- 76 Views
- Uploaded on
- Presentation posted in: General

3.3 Element Technology

Download Policy: Content on the Website is provided to you AS IS for your information and personal use and may not be sold / licensed / shared on other websites without getting consent from its author.While downloading, if for some reason you are not able to download a presentation, the publisher may have deleted the file from their server.

- - - - - - - - - - - - - - - - - - - - - - - - - - E N D - - - - - - - - - - - - - - - - - - - - - - - - - -

Overview:

- In this chapter, we will present a brief overview to the following topics:
A. Beam Enhancements

1. Cross-Section Mesh Refinement

2. Built-Up Sections

3. Plasticity

B. Mixed U-P Formulations

C. Pressure Load Stiffness

D. 20-Noded Layered Solid

E. Initial Stress

Training Manual 001419

15 Aug 2000

3.3-1

- Cross-Section Enhancements
- Shear center, warping rigidity and shear correction factors are calculated for all sections, including user mesh
- No hard limits on section size (number of section cells)
- Cross-section mesh refinement
- Needed for accurate shear correction factors & direct shear stress calculations

- Built-up (multi-material) cross-sections
- Applications:
- sandwich beams
- airfoils
- MEMS
- reinforced beams

Training Manual 001419

15 Aug 2000

3.3-2

- Transformed section method is used for multi-material cross sections
- Sparse solver used for efficient section solution
- Extensive material library
- Orthotropic elasticity, BISO, MISO, BKIN, MKIN, KINH, NLISO, Creep, Chaboche, Rate Dependent plasticity, User material

- Initial Stresses supported for built-up beams
- assign initial stress based on the cell material number

- 3D post processing (/ESHAPE, /EFACET)
- visualization of direct shear stress

Training Manual 001419

15 Aug 2000

3.3-3

- Cross-Section Mesh Refinement
- Available for common and custom sections
- Refine with slider bar
- Refine by picking elements (EREFINE)

- Available for common and custom sections

Training Manual 001419

15 Aug 2000

3.3-4

- Built-Up Sections for BEAM188 and BEAM189
- Ability to specify a cross-section made up of different materials (EMODIF)
- Available for common and custom sections

Training Manual 001419

15 Aug 2000

3.3-5

- Plasticity for BEAM188 and BEAM189
- At revision 5.6, the treatment of material nonlinearities at the section points is based on uncoupled behavior between the stress components
- Axial and the torsional shear stress components behave independently
- As a result of this approximation, the equivalent stress output by PRSSOL may at times exceed yield stress and yet no active yielding is reported

- At revision 5.7, the actual state of stress within the beam is used to perform the plasticity calculation
- The new formulation will release the restriction on the beam elements of handling complete state of stress in plasticity and will provide more realistic state of stress in the beam elements

- At revision 5.6, the treatment of material nonlinearities at the section points is based on uncoupled behavior between the stress components

Training Manual 001419

15 Aug 2000

3.3-6

- Mixed U-P formulation option added to elements: PLANE182, PLANE183, SOLID185, SOLID186, SOLID187
- Includes hydrostatic pressure as an independent DOF

- Applications
- hyper-elastic materials (typically fully incompressible)
- elasto-plastic materials undergoing large plastic strains
- linear elastic materials with Poisson’s ratio > 0.4999

- Advantage - better convergence and more robust
- Disadvantages
- Additional DOF’s (longer solution time per equilibrium iteration)
- Does not support modal and buckling analyses

Training Manual 001419

15 Aug 2000

3.3-7

- Activation
- keyopt(6) = 0, regular formulation (default)
- keyopt(6) = 1 (or 2 for SOLID187), mixed U-P formulation
- The solver (EQSLV command) must be either the frontal solver (default) or the sparse solver - (frontal is recommended)

- Internal nodes used for pressure DOF’s
- Created automatically
- Not accessible by user

*** NOTE *** CP= 54.625 TIME= 14:28:22

Internal nodes from 2360 to 3831 are created.

1472 internal nodes are used for 18x elements with mixed formulation.

Training Manual 001419

15 Aug 2000

3.3-8

- The examples below were solved with mixed U-P formulations

Inflation of a hyperelastic membrane

Inflation and pinch flat of a bicycle tire

Training Manual 001419

15 Aug 2000

3.3-9

- Pressure load stiffness option added to elements: PLANE2, PLANE42, SOLID45, SOLID46, SOLID64, SOLID65, PLANE82, VISCO88, VISCO89, SOLID92, SOLID95, SURF153, PLANE182, PLANE183, SOLID185, SOLID186, SOLID187
- Benefits models with element pressure loads
- Improved convergence for large deflection analyses
- Improved accuracy for linear buckling analyses

- New options on existing commands:
- Pressure load stiffness controlled by a new field (Key3) on the SOLCONTROL command
- Unsymmetric stiffness matrix controlled by a new Option on the NROPT command

Training Manual 001419

15 Aug 2000

3.3-10

- SOLCONTROL, Key1, Key2, Key3
- Key3 = NOPL
- Do not include pressure load stiffness for any elements

- Key3 = no entry (default)
- Include pressure load stiffness for elements SURF153, SURF154, SHELL181, PLANE182, PLANE183, SOLID185, SOLID186, SOLID187, BEAM188, and BEAM189
- Do not include pressure load stiffness for elements PLANE2, PLANE42, SOLID45, SOLID46, SOLID64, SOLID65, PLANE82, VISCO88, VISCO89, SOLID92, SOLID95, and SOLID191

- Key3 = INCP
- Include pressure load stiffness for elements PLANE2, PLANE42, SOLID45, SOLID46, SOLID64, SOLID65, PLANE82, VISCO88, VISCO89, SOLID92, SOLID95, SURF153, SURF154, SHELL181, PLANE182, PLANE183, SOLID185, SOLID186, SOLID187 BEAM188, BEAM189, and SOLID191

- Key3 = NOPL

Training Manual 001419

15 Aug 2000

3.3-11

- NROPT, Option, --, Adptky
- Option = UNSYM
- Use full Newton-Raphson with unsymmetric matrices of elements where the unsymmetric option exists

- If an unsymmetric matrix is needed for pressure load stiffness effects, use NROPT,UNSYM
- For analyses involving friction, using NROPT,UNSYM is useful (and, in fact, sometimes required) for problems where the normal and tangential (sliding) motions are strongly coupled, such as in a wedge insertion problem
- You should first try NROPT,FULL; then try NROPT,UNSYM if you experience convergence difficulties

- Option = UNSYM

Training Manual 001419

15 Aug 2000

3.3-12

- New element: SOLID191 3D 20-Noded Layered Structural Solid
- Enhances element library for composites
- Uses SHELL91 data structure
- stable, fully integrated

- Uses SOLID95 displacement shapes
- Better accuracy for curved boundaries

- Input similar to SOLID46
- Includes stress stiffening capability
- Does not support nonlinear materials or large deflections

Training Manual 001419

15 Aug 2000

3.3-13

- Enhancements made to Initial Stress loading
- New commands
- ISTRESS
- Defines a set of initial stress values

- ISWRITE
- Determines whether an initial stress file is written (or not)

- ISTRESS
- New options
- Ability to apply initial stresses only to specified materials

- Existing command
- ISFILE
- Reads an initial stress state from a file into ANSYS
- Lists initial stresses
- Deletes initial stresses

- ISFILE

- New commands

Training Manual 001419

15 Aug 2000

3.3-14