Presentation on theme: "ANSYS Model of a Cylindrical Fused Silica Fibre"— Presentation transcript:
1ANSYS Model of a Cylindrical Fused Silica Fibre Steven ZechEmbry-Riddle Aeronautical UniversityDr. David Crooks and Dr. Calum TorrieUniversity of Glasgow29 June 2006
2Overview 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 = 7.2E10PRXY = 0.17Density = 2202Boundary Conditions:Constrained at one end.
3Designing 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 LinesMain 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 TypeMain 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
4Designing the Fibre Defining the 3 “BEAM” Sections Main Menu > Preprocessor > Sections >Beam > Common SectionsFor ID 1 [Name: Top, Sub-Type: Circle, R: 1.5e-3, N: 100] > ApplyFor ID 2 [ID: 2, Name: Bottom, Sub-Type: Circle, R: 470e-6, N: 100] > OKMain 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
5Designing the Fibre (Meshing) Meshing (creating the BEAM Elements)Main Menu > Preprocessor > Meshing > MeshTool (see image to the Right)Element Attributes > Lines > SetPick Line 1 > Apply [SECT: 2 Bottom] > ApplyPick Line 2 (may need to zoom in) > Apply [SECT: 3 Taper] > ApplyPick Line 3 > Apply [SECT: 1 Top] > OKSize 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
6Designing the Fibre (Meshing) MeshTool > Mesh > Pick All- NOTE: If the structure does not show the next command is neededIn the ANSYS Command Prompt Type: /ESHAPE, 1 [enter] EPLOT [enter] – zoom in to see structure of elements if desired.
7Applying a Load & Solving Applying the LoadMain Menu > Preprocessor > Loads > Define Loads > Apply > Structural > Displacement > On Keypoints – click fit viewPick the top keypoint (keypoint 4) > Apply > All DOF > OKSolutionMain Menu > Solution > Analysis Type> New Analysis > Modal > OK> Analysis Options [No. of Modes to extract: 6; NMODE: 6; Calc. Elem Results: Check Yes] > OK > OKSAVE (Utility Menu > File > Save OR type SAVE in the ANSYS Command Prompt.)
8Solving. . .Main Menu > Solution > Solve > Current LS – Begin Solution of Current Load Step > OKWhen the solution is done click [Close] and proceed to Post-Processing
9Post-Processing Finding the Energy Main Menu > General PostProc > Read Results > by PickThis will show the 6 solutions (or modes) and the frequency at which the mode exists.Pick Set 1 > Read > CloseMain Menu > General PostProc > Element Table > Define Table > Add [Item: Energy > SENE] > OK > CloseFor a list of each element and its energy at the picked frequency:Main Menu > General PostProc > Element Table > List Elem TableFor the total energy at the picked frequency:Main Menu > General PostProc > Element Table > Sum of Each Item > OKTo get an Energy of a Different Frequency or Mode:Pick Frequency > Read > CloseMain Menu > General PostProc > Element Table > Define Table > Update
10Energy in the Tapered Neck Selecting the Elements in the NeckUtility Menu > Select > Entities > Lines > By Num/PickSelect line 2 > OK (Raise Hidden)> Elements > Attached to > Lines > Apply > Plot
11Energy in the Tapered Neck Finding the EnergyRepeat the process from finding the total energy only Results will be for selected region only.Selecting EverythingUtility Menu > Select > EverythingUtility Menu > Plot > Elements (or type EPLOT in the ANSYS Command Prompt
12Applying gravity and Using Stress Stiffening Effects Steven ZechEmbry-Riddle Aeronautical University3 August 2006
13Setting up an example model Create a Pendulum using the methods from “ANSYS Model of a Cylindrical Fused Silica Fibre” by the same AuthorChoose an element that has stress stiffening effects (i.e. BEAM189) and add material propertiesCreate 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
14Adding Gravity to the ANSYS Model Applying GravityMain 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 > OKSolve
15Adding 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 > OKSOLVEReview the ResultsThe 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.