CAE Project Assignment

Part 2: ANSYS Instructions

Outline

Based heavily on the ANSYS outline by Michael Paisner

Introduction
ANSYS Instruction Conventions

I. Start Ansys
II. Import the Part
III. Mesh the Part
IV. Apply Boundary Conditions
V. Apply Loads
VI. Print Image
VII. Solve
VIII. Print Image
IX. Graph Stresses for a Cross Section of the Wrench
X. Print Image
XI. Exit the Program

Introduction

Part 2 of the CAE project is to do a Finite Element Analysis of your wrench using Ansys. You must have completed Part 1 of the CAE project and exported the wrench before you can begin on this second part of the project!

[Return to Outline]

ANSYS Instruction Conventions

The following conventions are used in the Ansys Instructions:

CAPITALS	Menu Headings
Bold	Menu Choices
Italics	Enter text or a carriage return
Underlined	Mouse button to be clicked in the ANSYS GRAPHICS window

Examples:

UTILITY MENU -> File

means go to the menu labeled UTILITY MENU and select the menu choice File.

ANSYS INPUT -> aplot <CR>

means go to the ANSYS INPUT window, enter the text aplot followed by a carriage return.

When entering text, you must move the cursor over the window where the text is to be entered.

[Return to Outline]

I. Start ANSYS

You must have completed Part 1 of the CAE project and exported the wrench before you can begin on this second part of the project!

Using the same computer account which was used to draw the wrench, log in at any of the HP computers in the Mechanical Engineering cluster (except for hpme12) and open up ANSYS by going to the Xterm window and typing:

/data/ansys52/bin/xansys52 <CR>.

The XANSYS52 menu window will appear. Pick a location for this menu by clicking once with the left mouse button. Choose:

XANSYS52 -> Interactive

INTERACTIVE ->

"Memory requested (megabytes)"

"for total workspace" Type in 8

"for database" Type in 4

INTERACTIVE -> Run

The ANSYS_5.2_OUTPUT window will appear. Type a <CR> when you are prompted to in this window. The ANSYS program will now begin.

Note: The UTILITY MENU is located at the top of the screen. The MAIN MENU is located on the left side of the screen. Text should be entered in the ANSYS INPUT window at the top left corner of the screen unless noted otherwise.

[Return to Outline]

II. Import the Part

UTILITY MENU -> File

FILE -> Import

IMPORT IGES FILE -> highlight {your-iges-file}.igs

IMPORT IGES FILE -> OK

VERIFY ->Yes

Wait while the program transfers the file to the Ansys database. The part will be transferred as surface acreas.

ANSYS INPUT -> aplot <CR>

This will display the surface areas as a wireframe as shown in Figure 1.

Figure 1

ANSYS INPUT -> /prep7 <CR>

This opens the preprocessor.

ANSYS INPUT -> et,1,82 <CR>

This defines element type 82 and assigns it to reference 1. Element type 82 is the plane stress quadratic displacement 8-noded element.

[Return to Outline]

III. Mesh the Part

Meshing the part means it breaks the part into smaller pieces so that the program can analyze the stresses within the part. Breaking the part into many, small pieces (a fine mesh) will give more accurate results, but will use up more time and memory. Using fewer, larger pieces (a rough mesh) will run more quickly and use less memory, but will give less accurate results.

MAIN MENU -> Preprocessor

PREPROCESSOR -> Material Props

MATERIAL PROPS -> Isotropic

ISOTROPIC MATERIAL PROPERTIES -> OK

ISOTROPIC MATERIAL PROPERTIES -> In the box for "Young's Modulus", type 10e6.

ISOTROPIC MATERIAL PROPERTIES -> OK

PREPROCESSOR -> Mesh

MESH -> Areas

MESH AREAS -> Pick All. The part will turn light blue.

MESH AREAS -> OK

Wait for the program to mesh the part - this may take several seconds. You may get warnings at this point. If you get warnings, click OK to them. The part will now appear broken down into smaller pieces similar to Figure 3.

Figure 3

Close the MESH window.

[Return to Outline]

IV. Apply Boundary Conditions

This section tells the program what boundary conditions exist for the movement of the wrench.

PREPROCESSOR -> Loads

LOADS -> Apply

APPLY -> Displacements

DISPLACEMENTS -> On Nodes

(There are three choices labeled On Nodes. Choose the top most one).

ANSYS GRAPHICS WINDOW-> With the left mouse button, select two nodes in the wrench jaws where the jaws will contact the part to be twisted. Figure 4 shows the nodes.

Figure 4

APPLY U,ROT ON NODE ->OK

APPLY U,ROT ON NODES -> "DOFs to be constrained" highlight All DOF

APPLY U,ROT ON NODES -> "Displacement Value" type 0

APPLY U,ROT ON NODES -> OK

The figure should now look like Figure 5 with arrows marking the points which are limited to zero displacement.

Figure 5

Close DISPLACEMENT window.

[Return to Outline]

V. Apply Loads

This section tells the program what loads are being applied to the part.

APPLY -> Force/Moment

FORCE/MOMENT -> On Nodes

ANSYS GRAPHICS WINDOW-> With the left mouse button, select a node at the end of the handle as shown in Figure 6.

Figure 6

APPLY F/M ON NODES -> For "Direction of Force/Moment" choose FY

APPLY F/M ON NODES -> For "Force/Moment value" enter the load in pounds. If you chose the contact nodes such that the handle load must point down, then enter a negative load.

APPLY F/M ON NODES -> OK.

An arrow should appear on the handle as shown in Figure 7.

Figure 7

[Return to Outline]

VI. Print Image

UTILITY MENU -> PlotCtrls

PLOTCTRLS -> Capture Image

Click once with the left mouse button to set the window.

FILE -> Print

IMAGE HARD COPY -> Click next to the Print to: option to turn it on.

Click in the text field just below Print to:

Type: print -P dogweed

IMAGE HARD COPY -> OK

FILE -> Close To close the capture image window.

[Return to Outline]

VII. Solve

ANSYS INPUT -> /solu <CR>

ANSYS INPUT -> solve <CR>

Wait while the program solves the problem. After the program reaches a solution:

INFORMATION: SOLUTION IS DONE! -> Close

MAIN MENU -> General Postproc

GENERAL POSTPROC -> Plot Results

PLOT RESULTS -> Nodal Solu …

CONTOUR NODAL SOLUTION DATA -> Highlight Stress

CONTOUR NODAL SOLUTION DATA -> Highlight X-direction SX

CONTOUR NODAL SOLUTION DATA -> OK

This displays the results data as contoured stress lines across the model. You should now have a color representation of the stress of your part similar to Figure 8.