# ANSYS Model of a Cylindrical Fused Silica Fibre by nyut545e2

VIEWS: 39 PAGES: 15

• pg 1
```									ANSYS Model of a Cylindrical
Fused Silica Fibre

Steven Zech
Embry-Riddle Aeronautical University

Dr. David Crooks and Dr. Calum Torrie
University of Glasgow
29 June 2006

1
Overview
NOTE: This Tutorial was designed for a person with some general
Knowledge of ANSYS.
 Model a Cylindrical Fused Silica Fibre using Beam
elements.
 Extract the energy in the tapered region and compare to
overall energy.
Material Properties:
 EX = 7.2E10
 PRXY = 0.17
 Density = 2202
Boundary Conditions:
 Constrained at one end.

2
Designing the Fibre
•   Enter ANSYS
•   Create 4 Keypoints [at the points: (0,0); (0,0.375); (0,0.38); (0,0.39)]
•   Main Menu > Preprocessor > Model > Create > Keypoints> On
Working Plane (This is used to create 3 lines)
•   Create 3 Lines
•   Main Menu > Preprocessor > Model > Create > Lines > Straight Lines
(pick Keypoint 1 and then keypoint 2 to create the first line, repeat for 2,3 and 3,4). The 3
Lines will be used to Create designated regions which will define a base, tapered neck and the
fibre.

•   Define Material Properties & Element Type
•    Main Menu > Preprocessor > Material Props > Material Models >
Structural
•    > Linear > Elastic > Isotropic [enter EX: 7.2e10; PRXY: 0.17]
•    > Nonlinear> Density [Density: 2202]
BEAM 189 (Beam > 3 node 189) > OK > Close

3
Designing the Fibre
•   Defining the 3 “BEAM” Sections
•    Main Menu > Preprocessor > Sections >Beam >
Common Sections
•    For ID 1 [Name: Top, Sub-Type: Circle, R: 1.5e-3,
N: 100] > Apply
•    For ID 2 [ID: 2, Name: Bottom, Sub-Type: Circle,
R: 470e-6, N: 100] > OK
•    Main Menu > Preprocessor > Sections > Taper
Sections > by XYZ Location (see Create Taper Section box below)
•    Taper section ID 3 [Name: Taper, Beg. Sec. ID: 1 Top,
XYZ Loc. Beg. Sect: 0, 0.38; End Sec. ID: 2 Bottom;
XYZ Loc. End Sect: 0, 0.375
•    > OK

4
Designing the Fibre                          (Meshing)

•   Meshing (creating the BEAM Elements)
•   Main Menu > Preprocessor > Meshing >
MeshTool (see image to the Right)
•   Element Attributes > Lines > Set
•   Pick Line 1 > Apply [SECT: 2 Bottom] > Apply
•   Pick Line 2 (may need to zoom in) > Apply [SECT: 3 Taper] >
Apply
•   Pick Line 3 > Apply [SECT: 1 Top] > OK
•   Size Controls > Global > Set        (see image below)
•   [NDIV No. of element Divisions: 10] – this sets the number of
Divisions per segment. The Beam is divided into 3 line
segments so 30 elements will be produced. > OK

5
Designing the Fibre                         (Meshing)

•   MeshTool > Mesh > Pick All
- NOTE: If the structure does not show the next command is needed

•    In the ANSYS Command Prompt Type: /ESHAPE, 1 [enter]
EPLOT [enter] – zoom in to see structure of elements if desired.

6
Structural > Displacement > On Keypoints – click fit view
•     Pick the top keypoint       (keypoint 4)   > Apply > All DOF > OK

•   Solution
•     Main Menu > Solution > Analysis
Type
•     > New Analysis > Modal > OK
•     > Analysis Options [No. of
Modes to extract: 6; NMODE: 6;
Calc. Elem Results: Check Yes]
> OK > OK
•     SAVE    (Utility Menu > File > Save OR type
SAVE in the ANSYS Command Prompt.)

7
Solving. . .
•   Main Menu > Solution > Solve > Current LS –           Begin Solution of
•   When the solution is done click [Close] and proceed to Post-Processing

8
Post-Processing
•   Finding the Energy
•   Main Menu > General PostProc > Read Results > by Pick
This will show the 6 solutions (or modes) and the frequency at which the mode exists.
•    Pick Set 1 > Read > Close
•   Main Menu > General PostProc > Element Table > Define Table >
Add [Item: Energy > SENE] > OK > Close
•   For a list of each element and its energy at the picked frequency:
•    Main Menu > General PostProc > Element Table > List Elem Table
•   For the total energy at the picked frequency:
•    Main Menu > General PostProc > Element Table > Sum of Each Item >
OK
•   To get an Energy of a Different Frequency or Mode:
•    Main Menu > General PostProc > Read Results > by Pick
•    Pick Frequency > Read > Close
•    Main Menu > General PostProc > Element Table > Define Table >
Update
•    Main Menu > General PostProc > Element Table > Sum of Each Item >
OK

9
Energy in the Tapered Neck
•   Selecting the Elements in the Neck
•   Utility Menu > Select > Entities > Lines > By Num/Pick
•   Select line 2 > OK (Raise Hidden)
•   > Elements > Attached to > Lines > Apply > Plot

10
Energy in the Tapered Neck
•   Finding the Energy
•   Repeat the process from finding the total energy only
Results will be for selected region only.
•   Selecting Everything
•   Utility Menu > Select > Everything
•   Utility Menu > Plot > Elements (or type EPLOT in the
ANSYS Command Prompt

11
Applying gravity and Using
Stress Stiffening Effects

Steven Zech
Embry-Riddle Aeronautical University

3 August 2006

12
Setting up an example model

•       Create a Pendulum using the methods from
“ANSYS Model of a Cylindrical Fused Silica
Fibre” by the same Author
•       Choose an element that has stress stiffening
effects (i.e. BEAM189) and add material
properties
•       Create keypoints, lines and Beam sections.
•       Apply mesh and all Displacement criteria in the
pre-processor (Prep7)

This was made with the Information from
Wilde FEA Ltd. and the ANSYS Product Help

13
Adding Gravity to the ANSYS Model
•   Applying Gravity
•   Main Menu > Solution (can also be applied in Preprocessor) >
Define Loads > Apply > Structural > Inertial > Gravity > Global.
•   To apply gravity (or to “Simulate Gravity”), An acceleration must be
applied in the opposite direction of gravity. Example: if gravity is in the
negative y-direction (i.e. -9.81 m/s2) then apply an ACEL Y of +9.81.
(See figure)
•   Solving using a Static Solution (Including Stress Stiffening)
•   A Static solution must be ran before the Modal solution to calculate
the Eigen values and eigenvectors to properly model Stress
stiffening as a result of gravity.
•   Main Menu > Solution >
Analysis Type > New Analysis >
Static > OK
•   Solve

14
•   Modal Solution
PostProc (to avoid error messages)
•   Main Menu > Solution >
Analysis Type
•  > New Analysis > Modal
> OK
• > Analysis Options [No.
of Modes to extract: 24;
NMODE: 24; Calc. Elem
Results: Check Yes;
PSTRES: Check Yes] >
OK > OK
•   SOLVE
•   Review the Results
The PSTRES command uses the Eigen values and Eigenvectors calculated in the Static
solution to add stress stiffening, which is needed to simulate gravity in the model.

15

```
To top