Modeling Realistic Fans with Ansys Icepak
Welcome to an Ozen Engineering video. In this video, we will focus on ANSYS Icepak and specifically on how to model fans. Icepak offers a straightforward method to model 3D fans using the available fan object. However, this object can sometimes exhibit behavior that differs slightly from a real fan due to flow features like swirl and centrifugal spread caused by the spinning of the fan rotor.
Using CAD Models and MRF Approach
If you have a CAD model of the fan and blades, it may be beneficial to resolve the fan and blade details using a Moving Reference Frame (MRF) approach in ANSYS Icepak. For this purpose, I've imported a CAD model of a fan. The model includes:
- The pink line representing the casing of the fan.
- The red lines indicating the hub and blades of the fan.
- The blue cutout region behind, which transitions from the fan volume to the enclosure volume.
Defining the MRF Domain
To implement an MRF approach, we need to define a fluid volume. Currently, there is no fluid volume around the blades, so we will create one by producing a block around the fan.
- Double-click on the block and name it MRF1.
- Set its geometry to a cylinder and work on the YZ plane.
- Input the center location and dimensions (20 mm high with a radius of 34 mm).
- Assign a rotation of 6000 RPM to the block and change it to fluid.
Replicating the MRF Domain
To replicate the MRF domain for a second fan:
- Copy the MRF1 block and translate it in the Z direction by -74 mm.
- Rename the new block to MRF2.
- Adjust the meshing priority to ensure the fan objects have higher priority.
Meshing the Model
Next, we proceed to meshing:
- Click the mesh button and set maximum element sizes for efficient meshing.
- Mesh the assemblies separately and use uniform mesh parameters for the fan mesh.
- Turn solids into hollow objects to save on meshing.
High-Quality Meshing for Fan Regions
For careful high-quality meshing of fan regions:
- Double-click on the assembly and go under meshing.
- Set slack settings appropriate for the geometry and avoid global mesh control settings.
- Enable multi-level meshing to capture fine details without excessive cells.
- Edit levels for component-specific multi-level meshing.
Setting Up the Model
With the mesh ready, we set up the model:
- Define basic parameters such as solving for flow temperature and using the realizable two-equation turbulence model.
- Set numerical solution settings, including iterations and convergence criteria.
- Add monitor points near the fan to ensure solution convergence.
Running the Solution
Execute the model by starting the solution. Once available, examine the temperature field and flow speed:
- View contours of temperature and identify heat-generating components.
- Use cut planes to analyze flow speed and distribution.
Comparing MRF and 3D Fan Models
To compare the detailed MRF approach with the simplified 3D fan model:
- Deactivate the MRF model and activate the 3D fan model.
- Submit the run with adjusted convergence criteria and analyze the results.
- Observe differences in flow distribution, particularly near the fan area.
In conclusion, using CAD models with the MRF approach in Icepak and other CFD models is recommended for more accurate fan modeling. Thank you for watching. Have a good day!
Hello, welcome to an Ozen Engineering video. In this video, I'm going to be talking about ANSYS Icepak and focusing on how to model fans. In Icepak, there's a fairly easy way to model 3D fans using the available fan object.
However, the object sometimes produces behavior that is slightly different than a real fan due to flow features like swirl and centrifugal spread.
If you have a CAD model of the fan and the blades, it may be better to resolve the fan and the blade details and use a moving reference frame, MRF approach in ANSYS Icepak. For this purpose, I've brought a model of a fan. I've brought in a CAD model where we have the nice model of our fan.
The pink line is the casing for our fan. The red lines indicate the hub and the blades of our fan. And then in blue behind, we have that cutout region which is a transition from the fan volume to the enclosure volume. To do an MRF type approach, we need to define a fluid volume around the blades.
I'm going to produce a block around our fan. I'm going to name it MRF 1. Its geometry will be a cylinder, and we'll work on the YZ plane. Our center will be at this location. The block will be 20 millimeters high with a radius of 34 millimeters.
We'll assign this block a rotation of 6000 RPM and change it to fluid. Now we have our MRF domain for one of the fans, and we want to replicate it for the second one. We can easily do this by copying and translating it in the Z direction. We're going to translate it -74 millimeters.
Now we have a nice fluid volume around our geometry. We're going to name this MRF2 and move these over here so that they have lower meshing priority. We have multiple assemblies within our domain where some heat is generated.
We have our fans and the two grills or openings in the min and max X directions to pull the flow through. The next step is meshing. We're going to set maximum element size for a quick and efficient mesh. We want to mesh the assemblies separately and use set uniform mesh parameters.
We have our fan objects, which are solids. Instead of resolving the solids, we can turn them to hollow to save on meshing. We need to do careful high-quality meshing for our fan regions. We're going to double click on our assembly and go under meshing.
We want to mesh this zone separately and set our own maximum element sizes and gaps. We want to use multi-level settings to capture fine details without adding lots of cells. We're going to turn on allow multi-level meshing and keep the proximity and curvature size functions on.
We're going to change some maximum levels for the blade surface. We want to do three layers of meshing for the blade surface. Now we're done with setting up the mesh. We're going to hit generate, and it's going to start meshing. We want to examine the mesh after about a minute.
Our window came back, and it says the number of elements is around 383,000, which seems reasonable. We can look at our mesh and see that we're properly resolving the geometry. We can also look at a section and see the detailed mesh in the fan region and the rest of the enclosure.
Now that the mesh is ready, we essentially want to go and set up our model. We want to solve for flow temperature, use the realizable two-equation turbulence model, and set the natural convection option. We're going to do some basic settings for numerical solution and hit accept.
Before submitting any job, it's always best to put some monitor points. We want to make sure the solution is converged. We're going to execute our model and look at the temperature field for example.
We can see the heat-generating components and temperatures as high as 59 degrees C where the heat is generated the most. Another way to look at the solutions is to add a cut plane and look at flow speed. We can see that there's a fast flow region there.
We can switch to the 3D fan object, turn off our MRF approach, and compare the results. The flow distribution is fairly different particularly near the fan area.
This suggests that whenever possible, we should be using CAD models along with the moving reference frame approach with Icepak as well as other CFD models. Thanks for your patience. Have a good day. Bye.
