Sign-up for free online course on ANSYS simulations!Step 2: Specify element type and constants
Specify Element Type
We next select the appropriate element type(s) for our problem from a large list of about 200 candidates. Consider this as equivalent to rifling through a sizable chest, picking out one or more entities and placing them on a table for later use (in step 5, in our case). To see which element types are appropriate for this problem, bring up the pictorial summary of element types: Utility menu > Help > Help Topics. Search for "pictorial summary" and double-click on the search result titled 3.2 Pictorial Summary. Click on the link to SOLID Elements. These are the element types you can use to mesh a solid volume. Check out the Solid45 element type. It is a brick-shaped element of the type referred to as "hexahedral" or "hex". It has a node at each corner and each node has three degrees of freedom: displacement in the x, y and z directions.
Click on the SOLID45 link in the pictorial summary. This takes you to the help page for this element. Read through the juicy information at the beginning of this help page. Click on SOLID45 in the statement "See SOLID45 in the Theory Reference for ANSYS and ANSYS Workbench for more details about this element" near the top of the page. Click on Equation 12-188. This shows you the shape function for the element i.e. the equation used to determine the displacement at a general point within the element from the displacement values at the 8 nodes.
We will create our volume mesh by in two steps:
- Mesh the front surfaces of the crank as well as the pedal shaft.
- Extrude these surface meshes to get the corresponding volume meshes.
This is analogous to creating a sketch and then extruding in a CAD package. Since we cannot mesh surfaces with SOLID45, we need an additional element type called MESH200. Go back to the pictorial summary of element types. Scroll to the top of the page and click on the link to MESH Elements. This takes you to the MESH200 element type.
Click on the MESH200 link in the pictorial summary to see the help page for this element. You see the following information:
"MESH200 is a "mesh-only" element, contributing nothing to the solution. This element can be used for the following types of operations:
- Multistep meshing operations, such as extrusion, that require a lower dimensionality mesh be used for the creation of a higher dimensionality mesh"
In our case, meshing the two front surfaces with MESH200 elements can be thought as going to these surfaces and marking out points and lines with a pen to show ANSYS where to put the corresponding SOLID45 nodes and elements. The SOLID45 nodes and elements are actually placed at these pre-marked locations in the extrusion step. Referring to Figure 200.1 in the MESH200 help page, we see that this element type comes in 12 different flavors. For our purposes, we will be using the 3-D quadrilateral with 4 nodes option since this correponds to the intersection of SOLID45 with a suitably aligned surface. Note that this option is selected by setting KEYOPT(1) = 6.
Minimize the ANSYS Help window. Select
Main Menu > Preprocessor> Element Type > Add/Edit/Delete > Add...
Pick Structural Mass Solid in the left field and Brick 8node 45 in the right field. Click Apply to select this element.
Pick Not Solved in the left field and Mesh Facet 200 in the right field. Click OK to select this element.
The Element Types window should list two types of elements: MESH200 and SOLID45.
In order to set the 3-D quadrilateral with 4 nodes option for MESH200, select QUAD 4-NODE next to Element shape and # of nodes K1. Click OK.
Let's take a look at the online help pages to learn about the properties of these elements.
Click Help in the Element Types window. Select the Search tab, type in pictorial summary as the keyword and click List Topics. You should see Pictorial Summary as one of the topics listed; double-click on this. This brings up the Pictorial Summary of Element Types help page. Scroll down to SOLID45 under SOLID Elements. This brick element is defined by 8 nodes with 3 displacement degrees of freedom.
Return to the Pictorial Summary page and scroll down to MESH200 under MESH Elements. Click on the MESH200 link to view a description of this meshing element. We will use this element to create a 2-D mesh from which we will create an extrusion to define the mesh for the entire crank volume (analogous to creating a sketch and extrude in SolidWorks).
Note that the MESH200 element does not contribute to the solution. We could have simply meshed the entire volume with SOLID45 elements. However, the advantage to first meshing an area with MESH200 is that it provides greater control over element sizes (this will become apparent in the meshing step).
Close the Element Types menu.
Specify Element Constants
There are no real constants for our configuration.
Save your work
Toolbar > SAVE_DB
Go to Step 3: Specify material properties