Skip to main content
All CollectionsTutorialsPiper Cherokee
Piper Cherokee - Upload CAD
Piper Cherokee - Upload CAD

Upload a CAD file that includes a far-field surface and generate a mesh.

Updated yesterday
CAD File

With your new project open, you'll see a dialog box asking you to upload a file:

  1. Download the CAD file to your computer by clicking the above link.

  2. Upload the file to your project. There are two ways to do this:

    1. Drag the file directly from your computer onto this box. This will open the File Upload window with this file preselected.

    2. Click the Upload File... button and from the File Upload window clicking the Browse button to search for the file on your computer.

  3. Click the Import button to upload it.

  4. You'll be taken to the Geometry tab. Since this CAD model doesn't require any modification, click Load to Setup on the right side of the screen:
    ​

Once you click "Load to Setup" you will be brought to the Setup tab, where you can edit the surface/group names as well as setup simulation settings (mesh sizing, boundary conditions, initial conditions, etc). During this process the geometry will be checked for quality, which may take a few minutes to complete.

Rename the Surface Groups

Following successful import, you'll see a round sphere in the 3D Viewer. This is the far field. On the left, you'll see the different objects that were imported in the Geometry panel. In the Surfaces subsection you'll see a surface group labeled "1" that contains "Shell 1 of Volume 1" and "Shell 2 of Volume 1". Expand these groups to see the different surfaces contained within them.

Rename these surface groups so you know which is which:

  1. Right-click on "Shell 1 of Volume 1" and select Rename. Name this "Far Field".

  2. Right-click on "Shell 2 of Volume 1" and select Rename. Name this "Airplane".

Now, click the eye to the right of the Far Field surface group. This will turn off visibility for those surfaces.

Click Zoom to Fit in the toolbar at the bottom of the 3D Viewer to zoom in to the remaining Airplane surfaces.

A few other useful 3D Viewer controls to experiment with include:

  • Click and drag with your mouse. This will rotate the model.

  • Hold down the Control button and click and drag with your mouse. This will translate the model.

  • Scroll upwards and downwards with your mouse scroll button. This will zoom in and out.

Define the Body Frame

Before moving on to the next stage of this project, define the Body Frame for this simulation. This information is critical if you want to define flow conditions using angles of attack or calculate output quantities such as lift or drag (i.e., for all of these you need to know which directions constitute forwards, upwards, etc.).

To define the Body Frame:

  1. Click on the Frames & Motion section header in the control panel.

  2. Click the + icon to the right.

  3. Select Body Frame.

  4. Ensure Origin is set to 0, 0, 0, pointing from the center of the airplane out through its starboard wing.)

  5. Ensure Orientation is set to 0, 180, 0, pointing from the center of the airplane out through its nose.

With the geometry imported, you can generate a computational mesh.

Generate Mesh

Before running a simulation, generate a computational mesh based on the geometry in the project. You'll do this within the Mesh section of the control panel.

First set up the parameters that are used to generate the mesh. In a real meshing situation, you'll want to iterate this process, starting with a coarser mesh and refining it as needed.

We recommend starting coarser and refining because this will require fewer computational resources in total. In this project, you'll generate a fine mesh and use a Clip to analyze it.

Set Mesh Parameters

To set up the mesh parameters for your mesh:

  1. Click on the Mesh section in the control panel.

  2. Select New Manual Mesh from the properties panel.

  3. From the Sizing Strategy dropdown, select Target Count.

  4. Enter 20 in the box (20 million CVs).

  5. Scroll down to the Mesh Size subsection and click Edit to set the parameters for the mesh within the volume:

    1. Min Size: 0.005

    2. Max Size: 50

    3. Applies to: All Volumes

  6. Click on the Model subsection in the control panel to set the parameters for surface mesh on the airplane:

    1. Curvature: 4°

    2. Max Size: 0.05

    3. Applies to: Selected Surfaces, then click inside the box to add the Airplane surface group. Select the Airplane surface group by clicking on it in the 3D Viewer or in the Geometry panel.

  7. Click on the Boundary Layer subsection in the control panel above to set the parameters for the boundary layer on the airplane:

    1. Number of Layers: 20

    2. Initial Size: 0.00001

    3. Growth Rate: 1.2

    4. Applies to: Selected Surfaces, then click inside the box to add the Airplane surface group. Select the Airplane surface group by clicking on it in the 3D Viewer or in the Geometry panel.

  8. Click on the Mesh section in the control panel and scroll to the Optional section. Check the box to enable Auto Refinement.

  9. At the bottom of the properties panel click Generate Mesh.

When the mesh has been generated, in the properties panel, you should see that the mesh has around 19M control volumes.

Note: This process does not always create exactly the same number of control volumes.

At the top left of the 3D Viewer, the first dropdown menu allows you to toggle between viewing the Geometry and Mesh. The dropdown menu to the right allows you to select the appearance geometry or mesh entities. With Mesh selected and the Far Field surface hidden, choose Surface With Edges to view the surface mesh on the airplane.

Analyze the Mesh

Create clips through the volume to get a better view of the mesh. One of these will cut vertically through the centerline of the plane and the other vertically from wingtip to wingtip.

To create a clip through the centerline:

  1. On the right of the Visualization toolbar above the 3D Viewer, click the Clip tool.

  2. In the properties panel, set:

    1. Representation: Surface With Edges. This will make seeing the cells on the clips surface a little easier.

    2. Clip Type: Plane

    3. Origin: 0, 0, 0

    4. Normal: 0, 1, 0 (or click Y)

  3. Click the check button to create the clip.

To create a clip from wingtip to wingtip:

  1. Ensure the previous clip is not selected in the control panel. To check this, click on the Visualizations section. If the previous clip was selected, the clips will be layered on top of each other.

  2. Follow the same method as before, but with the Origin set to 3, 0, 0 and Normal set to 1, 0, 0.

Viewed from the +X direction you'll see a fine mesh with a small boundary layer.

Next Steps

With the mesh generated, now set up a basic simulation. Choose between the following:

  • Manually set up the simulation

  • Upload a settings file to quickly configure the simulation

Use the buttons below to choose:

Set Up Basic Simulation
Upload Basic Simulation Settings

Related Articles
Upload CAD
CAD Model Best Practices
Did this answer your question?