NOTE: This tutorial was updated on 10/2016 to match the updated version of the platform
Submitting all three homework assignments will qualify you for a free Professional Training (value of 500€), a certificate of participation and will give you a chance to win a fully-working prototype of a 3D printer with your design modifications.
Homework 3 - Deadline 16.03 12:00pm
A heated bed can help to improve the quality of your print and avoid critical issues like wrapping. Your task is to simulate the heat distribution around the bed by using CFD simulations. Please create four simulation runs with different heat bed temperatures (393k, 420k, 440k, 460k).
First of all, you have to import the geometry into your SimScale workspace. For this, you only have to click on this link. Please note that this can take several minutes.
Now, click on the Meshes item in the project tree. This will open an additional column in the middle.
Next click the New Mesh button to generate a new mesh.
This will open a new middle menu where you can specify the mesh operation you want to use to create the mesh.
Select Hex-dominant parametric from the list. In the same panel under Bounding Box Discretization specify the following values for number of cells in each X,Y and Z directions for the BaseMeshBox
- Number of cells in x direction: 20
- Number of cells in y direction: 20
- Number of cells in y direction: 10
- and under ‘Parallel Processing’, the number of processors as : 8
Now, click on on Save button to save the settings.
After saving , sub-trees named Geometry Primitives and Mesh Refinements will automatically appear under the default project tree
Under Geometry Primitives, click on BaseMeshBox and specify the following values as and click on Save.
- Min. Point (x): -1
- Min. Point (y): -1
- Min. Point (z): -0.08
- Max. Point (x): 1
- Max. Point (y): 1
- Max. Point (z): 0.92
Next, click on Material point and specify the following values:
- Center (x) : 0.9
- Center (y) : 0
- Center (z) : 0.1
This will place the material point in the space between the Bounding BaseMeshBox and the geometry surfaces. So, this is the confined space that will be meshed.
Now, we add the necessary surface refinements for the mesh.
Click on Mesh refinements item in the tree and on New in the middle column to create a new refinement item and adapt the following settings:
- Name: Extruder_Refinement
- Type: Surface refinement
- Level min: 7
- Level max: 7
- Finally, assign it to solid_0 and Save.
Next we will create an additional surface refinement item with the following settings:
- Name: Bed_Refinement
- Type: Surface refinement
- Level min: 6
- Level max: 6
- Finally, assign it to solid_1 and Save.
Once done, start the meshing process by clicking on the Start button at top. The meshing process will take less than 20 minutes to finish.
Mesh after computation:
Clip plane through the mesh:
Click on the Simulation Designer tab and then on New button to create a simulation run. This will open an additional column in the middle. Here you can select the type of simulation you want to run.
In our case we will run a Fluid dynamics simulation of Natural convective heat transfer.
Now you can define some additional settings. First of all choose Laminar as the turbulence model, since we are not expecting any turbulence. Then choose Steady-State from the drop down field below. This means that we will simulate the stationary flow field.
Also, turn off the Boussinesq approximation. This is usually turned off for cases where there is a significant temperature difference in the domain. Finally, save your settings by clicking the related button at the bottom, which will create additional items in the project tree on the left side.
Going forward, this tree will guide us through all necessary steps. Please note that some of the items are optional.
Next you have to specify which mesh you want to use for your simulation. Click on Domain item in the project tree and select Heat Bed mesh from the menu which disappears in the middle column. Don’t forget to save your selection.
Since this analysis involves natural convection, gravity plays a very important role in driving the flow. Hence the next step is to define the magnitude and direction of gravitational force. Go to Model and then specify the following parameters:
- x value [m/s2]: 0
- y value [m/s2]: 0
- z value [m/s2]: -9.81
Finally save the settings by clicking on the related button.
Now we have to specify the material properties of the fluid by defining the kinematic viscosity. Therefore click on the Materials sub-item in the project tree.
Click on the New button.
This will open a new middle column windows where you can assign fluids to your mesh. SimScale also comes with a material library which we will use. Click on the Import from material library button.
Here choose Air from the list on the left side and Save your selection.
Finally, we have to assign which parts of the mesh should be from this material. Please assign the material model to your mesh (region0) and Save.
Please skip Initial Conditions since they don’t need to be modified
Now you can specify the Boundary Conditions for all faces of the mesh.
Click on the Boundary Condition item in the project tree which will again open a new column in the middle of the windows. Here you can see an overview of all boundary conditions which are applied to your mesh. To add a new Boundary Condition, please click on the New button at the bottom of the middle column.
This will add a sub-item to the project list and open again a new window where you can define the boundary condition. Here you can define a name for the boundary condition, choose the type and assign it to face by using the list below.
It is also possible and recommended to select the faces which you want to assign to the boundary condition graphically. Therefore you have to select the faces in the 3D model window on the left side by clicking on them with the left mouse button; to add them to the list, just click on the Add selection from Viewer button in the middle column.
Since the full mesh domain is displayed, it is necessary to hide these faces in order to be able to select the inner faces. For this, just select the faces you want to hide and click on the Hide Selection button from the drop down menu on top of the 3D model windows. Note that you can unselect faces by re-clicking on them.
Please create the following boundary conditions:
- Name: Hot Bed
- Type: Wall
- Velocity: No-slip
Temperature: Fixed Value
- Temperature value [K]: 393
- Topological Mapping: solid_1_solid_1_face_5
- Name: Inlet
- Type: Custom
- Velocity: Pressure-inlet-outlet velocity
Pressure: Total pressure
- Total pressure [Pa]: 101325
- Gamma [-]: 1.4
- Inlet value [k]: 293
- Topological Mapping: boundingBox5, boundingBox6
- Name: Slip Walls
- Type: Wall
- Velocity: Slip
- Temperature: Set gradient to zero
- Topological Mapping: boundingBox1, boundingBox2, boundingBox3, boundingBox4
- Name: Walls
- Type: Wall
- Velocity: No-slip
- Temperature: Fixed Value
- Temperature value [K]: 293
- Topological Mapping: All faces except solid_1_solid_1_face_5 and the boundingBox faces. Here we recommend using graphical selection with the invert selection function.
Now we have to modify some of the numerical settings. This is not absolutely necessary but it will help to reduce the simulation time and make it more stable. Click on the Numerics items in the tree and change the settings and values according to the image below (Please note that you may have scroll down).
Click on the Simulation Control item in the project tree to specify how fast and accurate you want the simulation to be computed.
Choose 0 as the Start time value and 500 as the End time value. The time step length must be 1 and the write interval 500. Finally, choose 8 computing cores from the drop down menu.
To start the simulation, click on the Simulation Run item in the tree and click on the New button at the bottom of the middle column menu. This will create a snapshot of your simulation settings as a new sub-item.
Once your simulation is finished you can take a look inside the temperature and velocity distribution by using the Slice filter in the integrated post processing environment
The results shown above is obtained using a coarser mesh, so temperature and velocity fields appear to be diffused in the domain. By refining the mesh you can get much better results as shown in the figure below.