# T-pipe Connection

## 1. Create Case

After opening SimFlow, we will create a new case named t_pipe_connection

1. Go to panel

2. Provide name t_pipe_connection

3. Click

## 2. Create Geometry - Cylinder 1

We will create a T-pipe geometry by joining together two cylinders.

1. Go to Geometry panel

2. Select Create Cylinder

3. Set the cylinder dimensions:
Length $$\sf{[m]}$$0.4
Radius $$\sf{[m]}$$0.05

## 3. Create Geometry - Cylinder 2

1. Select Create Cylinder

2. Set the origin and axis:
Origin $$\sf{[m]}$$0-0.40
Axis $$\sf{[-]}$$010

3. Set the cylinder dimensions:
Length $$\sf{[m]}$$1.5
Radius $$\sf{[m]}$$0.075

## 4. Unite Geometries

We will join two geometries by using unite tool. This is a geometric boolean operation that will result in a single solid geometry.

1. Select both cylinder with CTRL key pressed

2. Click Unite Geometries

3. New geometry will be listed below the cylinders. Double click on its name and change it from unite to t_joint

## 5. Geometry - T-pipe

The resulting geometry will be displayed in the graphics window.

1. Click Fit View to zoom in the geometry

## 6. 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. 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 key to clear the selection

## 7. Creating Face Group - Inlet 2

Next, select the second inlet and create a new face group.

1. Select the second inlet. Press CTRL key and click on the face as below

2. Click on the Face Group button in the graphics context toolbar

3. Press Esc key to clear the selection

## 8. Creating Face Group - Outlet

Now, rotate the view in a way you will be able to see the second end of the geometry.

1. Select the outlet face. Press CTRL key and click on the face

2. Click on the Face Group button in the context toolbar

## 9. Rename Face Groups

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

2. Expand Geometry Faces

3. Change face groups names accordingly (double-click on a group name to start editing)
group_1 $$\rightarrow$$ inlet1
group_2 $$\rightarrow$$ inlet2
group_3 $$\rightarrow$$ outlet

## 10. Meshing Parameters - T_joint

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

1. Go to Hex Meshing panel

2. Select the t_joint component

3. Enable Mesh Geometry

4. Enable Create Boundary Layer Mesh

5. Set surface Refinement to Min 0 Max 1

## 11. Base Mesh - Domain

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

1. Go to Base tab

2. Click on to adopt box to visible geometries

3. Define the number of divisions
Division2520060

## 12. Start Meshing

Everything is now ready for meshing.

1. Switch to Mesh tab

2. Start the meshing process with button

## 13. Mesh

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

## 14. Boundaries

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

1. Define boundary types accordingly
t_joint wall
t_joint_inlet1 patch
t_joint_inlet2 patch
t_joint_outlet patch

## 15. Select Solver

We want to analyze incompressible turbulent flow. For this purpose, we will use the SIMPLE (simpleFoam) solver.

1. Go to SETUP panel

2. Select type

3. Select flow filter

4. Select SIMPLE solver

5. Click button to confirm

## 16. 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

## 17. Transport Properties - Water

As a fluid material, we will use water.

1. Go to Transport Properties panel

2. Open

3. Pick up water from the list

4. Click

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.

## 18. 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 t_joint_inlet1 boundary

3. Set the Velocity Inlet character

4. Set the inlet velocity
U Reference Value $$\sf{[m/s]}$$0.8

## 19. Boundary Conditions - Inlet 2

The second inlet will be defined using pressure inlet condition. For the pressure value, we will use 1 [kPa]. Note, 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 t_joint_inlet2

2. Set the total pressure value
$$p_0$$ $$\sf{[m2/s2]}$$1

## 20. Boundary Conditions - Outlet

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

1. Select t_joint_outlet

2. Set the Pressure Outlet character

## 21. 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, runtime post-processing can only be configured before starting calculations and can not 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 $$\sf{[-]}$$100

## 22. Monitors – Sampling (II)

Additionally, to specifying the geometry we need to choose which results should be sampled.

1. Expand Fields list

2. Select pressure p and velocity U

## 23. 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 button

## 24. 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 iteration. 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

## 25. Slice - Velocity Field

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