monitors – Sampling (II)

Additionally, we need to specify the variables to be sampled.

1. Expand *Fields* list
2. Select pressure *p* and velocity *U*

![image](https://help.sim-flow.com/tutorials/images/t-pipe-connection/t-pipe-22-monitors-fields.png)

## 26. Run - Time Control

Finally, we can start our computation.

Estimated computation time for single-core: 5 minutes

1. Go to *RUN* panel
2. Set the maximum *Number of Iteration* to `500`
3. Click **Run Simulation** button

![image](https://help.sim-flow.com/tutorials/images/t-pipe-connection/t-pipe-23-run.png)

## 27. Residuals

When the calculation is finished, we should see a similar residual plot. All the residual values have reached \(10^{-4}\) and the solver has automatically stopped the calculation. The residuals are the measure of how results change between iterations. Reaching a very low value indicates that we have found a steady-state solution and results do not change regardless of further computations.

1. Go to *Residuals* tab

![image](https://help.sim-flow.com/tutorials/images/t-pipe-connection/t-pipe-24-residuals.png)

## 28. Slice - Velocity Field

The *Slices* tab appears next to the *Residuals*. Under this tab, we can preview results on the defined section plane.

1. Change tab to *Slices*
2. Select the velocity *U*
3. Click *Adjust range to data*
4. Set the YZ orientation *View YZ*
5. Click *Fit View*

![image](https://help.sim-flow.com/tutorials/images/t-pipe-connection/t-pipe-25-results.png)

## 29. Start Postprocessing with ParaView

To access more advanced postprocessing functions, use the integrated ParaView software.

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

![t pipe 26 paraview](https://help.sim-flow.com/tutorials/images/t-pipe-connection/t-pipe-26-paraview.png)

## 30. ParaView - Load Results

A new ParaView window should open. Load results into ParaView. Be aware that in a steady-state simulation, SimFlow saves only the last two iterations by default. View the last one to see the final solution.

1. Click **Apply** to load results into ParaView
2. Display the results from the last frame
3. After loading results, they will be shown in the 3D graphics window

![t pipe 27 pv open](https://help.sim-flow.com/tutorials/images/t-pipe-connection/t-pipe-27-pv-open.png)

## 31. ParaView - Display Streamlines (I)

Advanced postprocessing features give us a possibility to display, e.g., streamlines. To do that, follow these steps:

1. Make sure the *pipe_flow.foam* case is selected and highlighted in blue
2. Select *Stream Tracer* from the top menu
3. Change *Seed Type* to *Point Cloud*
4. Type the center coordinate and radius of the sphere:
   *Center*`0``0``0`
   *Radius*`0.15`
5. Increase the number of points to `150`
6. Click **Apply**
7. Select the velocity *U* from the list

![t pipe 28 pv streamlines](https://help.sim-flow.com/tutorials/images/t-pipe-connection/t-pipe-28-pv-streamlines.png)

## 32. ParaView - Display Streamlines (II)

To enhance visibility, we can render the streamlines.

1. Expand the *Toggle advanced properties*
2. Scroll down to the *Styling* section and increase *Line Width* to `2`
3. Mark *Render Lines As Tubes* option

![t pipe 29 pv streamlines style](https://help.sim-flow.com/tutorials/images/t-pipe-connection/t-pipe-29-pv-streamlines-style.png)

## 33. ParaView - Display Transparent Geometry

We can additionally display the transparent geometry to observe how the streamlines are distributed in relation to it.

1. Click on the *eye* next to the *pipe_flow.foam* base case to display it
2. Select the *Solid Color* from the list
3. Set the *Opacity* to `0.3`

![t pipe 30 pv opacity](https://help.sim-flow.com/tutorials/images/t-pipe-connection/t-pipe-30-pv-opacity.png)

## 34. ParaView - Streamline Results

The final results contain the transparent geometry and streamlines colored by the velocity.

![t pipe 31 pv results](https://help.sim-flow.com/tutorials/images/t-pipe-connection/t-pipe-31-pv-results.png)

## 35. 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)