# ANSYS Model of a Cylindrical Fused Silica Fibre

## Presentation on theme: "ANSYS Model of a Cylindrical Fused Silica Fibre"— Presentation transcript:

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

Overview Material Properties: Boundary Conditions:
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.

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] Main Menu > Preprocessor > Element Type > Add/Edit/Delete > Add > BEAM 189 (Beam > 3 node 189) > OK > Close

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

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

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.

Applying the Load Main Menu > Preprocessor > Loads > Define Loads > Apply > 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.)

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

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: Pick Frequency > Read > Close Main Menu > General PostProc > Element Table > Define Table > Update

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

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

Applying gravity and Using Stress Stiffening Effects
Steven Zech Embry-Riddle Aeronautical University 3 August 2006

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

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 m/s2) then apply an ACEL Y of (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

Adding Gravity cont. . . Modal Solution
Main Menu > General 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.

Similar presentations