Skip to end of metadata
Go to start of metadata

You are viewing an old version of this page. View the current version.

Compare with Current View Page History

« Previous Version 7 Next »

Problem Specification
1. Start-up and preliminary set-up
2. Specify element type and constants
3. Specify material properties
4. Specify geometry
5. Mesh geometry
6. Specify boundary conditions
7. Solve!
8. Postprocess the results
9. Validate the results

Step 2: Specify element type and constants

Since thin structures can be modeled efficiently as shells, we'll use shell elements to build the finite-element model. Shell elements can support membrane and bending loads consistent with classical shell theory (sorry, FEA doesn't let you off from understanding basic theory). As you can imagine, shell elements are appropriate when the thickness of the structure is small compared to the other dimensions. The computational savings come about because only the mid-surface of the structure is modeled; the thickness and other cross-sectional properties are incorporated into the element stiffness matrix and input as "real constants" in ANSYS. (This is analogous to modeling beams using beam elements where the beams are modeled as lines with thickness and other cross-sectional properties being "real constants"). Section 2.10 in the ANSYS Element Reference manual gives you a page of useful information on shell elements. Be sure to peruse it in the online documentation since it'll be on the final. (wink)

Specify Element Type

Let's take a peek at the shell elements available in ANSYS. Bring up the ANSYS documentation window, select the Search tab, enter the phrase "pictorial summary" and click on List Topics. Then double-click on 3.2 Pictorial Summary in the left pane. At the top of the pictorial summary of element types in the right pane, click on SHELL Elements. This brings up the list of shell elements available in ANSYS including many with specialized capabilities. Perusing this list, you'll see thatSHELL63 (4-node elastic shell) is a basic shell element and a possible candidate for our problem. A close relative is SHELL93(8-node elastic shell) which has mid-side nodes in addition to the corner nodes. Since the mid-side nodes give greater accuracy, we'll useSHELL93 for our problem. Click on SHELL93in the help and take a few minutes to persue the manual page for this element. What are the "real constants" that we'll need to enter in the next step? Note that each node has six degrees of freedom: three translational and three rotational.
Main Menu > Preprocessor> Element Type > Add/Edit/Delete > Add...
Pick Shell in the left field and Elastic 8node 93 in the right field. Click OK to select this element. The SHELL93 element will now be available in the meshing step. Close the Element Types menu.

Specify Element Constants

Main Menu > Preprocessor> Real Constants > Add/Edit/Delete > Add
This brings up the Element Type for Real Constants menu. Click OK to specify the real constants for the SHELL93 element.
When meshing, we'll have to assign three different thickness values: H1 for the plate; W2 and W3 for the stiffeners in the x and ydirections, respectively. This means we'll have to create three real constant sets, one for each of these thickness values. According to theSHELL93 help page, if the element has a constant thickness, only TK(I), the shell thickness at the first corner node, needs to be input.
Create the first real constant set: make sure Real Constant Set No. is set to 1. For TK(I), enter H1. Leave the other fields blank since they are not applicable to our problem. Click Apply.
Create the second set: For Real Constant Set No., enter 2. For TK(I), enter {W2}} and click Apply.
Create the last set: For Real Constant Set No., enter 3. For TK(I), enter W3 and click OK.
Save: Toolbar > SAVE_DB
Go to Step 3: Specify material properties

Copyright 2006.
Cornell University
Sibley School of Mechanical and Aerospace Engineering.
ANSYS Short Course-Tutorial List

  • No labels