Skip to end of metadata
Go to start of metadata

Step 5: Mesh geometry

Bring up the MeshTool:

Main Menu > Preprocessor > Meshing > MeshTool

We'll first mesh the two front surfaces using MESH200. Click Set next to Global under Element Attributes. Set the TYPE to MESH200 and click OK.


 
According to the ANSYS manual, "Smart element sizing (SmartSizing) is a meshing feature that creates initial element sizes for free meshing operations. SmartSizing gives the mesher a better chance of creating reasonably shaped elements during automatic mesh generation ... The SmartSizing algorithm first computes estimated element edge lengths for all lines in the areas or volumes being meshed. The edge lengths on these lines are then refined for curvature and proximity of features in the geometry." To turn on SmartSizing, check the box next to Smart Size. Drag the slider to a size of 4 to get a finer mesh than the default.

In order to have a little more control over what mesh ANSYS creates for us, we will set the starting element size for SmartSizing rather than use the default. Smartsizing will take this starting element size and modify/vary it over the geometry to account for curvature and corners. Under Size Controls, click the Set button next to Global. Enter an element edge length of 0.12 and click OK. The specified smart size of 4 and edge length of 0.12 are the result of an iterative process. You should experiment with different settings for these parameters to study the effect of the mesh on your solution, as discussed in Step 9. The goal is to obtain a solution that doesn't change as you refine the mesh.


Select Areas to be meshed with a Quad shape using the Free mesher. Click Mesh. Pick the front face of the crank and the pedal shaft.

 
 
Click OK. You will now see:

You'll get the following warning:


 
Elements that exceed shape warning limits can lead to degraded accuracy. Here it is a minor concern since only 1 element out of 682 is causing the warning. So it is reasonable to press on.  In general, it is always a good idea to pay close attention to the warnings and understand their effect on your solution. As a veteran in these things, I can attest that ignoring warnings can come back to bite you in incovenient parts of the anatomy. Close the warning window.

In the above, we chose the front faces of the crank arm and pedal shaft as the surface meshes for sweeping. However, we have found that for other crank geometries, when meshing using the MESH200 elements, it is a good idea to choose the two back faces of the crank arm and pedal shaft that are flush with each other (i.e. the negative-z faces). This ensures that the nodes around the circumference of the circle on the two parts will match up and may prevent problems in sweeping the volume elements.


Bring up the MeshTool again. Click Set next to Global under Element Attributes. Set the TYPE to SOLID45 and click OK. We want four layers of mesh elements to span the thickness of the crank, so the desired element edge length in the sweep direction is (0.5 /4) = 0.125 in. Under Size Controls, click the Set button next to Global. Enter an element edge length of 0.125 and click OK. We will now sweep, i.e. extrude, the surface meshes created above across the corresponding volumes. Select Volumes to be meshed with a Hex shape along with the Sweep option as shown below. Make sure Auto Src/Trg is selected; this will automatically pick a source (Src) surface mesh and sweep/extrude it to a target (Trg) surface.

Click Sweep and Pick All to sweep-mesh both volumes. ANSYS will extend our previous surface meshes across the corresponding volumes.
 

ANSYS issues a warning that 5 out of 3986 elements violate shape warning limits. Since the number of "bad" elements is small, this is a minor concern and we'll press on. But keep in mind that what we'll obtain is a reasonable first-cut solution but it will not be the final word. For that, you'll have to show that the solution is independent of the mesh. Close the warning window and the Meshtool.

Save Your Work

Toolbar > SAVE_DB

Go to Step 6: Specify boundary conditions

See and rate the complete Learning Module

Go to all ANSYS Learning Modules

  • No labels