User Guide: Fluid flow simulation through a centrifugal pump
This user guide demonstrates how to use SimScale to simulate (incompressible) fluid flow through a centrifugal pump. The complexity of this use case results from the requirement of modeling a rotating region. Rotating regions require additional preparation steps for both the meshing and simulation setup which we will cover in the context of this tutorial.
As a first step, import the tutorial project into the SimScale workbench.
By importing the tutorial project, a new project will be created for you, and the ‘Workbench’ will open with the prepared tutorial geometry already loaded into the viewer.
Before starting work on a fluid flow analysis with rotation, we need to make sure to prepare the CAD model to be compatible with this kind of analysis.
Take a look at the provided CAD model. It contains two regions (Change the render mode of the viewer to see the Rotating region body that is contained in inside of the flow region):
Flow domain This part represents the fluid region within our model. Essentially the volume that the fluid passing through the pump occupies. In most cases your original model will not contain the flow region, but the external walls of your pump. In such a case you can extract the flow region with the built in flow volume extraction tool.
Rotating region The second body in your model is just a simple cylinder, which needs to be defined as a CAD part in order to define the rotating region in your fluid domain.
Besides those two basic requirements, there are some more recommendation when it comes to the preparation of the CAD model:
Ensure that the imported geometry consists of Solid parts and not sheet/surface elements.
Remove any small fillets or faces which are insignificant for the analysis.
After making sure that the geometry is prepared for simulation, we can start to set up a simulation.
To create a new simulation, click on the “+” button next to ‘Simulations’ in the tree or the “Create Simulation” button on the geometry panel.
Select the “Incompressible” analysis type and click “Create Simulation“.
Left click on the mesh icon to create a new mesh.
Choose the Hex-Dominant (only CFD) Algorithm.
Change the meshing mode to Material point
Keep the sizing option as Automatic sizing and the Fineness as Coarse
Specify the number of processors to 16
Background Mesh Box
An important parameter is the size of the background mesh box. As this is a internal mesh the size of the background mesh box can be the the default.
Expand geometry primitives under Mesh to view the the coordinates of Background base mesh box
Material point: This is the parameter the algorithm uses to determine wether the mesh is created inside a shape or outside. In this case this point therefore lies within the pump but outside the impeller surface
Select the Material Point and give the coordinates as below:
A region refinement is used to refine the mesh within a volume.
The cylinder around the propeller will define a zone within the cells will be more refined than in the rest of the mesh.
Click on the ‘+’ icon next to Refinements and add an region refinement.
Select the Refinement mode as ‘inside’ and the Length of refinement as ‘0.001’.
Select the rotating region for region refinement as shown below:
In order to have a finer mesh over the surface of the body, we add surface refinement.
Click on Refinements to add a new refinement and select surface refinement. We use 2 surface refinements:
On the rotor to refine the cells near the blades and
On the cylinder to define the rotating zone.
Refinement for Blade surfaces
This refinement enforces that the cells near the propeller surface will get refined.
Select the impeller surfaces and define the minimum and maximum length as 0.001.
Refinement for the rotating (MRF/AMI) zone:
This step is crucial to correctly define the cell zone which will rotate.
Add a surface refinement and set the ‘Cell Zone’ option to ‘With Cell Zone’
Keep the minimum and maximum levels at 0.001.
Select the rotating region for the refinement
Boundary Layer Refinement
Layer refinements are used to create boundary layers near solid walls.
When considering turbulent effects, boundary layer refinement is required in order to obtain a correct solution.
Create a new layer refinement and assign all faces of the propeller and the pipe outer surfaces
This can be done by hiding the rotating region and using active box selection to select all the surfaces and deselect the inlet and outlet surfaces
Select the Inflate Boundary layer setting and the below values.
Once the mesh is fully set up, the mesh generation can be started.
The mesh generated is shown below:
After the mesh is generated, use the mesh as the domain for simulation and click on reset the assignments when prompted.
Click on generate mesh clip to inspect the internal mesh. Adjust the settings of the normal. Click on generate mesh clip icon.
Assign the standard air material to the fluid domain as shown below:
Default values for initial condition parameters are usually enough. If these parameters estimated correctly, the solution will converge faster.
We have to assign three boundary conditions.
The pump inlet needs to be assigned an inlet velocity boundary condition and the inlet velocity is as given below:
The outlet of the pump needs to be assigned a pressure outlet boundary condition.
Click on the ‘+’ icon next to rotating zones under Advanced concepts
Define the MRF rotating zone and select the rotating region as shown below:
The default settings are usually suitable. We only change the solver from PBiCG to smooth solver for all the variables for smoother convergence.
The Simulation Control settings define the general controls over the simulation. The following controls should be applied:
It is important to monitor the convergence of pressure values on the inlet and outlet faces.
We monitor the surface average data on the inlet and outlet faces
The settings are shown below:
Click on the ‘+’ icon next to simulation run and start the simulation
Check on the convergence of our field variables by clicking on the convergence plot icon under settings
Check to see if the value of pressure on the inlet surface is converged. The value at the outlet surface stays at zero.
Click on solution fields icon under the convergence plot icon to open the post processor. Click on results and select pressure to view the pressure field on the entire domain.
It is clearly seen that the inlet pressure is negative implying that the impeller is imparting a pressure head to the fluid.
Select the cutting plane in the x direction and select the scalar and vector as velocity to see the velocity contours and vectors
The rotating region clearly shows the rotating fluid inside it.
We can view the path tracked by the fluid particles by clicking on the ‘+’ icon next to particle traces and selecting the outlet face for seeding as shown below:
Click on velocity to map the scalar and to compute the vector
Last updated: November 19th, 2019
Did you find this article helpful?
How can we do better?
We appreciate and value your feedback.