ANSYS Custom Beam Output

ANSYS – Custom Beam Output Rev. 11/17/05

Sample Problem

Plot the bending moment diagram for the following simple frame:

E
I
A
h
Node
1
2
3 / Beam 1
Steel
.0833 in4
1 in2
0.5 in
X
0
10
10 / Beam 2
Steel
.0833 in4
1 in2
0.5 in
Y
0
0
10 / E=30e6
n=.28
Z
0
0
0

ANSYS

Change your jobname, title, default directory.

Switch Output to jobname.out [√] Append box.

Create Beam Model

>Preprocessor

>Element Type >Add/Delete/Edit (BEAM3 - 2-D elastic)

<Options> K6 Include Output

K9 5 intermed pts

>Real Constant (define I, J, A, w, h for each size beam)

>Material Models >Structural >Linear >Elastic >Isotropic

(enter Ex, PRx)

Material Props > Material Library >Select Units (BIN)

>Modeling >Create

>Nodes >In Active CS (enter x, y, z coordinates from keyboard)

>Elements

>Element Attributes (change Real Constant or Material number

>Auto numbered> Thru Nodes (Pick 2 nodes to define each beam)

Model Check Use the [List] and [Plot] options to check model geometry and coordinates

>Solution

Analysis Type >New Analysis (default is Static)

>Define Loads

>Apply >Structural

>Displacements - On nodes (define constraints)

Pick node <Apply>

1 All DOF <OK>

>Apply

>Force/Moments - On nodes (define applied loads)

Pick node

3 FX 1000

[Save db]

>Solve - Current Load Step (submit completed problem to FEM solver)

>General Postprocessor

>Plot Results >Deformed Shape Deformed and undeformed.

[PlotCtrls] Style> Displacement Scaling> User 2.0 (change deformation amplification)

>List input data: Nodal coordinates, elements, properties, real constants, loads, constraints

>List Results: Nodal Solution, Element Solution, and Reaction Solution

Create an ETABLE (Element table)

This operation extracts information from the solution file to output in a table. Sets of data are stored in groups called "items". Each data quantity also has a name. In this case we want the bending moments in the beams, which is named MMOMZ in item SMISC. (Element Handbook)

To see the bending moments at intermediate points on each beam, you must declare this option in the preprocessor before you perform the analysis. Do this by setting KOPT switches.

>Preprocessor >Element Type

Add... (define your beam elements)

Options (set KOPT switches)

KOPT(6) =Include Output

KOPT(9) = 5 (5 intermediate points requested - max is 9)

After performing the FEM solution, use the ETABLE to view the results.

>General Postprocessor >Element Table

We use the "Numerical Sequence" method. (see 4.3 Element Handbook, pp. 4-15 to 4-24)

To call up the KOPT tables for beams:

Help - beam3 (description of beam elements)

>Define Table <Add> (add desired data to the ETABLE)

Select "By sequence number" -

Note: This is last option on the list. Scroll down to it.

Select SMISC (the data block containing MMOZ)

SMISC, 6 <Apply> (add data item number 6 to the Selection Box)

Repeat for sequence numbers 12, 18, 24, 30, 36, 42 for MMOMZ

This data will go into the ETABLE for each beam.

at Node I, plus the 5 intermediate locations and Node J.

<OK>

To view the ETABLE:

>General Postprocessor >Element Table >List Element Table <ok>

Print Table

[File] >Print (Use File option in the table window)

Send to default printer: lp -d CB230ps

Plot the moment diagram along each beam:

>General Postprocessor >Plot Results >Contour Plot >Line Element Results

SMIS6 (starting data item)

SMIS42 <OK> (ending data item)

Screen Capture

[PlotCtrls] >Hard Copy

Send to default printer: lp -d CB230ps (delete the -p option)

Other Etable data of interest for beams:

SDIR / Axial direct stress
SBYT / Bending stress +Y side of beam
SBYB / Bending stress -Y side of beam
SMAX / Max stress (direct + bending)
SMIN / Min stress (direct - bending)
MFORX / Member force in local x direction
MFORY / Member force in local y direction
MMOZ / Member moment about local z axis