CFD homework: Analysis comparing 3 variants of fans


#1

CFD homework: Analysis comparing 3 variants of fans

Tasks 1.1 to 1.3 involve simulating the flow around 3 different variants of fan which are modelled earlier. Click the following link to copy the project to your account.

Project Link : https://www.simscale.com/projects/demo2/fan_analysis-2_variants/
Goto ‘Actions’ and ‘make a copy’.

You can also go to CAESES forum and obtain the geometry to modify it yourself:

Follow the steps below for setting up incompressible flow simulations on different fan variants.

Task 1.1

The fan geometry is already present in the project. It can be noted that there is a cylindrical box around the fan, which is important to create the cell zone for defining rotating objects. There are 2 ways of simulating the rotational motion - Multi Reference Frame (MRF) and Arbitrary Mesh Interface(AMI). More details about the types can be found here. In this tutorial we will be working with MRF approach. The first task is create a mesh, the setup for which is similar for all the 3 geometries. This can be done using the manual Hex-dominant parametric mesh of the SimScale platform, which is used to provide detailed parameters.

  • Click on the Baseline model and click Mesh geometry.

  • Select the options as shown above for the ‘Mesh operation’ - Hex-dominant parametric mesh and the number of cells in each direction.
  • Scroll down in the pane and change the ‘minVol’ option under ‘Mesh quality control’ to 1e-22. This is to ensure that smaller cells are generated near the surface of the fan. Now click the Save button at the bottom of the pane.
  • The dimensions of the base mesh box and material point should be as shown below. Enter these values and click the Save button.

  • Now we create 2 geometric primitives by clicking on Create new geometric primitives and selecting cylinders. Enter the following properties and select Save. This is used to create mesh refinements later.

  • The next step is create mesh refinements. It is done by selecting mesh refinements node in the sub-tree and selecting Add mesh refinement. The following refinements are created with the corresponding properties. Please select the Save button for each refinement.

  • The tree on the left pane should look like the following image.

  • Now click ‘Operation 1’ (or the name of the mesh, if you have renamed it) and select Start button, which starts the mesh generation process.

  • Create new mesh operations for Variant 1 and Variant 2 by following the same procedures. An easier approach for this is to ‘Duplicate’ the mesh and change the geometry domain to Variant-1 and Variant-2 respectively.

Task 1.2

The following task is to create a turbulent steady state simulation run for the above mesh. SimScale platform allows to select the ‘Analysis type’ from 5 different physical perspectives and a number of solver types are available to be selected within these broad classification, depending on the physics of the problem. The description of each physics and solver type is explained to help choose the exact conditions to be chosen.

  • The following Analysis type is selected and Save button is clicked. This generates the entire simulation setup tree.

  • In the Domain node of the sub-tree select the first variant mesh, which was created earlier.

  • Now name the faces using ‘Topological Entity Sets’ option for later usage. This is done by selecting the faces as shown below and naming them. The other 4 outer faces (apart from inlet and outlet are defined to be Walls). Fan is named by hiding the outer faces of bounding box, selecting all the faces and clicking on ‘Create entity set from selection’.

  • Select the material with following properties

  • The initial condition properties are left with the default values.
  • The boundary conditions are defined with settings as per the following table.

  • A rotation zone is defined as per shown below. As discussed a MRF type zone is used in our case.

  • The simulation controls can be used to set the properties of the process, like the time step control, the intervals at which results needs to be stored etc.

  • Result controls are defined to track the forces and moments, and also the surface data - like pressure drop etc.
  • Click on Simulation runs on the sub-tree and select Create new run.
  • Click the Start button to begin the simulation.

Task 1.3

A part of the post-processing window of SimScale is as shown in the following figures

  • Click Add filter and select Slice to slice the domain and view the flow properties along the cross section.
  • Follow the settings as shown in the image below to get the velocity contour at the final time step.

  • In the above we usually get only one instant of the solution field. If more than one is required then right click Solution field on the left pane and select Add result to viewer.

Submission

Please prepare a pdf document with the name FanAnalysis_YourLastName, containing your answers (with relevance to the following points) and mail it to Pawel Sosnowski at psosnowski@simscale.biz

  1. A plot of inlet velocity vs. pressure force/moments developed on the fan

  2. Pressure contour on the fan

  3. Velocity contour in the domain

  4. Velocity streamlines in the potential zones


#6

I do not attend the Webinar, but I like tutorials :slight_smile: I hope tha is not a problem!? :wink: Some Screenshots with paraview
v1:

v2:


#7

Great! @cbabua


#8

And now the own design!


#9

Hello,

I fail to make a velocity contour in the domain.
I have available (in the “contour by” field) p, k and omega.

Could you assist me?

I also fail to see how I should make the plot for Nr.1


#10

@maxp can you share the project link and we’ll have a look!

Best,
Anna


#11

Yes, of course.

https://www.simscale.com/projects/maxp/fan_analysis_-_2_variants/

Thank You!
Max


#12

Hi @maxp - Selecting the ‘U’ field directly for a slice filter/domain gives the result, does this answer your question? Or are you wanting to use the contour filter ?


#13

Yes, that’s what i will submit. But I wanted to use the contour filter.
alas, I dont seem to have it available.


#14

@maxp - just figured out the reason for this, so the contour filter can only be applied to scalar data and velocity is a vector field.

Here’s what you can do (*Note that this is a different project - just for demonstration purposes).

Use the calculator filter to take the magnitude of the velocity

Then with the result you can apply the contour filter


#15

Thank You, Great!

Is there a list of functions I can use with the filter?
Or are all functions I can use in paraview available? Then I can simply look through that user manual.


#16

The online post-processor is based on Kitware’s ParaViewWeb technology so using the functions as you would in a native version should work


#17

Short question… how can I see, which design is the best? :wink:


#18

In the webinar it was explained as:
It depends.
One design moves more air than the other, but the other has less moment on it per air it moves.
As soon as the vid is out you want to watch it, it is explained better at the end of the first session.


#19

@cbabua and @maxp, I’ve uploaded the recording. You’ll find it at the top of this post

Best,
Anna


#20

Thank you!