SlideShare a Scribd company logo
1 of 5
Download to read offline
TIPS
   鲁班人   (http://www.lubanren.com/weblog/)




                                                                                                www.ansys.belcan.com


Picking an Element Type For Structural Analysis:                                                   by Paul Dufour

Picking an element type from the large library of elements in ANSYS can be an intimidating thing for a
beginner. Out of the almost 200 available which one should I select? Why are there so many? Are there
181 kinds of shell elements? This article will address this issue for a structural analysis. The table below
shows the most commonly used element types for stress analysis.

    Element
                        2D Solid                     3D Solid                   3D Shell           Line Elements
     Order

                          PLANE42                     SOLID45                        SHELL63           BEAM3/44
     Linear
                          PLANE182                    SOLID185                       SHELL181          BEAM188


                        PLANE82/183                   SOLID95/186                    SHELL93            BEAM189
   Quadratic
                        PLANE2                        SOLID92/187


Element Naming Conventions:

Elements are organized into groups of similar characteristics. These group names make up the first part of
the element name (PLANE, SOLID, SHELL,etc). The second part of the element name is a number that is
more or less (but not exactly) chronological. As elements have been created over the past 30 years the
element numbers have simply been incremented. The earliest and simplest elements have the lowest
numbers (LINK1, BEAM3, etc), the more recently developed ones have higher numbers. The “18x, 20x,
and 22x” series of elements (SHELL181, SOLID187, etc) are the newest and most modern in the ANSYS
element library.

Some FEA codes (NASTRAN comes to mind) have just a handful of elements that do everything. There are
several reasons why there are such a large number of elements in ANSYS. First, there was a conscious plan
from the beginnings of the program that, for example, if you want to do a thermal analysis, there is no reason
to use an element with structural degrees of freedom. That just requires an element to carry a bunch of
baggage around that it is not using. While ANSYS does have coupled field elements that can do both,
generally speaking if you want to do a thermal analysis you use an element with a temperature degree of
freedom only, and structural elements do not drag around an unused temperature degree of freedom. This
was done in the name of computational efficiency. Secondly, old elements are rarely deleted out of the
program library for the sake of compatibility with older models. When a new and improved BEAM4
element was created, BEAM4 was not revised but left alone, and the BEAM44 was introduced. So the
library keeps getting larger as new and more capable elements are formulated. The last reason is that
ANSYS is a huge program with integrated capabilities in many physics fields. So there are elements for
fluids, electromagnetics, electric field, acoustics, and explicit dynamics analyses as well.




                                    Copyright 2003 Belcan Engineering Group, Inc.                                 1
鲁班人   (http://www.lubanren.com/weblog/)


Element Order:

Element order refers to the interpolation of an element’s nodal results to the interior of the element. This
determines how results can vary across an element, and is important if you have high gradients of strain. A
beam or plate in bending is a good example of this phenomenon, where the strain is changing sign over a
potentially very small distance. Element order can be linear or quadratic.

Linear elements do not have midside nodes. In general the strain can only vary linearly from one node to
another. This is complicated in ANSYS with many “linear” elements having so called “extra shapes” or
being “fully integrated”. This makes the elements behave more like a quadratic element, but not completely
so. Naturally a linear element is computationally faster than a quadratic element.

Quadratic elements have midside nodes. The shape function for strains varies in some nonlinear fashion
between the corner nodes. Whereas linear elements are flat on both the sides and in-plane, a quadratic
element can follow a curvature in both directions and is more accurate for a given number of nodes in the
model. For example, in a tube with a hole, the curvature is maintained around the edges of the hole as well
as on the curved edge of the panel; it is not a faceted representation as illustrated below.




   SHELL93 Quadratic Elements (8 nodes)                   SHELL181 Linear Elements (4 nodes)

Some considerations in picking an element order:

   •   For in-plane bending type problems, quadratic elements are much better than linear elements. Even
       several linear elements with “extra shapes” or “full integration” turned on are not as good one
       quadratic element.


                                                                                        σ theo = 4318 psi
                                                                                                 1
                                                                                        % error < %
                                                                                                 2




                                    Copyright 2003 Belcan Engineering Group, Inc.                             2
鲁班人   (http://www.lubanren.com/weblog/)


   •   Linear elements are more sensitive to non-perfect element shapes (i.e., have more error). A linear
       element is probably better in a mapped mesh than a free mesh.

   •   For out-of-plane, plate type bending, there isn’t much difference between linear and quadratic
       elements.

   •   Linear bricks give good results due to the “extra shapes” (full integration) if the elements are
       regularly shaped. If the volume has a shape complex enough to make skewed elements, mesh it with
       20 node bricks or tetrahedral elements. An important side note here…linear triangles and tets give
       poor results since they are actually constant-strain elements (one value of strain calculated for the
       whole element. No gradient at all. These elements are no longer even available in ANSYS except as
       degenerate elements.).

   •   As a general rule of thumb, one quadratic element containing three nodes should be more accurate
       than two linear elements having a total of three nodes across the same dimension.

   •   In nonlinear analysis, a finer mesh of linear elements is computationally more efficient, robust, stable
       and more accurate than a coarser quadratic mesh with a comparable number of nodes.

Make very simple models and experiment! Lame “advice”, I know…but it will never fail you!


2D Solid Elements:

How can a 2D element be a “solid”? That’s a question most new ANSYS users ask. There are two reasons
in ANSYS-speak. First, they are considered solid because they are not a shell or a beam element. Shells and
beams are structural abstractions that will be discussed in the following sections. Secondly, they are solids
because they fully represent a solid chunky part by modeling a cross section of that part. There are three
main kinds of 2D solid elements:

Plane Strain: In a plane strain analysis we are modeling something
that is so long that there is no strain in the thickness direction. A
cross section of a long beam or a dam holding back water would be
examples of this kind of behavior. Stresses in the thickness
direction are significant.

Axisymmetric: In this type of analysis we are modeling a cross section of a structure that is fully defined by
rotating the cross section around a central axis. A pressure vessel or bottle would be examples of this kind of
structure. The thickness direction here represents the circumferential (hoop) direction and those out-of-plane
stresses are very significant (picture a tank under pressure).

Plane Stress: This is not really a “solid” element per say but still falls into this category (since it doesn’t
really fit anywhere else). A plane stress analysis is a 2D model of a thin sheet with a small thickness and in-
plane loading. You would get the same results with a shell model with in-plane loads only and the out-of-
plane displacement constrained.


All 2D solid elements can be any one of these three types by changing the element key options.



                                    Copyright 2003 Belcan Engineering Group, Inc.                            3
鲁班人   (http://www.lubanren.com/weblog/)


PLANE42: Basic 2D solid element.

PLANE82: 8 noded version of PLANE42. Also has a triangular option.

PLANE182: Similar to PLANE42 except has capability for simulating deformations of nearly
incompressible elastoplastic materials, and fully incompressible hyperelastic materials.

PLANE183: 8 noded version of PLANE182.


3D Solid Elements:

These types of elements have their geometry fully defined by the element nodes. They are elements used to
mesh volumes in ANSYS. These volumes could be created in the ANSYS preprocessor or imported from a
CAD system. Hexahedral elements (bricks) can be used to mesh regularly shaped rectangular type volumes,
while tetrahedral elements (tets) can be used to mesh any volume. Even linear bricks (if they are not
distorted much) can model a thin plate in out-of-plane bending with one element through the thickness since
they all by default have the “extra shapes” turned on.

SOLID45: Basic linear brick.

SOLID95: 20 noded version of SOLID45. It can tolerate irregular shapes without as much loss of accuracy.
Well suited to model curved boundaries. These elements can also be tetrahedral and can automatically
transition between hexahedral and tetrahedral using pyramids.

SOLID185: Newer version of SOLID45. Also has mixed formulation capability for simulating
deformations of nearly incompressible elastoplastic materials, and fully incompressible hyperelastic
materials.

SOLID186: Newer version of SOLID95. Also has mixed formulation capability for simulating
deformations of nearly incompressible elastoplastic materials, and fully incompressible hyperelastic
materials.

SOLID92: Tetrahedral only element (10 noded quadratic).

SOLID187: Newer version of SOLID92. Similarly to other 18x elements also has mixed formulation
capability for simulating deformations of nearly incompressible elastoplastic materials, and fully
incompressible hyperelastic materials.




                                    Copyright 2003 Belcan Engineering Group, Inc.                        4
鲁班人   (http://www.lubanren.com/weblog/)


3D Shell Elements:

A shell element is a surface type element. It is really a 2D element that is called 3D because it is not
restricted to the XY plane like a 2D solid element; it can be located anywhere in three-dimensional space and
it can deform out-of-plane. Shell elements are engineering “abstractions” because a geometric surface has
no physical thickness. An ANSYS real constant is used to assign a thickness to a shell element. Shell
elements are also called plate elements, and are used to model panel type structures where the thickness is
small compared to the other dimensions of the part. They can carry in-plane loads (also called membrane
loads) and also out-of-plane bending moments and twisting.

SHELL63: This is an older but still very widely used shell element. It can analyze large deflections but not
plasticity.

SHELL93: Quadratic version of SHELL63. In addition it can analyze plasticity.

SHELL181: Newest linear shell element. Has plasticity and can also be used to model laminated composites
and sandwich panels. Note: There is no eight noded 18x series shell element.


Line Elements:

Line elements are a further engineering abstraction from shells; they are physically idealized as a simple line,
which represents a long slender structure that can carry axial, bending, shear and twisting forces. Real
constants define the cross sectional properties of the beam element.

BEAM3: Simple 2D beam element. Must be created in XY plane.

BEAM4: Beam element that can be modeled in 3D space. Has large deflection.

BEAM44: Tapered beam element. Can use the beam tool to define a section and have real constants
automatically calculated.

BEAM188: Timoshenko beam that includes shear deformation. Can handle plasticity and can define a
section with the beam tool. Can have a built-up cross section with more than one material. By default this is
a true linear element. You need a lot of them to give the same results as one BEAM3/4/44/189. In release
8.0 turn on KEYOPT(3) = 2 to give an internal quadratic shape function to eliminate this problem. Can
display stresses on the actual beam shape like it was solid.

BEAM189: Three noded quadratic version of BEAM188. This is pretty much the ultimate beam element
that can do everything well.


Conclusion:

ANSYS has many elements in its library, but it’s fast to narrow them down to just a few for your structural
analysis once you select an analysis approach. Try to stick with the 18x/20x series of elements when
possible because they incorporate the latest technology.




                                    Copyright 2003 Belcan Engineering Group, Inc.                             5

More Related Content

What's hot

Bending Stress In Beams
Bending Stress In BeamsBending Stress In Beams
Bending Stress In BeamsHitesh Singh
 
Finite element-modelling-techniques-in-msc-nastran-and-lsdyna
Finite element-modelling-techniques-in-msc-nastran-and-lsdynaFinite element-modelling-techniques-in-msc-nastran-and-lsdyna
Finite element-modelling-techniques-in-msc-nastran-and-lsdynaMarin Srdelić
 
13 r1-transient analysis methodology
13 r1-transient analysis methodology13 r1-transient analysis methodology
13 r1-transient analysis methodologychowdavaramsaiprasad
 
ME6603 - FINITE ELEMENT ANALYSIS UNIT - V NOTES AND QUESTION BANK
ME6603 - FINITE ELEMENT ANALYSIS UNIT - V NOTES AND QUESTION BANKME6603 - FINITE ELEMENT ANALYSIS UNIT - V NOTES AND QUESTION BANK
ME6603 - FINITE ELEMENT ANALYSIS UNIT - V NOTES AND QUESTION BANKASHOK KUMAR RAJENDRAN
 
Abaqus modelling and_analysis
Abaqus modelling and_analysisAbaqus modelling and_analysis
Abaqus modelling and_analysisDebanshu Sharma
 
An Introduction to the Finite Element Method
An Introduction to the Finite Element MethodAn Introduction to the Finite Element Method
An Introduction to the Finite Element MethodMohammad Tawfik
 
Introduction to Finite Element Analysis
Introduction to Finite Element Analysis Introduction to Finite Element Analysis
Introduction to Finite Element Analysis Madhan N R
 
Introduction to FEM
Introduction to FEMIntroduction to FEM
Introduction to FEMmezkurra
 
Finite element - axisymmetric stress and strain
Finite element - axisymmetric stress and strainFinite element - axisymmetric stress and strain
Finite element - axisymmetric stress and strainأحمد شاكر
 
Abaqus tutorial
Abaqus tutorialAbaqus tutorial
Abaqus tutorialnghiahanh
 
Rigid Body Dynamic
Rigid Body DynamicRigid Body Dynamic
Rigid Body DynamicNabeh Wildan
 

What's hot (20)

Finite Element Methods
Finite Element  MethodsFinite Element  Methods
Finite Element Methods
 
Joints powerpoint
Joints powerpointJoints powerpoint
Joints powerpoint
 
Bending Stress In Beams
Bending Stress In BeamsBending Stress In Beams
Bending Stress In Beams
 
Finite element-modelling-techniques-in-msc-nastran-and-lsdyna
Finite element-modelling-techniques-in-msc-nastran-and-lsdynaFinite element-modelling-techniques-in-msc-nastran-and-lsdyna
Finite element-modelling-techniques-in-msc-nastran-and-lsdyna
 
MEE1005 Materials Engineering and Technology s2- l9 -12
MEE1005 Materials Engineering and Technology s2- l9 -12MEE1005 Materials Engineering and Technology s2- l9 -12
MEE1005 Materials Engineering and Technology s2- l9 -12
 
Eg stress in beam
Eg stress in beamEg stress in beam
Eg stress in beam
 
ABAQUS 2018 Technical Update
ABAQUS 2018 Technical UpdateABAQUS 2018 Technical Update
ABAQUS 2018 Technical Update
 
13 r1-transient analysis methodology
13 r1-transient analysis methodology13 r1-transient analysis methodology
13 r1-transient analysis methodology
 
ME6603 - FINITE ELEMENT ANALYSIS UNIT - V NOTES AND QUESTION BANK
ME6603 - FINITE ELEMENT ANALYSIS UNIT - V NOTES AND QUESTION BANKME6603 - FINITE ELEMENT ANALYSIS UNIT - V NOTES AND QUESTION BANK
ME6603 - FINITE ELEMENT ANALYSIS UNIT - V NOTES AND QUESTION BANK
 
Abaqus modelling and_analysis
Abaqus modelling and_analysisAbaqus modelling and_analysis
Abaqus modelling and_analysis
 
An Introduction to the Finite Element Method
An Introduction to the Finite Element MethodAn Introduction to the Finite Element Method
An Introduction to the Finite Element Method
 
Introduction to Finite Element Analysis
Introduction to Finite Element Analysis Introduction to Finite Element Analysis
Introduction to Finite Element Analysis
 
Introduction to FEM
Introduction to FEMIntroduction to FEM
Introduction to FEM
 
FEA Report
FEA ReportFEA Report
FEA Report
 
Ansys tutorial
Ansys tutorialAnsys tutorial
Ansys tutorial
 
Finite element - axisymmetric stress and strain
Finite element - axisymmetric stress and strainFinite element - axisymmetric stress and strain
Finite element - axisymmetric stress and strain
 
Abaqus tutorial
Abaqus tutorialAbaqus tutorial
Abaqus tutorial
 
Rigid Body Dynamic
Rigid Body DynamicRigid Body Dynamic
Rigid Body Dynamic
 
What is FEA: Defining Finite Element Analysis
What is FEA: Defining Finite Element AnalysisWhat is FEA: Defining Finite Element Analysis
What is FEA: Defining Finite Element Analysis
 
Axis symmetric
Axis symmetricAxis symmetric
Axis symmetric
 

Viewers also liked

Reanalysis Method: Direct Method
Reanalysis Method: Direct MethodReanalysis Method: Direct Method
Reanalysis Method: Direct MethodAshvini Kumar
 
Presentation 24 October 2012 to School of Civil and Building Engineering, Lou...
Presentation 24 October 2012 to School of Civil and Building Engineering, Lou...Presentation 24 October 2012 to School of Civil and Building Engineering, Lou...
Presentation 24 October 2012 to School of Civil and Building Engineering, Lou...Andrea Wheeler
 
Teaching Kids and Students
Teaching Kids and StudentsTeaching Kids and Students
Teaching Kids and Studentskmaschke
 
Tecnology project structures
Tecnology project structuresTecnology project structures
Tecnology project structuresMiguelMarina97
 
The development of a new language of structures
The development of a new language of structuresThe development of a new language of structures
The development of a new language of structuresWolfgang Schueller
 
Pascal's Triangle slideshow
Pascal's Triangle slideshowPascal's Triangle slideshow
Pascal's Triangle slideshowecooperms
 

Viewers also liked (12)

Reanalysis Method: Direct Method
Reanalysis Method: Direct MethodReanalysis Method: Direct Method
Reanalysis Method: Direct Method
 
Presentation 24 October 2012 to School of Civil and Building Engineering, Lou...
Presentation 24 October 2012 to School of Civil and Building Engineering, Lou...Presentation 24 October 2012 to School of Civil and Building Engineering, Lou...
Presentation 24 October 2012 to School of Civil and Building Engineering, Lou...
 
bad architects group - selection
bad architects group - selection bad architects group - selection
bad architects group - selection
 
Teaching Kids and Students
Teaching Kids and StudentsTeaching Kids and Students
Teaching Kids and Students
 
Structures
StructuresStructures
Structures
 
Tecnology project structures
Tecnology project structuresTecnology project structures
Tecnology project structures
 
Steve Jones - Development of Civil Engineering Design skills through active l...
Steve Jones - Development of Civil Engineering Design skills through active l...Steve Jones - Development of Civil Engineering Design skills through active l...
Steve Jones - Development of Civil Engineering Design skills through active l...
 
The development of a new language of structures
The development of a new language of structuresThe development of a new language of structures
The development of a new language of structures
 
Pascal's Triangle slideshow
Pascal's Triangle slideshowPascal's Triangle slideshow
Pascal's Triangle slideshow
 
What is architecture
What is architectureWhat is architecture
What is architecture
 
High rise structure & core
High rise  structure & coreHigh rise  structure & core
High rise structure & core
 
Plan, section, elevation revised
Plan, section, elevation revisedPlan, section, elevation revised
Plan, section, elevation revised
 

Similar to Struct element types

Surface Structures, including SAP2000
Surface Structures, including SAP2000Surface Structures, including SAP2000
Surface Structures, including SAP2000Wolfgang Schueller
 
Stages of fea in cad environment
Stages of fea in cad environmentStages of fea in cad environment
Stages of fea in cad environmentrashmi322
 
03_Finite element method of analysis_Q & A (1) (1).pdf
03_Finite element method of analysis_Q & A (1) (1).pdf03_Finite element method of analysis_Q & A (1) (1).pdf
03_Finite element method of analysis_Q & A (1) (1).pdfPreethiRVR
 
Basic applied fem
Basic applied femBasic applied fem
Basic applied femAlbin Coban
 
Unit 1 notes-final
Unit 1 notes-finalUnit 1 notes-final
Unit 1 notes-finaljagadish108
 
ENGR7961 Finite Element MethodsAssessment I - Report Semes
ENGR7961 Finite Element MethodsAssessment I - Report SemesENGR7961 Finite Element MethodsAssessment I - Report Semes
ENGR7961 Finite Element MethodsAssessment I - Report SemesTanaMaeskm
 
Finite Element Modeling On Behaviour Of Reinforced Concrete Beam Column Joint...
Finite Element Modeling On Behaviour Of Reinforced Concrete Beam Column Joint...Finite Element Modeling On Behaviour Of Reinforced Concrete Beam Column Joint...
Finite Element Modeling On Behaviour Of Reinforced Concrete Beam Column Joint...IJERA Editor
 
Intro to fea software
Intro to fea softwareIntro to fea software
Intro to fea softwarekubigs
 
Free Vibration and Transient analysis of a Camshaft Assembly using ANSYS
Free Vibration and Transient analysis of a Camshaft Assembly using ANSYSFree Vibration and Transient analysis of a Camshaft Assembly using ANSYS
Free Vibration and Transient analysis of a Camshaft Assembly using ANSYSIRJET Journal
 
Finite element method (matlab) milan kumar rai
Finite element method (matlab) milan kumar raiFinite element method (matlab) milan kumar rai
Finite element method (matlab) milan kumar raiMilan Kumar Rai
 
FEA good practices presentation
FEA good practices presentationFEA good practices presentation
FEA good practices presentationMahdi Damghani
 
3D printing in textiles - programming and construction
3D printing in textiles - programming and construction3D printing in textiles - programming and construction
3D printing in textiles - programming and constructionmegr1412
 
feagoodpracticepresentation-191125101221.pdf
feagoodpracticepresentation-191125101221.pdffeagoodpracticepresentation-191125101221.pdf
feagoodpracticepresentation-191125101221.pdfJethallalGada
 

Similar to Struct element types (20)

Surface Structures, including SAP2000
Surface Structures, including SAP2000Surface Structures, including SAP2000
Surface Structures, including SAP2000
 
Introduction to fem
Introduction to femIntroduction to fem
Introduction to fem
 
Stages of fea in cad environment
Stages of fea in cad environmentStages of fea in cad environment
Stages of fea in cad environment
 
03_Finite element method of analysis_Q & A (1) (1).pdf
03_Finite element method of analysis_Q & A (1) (1).pdf03_Finite element method of analysis_Q & A (1) (1).pdf
03_Finite element method of analysis_Q & A (1) (1).pdf
 
Basic applied fem
Basic applied femBasic applied fem
Basic applied fem
 
Fem presentation
Fem presentationFem presentation
Fem presentation
 
Unit 1 notes-final
Unit 1 notes-finalUnit 1 notes-final
Unit 1 notes-final
 
ENGR7961 Finite Element MethodsAssessment I - Report Semes
ENGR7961 Finite Element MethodsAssessment I - Report SemesENGR7961 Finite Element MethodsAssessment I - Report Semes
ENGR7961 Finite Element MethodsAssessment I - Report Semes
 
Q26099103
Q26099103Q26099103
Q26099103
 
I044083842
I044083842I044083842
I044083842
 
FEM_PPT.ppt
FEM_PPT.pptFEM_PPT.ppt
FEM_PPT.ppt
 
Finite Element Modeling On Behaviour Of Reinforced Concrete Beam Column Joint...
Finite Element Modeling On Behaviour Of Reinforced Concrete Beam Column Joint...Finite Element Modeling On Behaviour Of Reinforced Concrete Beam Column Joint...
Finite Element Modeling On Behaviour Of Reinforced Concrete Beam Column Joint...
 
Ao04605289295
Ao04605289295Ao04605289295
Ao04605289295
 
Intro to fea software
Intro to fea softwareIntro to fea software
Intro to fea software
 
fea qb
 fea qb fea qb
fea qb
 
Free Vibration and Transient analysis of a Camshaft Assembly using ANSYS
Free Vibration and Transient analysis of a Camshaft Assembly using ANSYSFree Vibration and Transient analysis of a Camshaft Assembly using ANSYS
Free Vibration and Transient analysis of a Camshaft Assembly using ANSYS
 
Finite element method (matlab) milan kumar rai
Finite element method (matlab) milan kumar raiFinite element method (matlab) milan kumar rai
Finite element method (matlab) milan kumar rai
 
FEA good practices presentation
FEA good practices presentationFEA good practices presentation
FEA good practices presentation
 
3D printing in textiles - programming and construction
3D printing in textiles - programming and construction3D printing in textiles - programming and construction
3D printing in textiles - programming and construction
 
feagoodpracticepresentation-191125101221.pdf
feagoodpracticepresentation-191125101221.pdffeagoodpracticepresentation-191125101221.pdf
feagoodpracticepresentation-191125101221.pdf
 

Recently uploaded

Presiding Officer Training module 2024 lok sabha elections
Presiding Officer Training module 2024 lok sabha electionsPresiding Officer Training module 2024 lok sabha elections
Presiding Officer Training module 2024 lok sabha electionsanshu789521
 
Proudly South Africa powerpoint Thorisha.pptx
Proudly South Africa powerpoint Thorisha.pptxProudly South Africa powerpoint Thorisha.pptx
Proudly South Africa powerpoint Thorisha.pptxthorishapillay1
 
call girls in Kamla Market (DELHI) 🔝 >༒9953330565🔝 genuine Escort Service 🔝✔️✔️
call girls in Kamla Market (DELHI) 🔝 >༒9953330565🔝 genuine Escort Service 🔝✔️✔️call girls in Kamla Market (DELHI) 🔝 >༒9953330565🔝 genuine Escort Service 🔝✔️✔️
call girls in Kamla Market (DELHI) 🔝 >༒9953330565🔝 genuine Escort Service 🔝✔️✔️9953056974 Low Rate Call Girls In Saket, Delhi NCR
 
Framing an Appropriate Research Question 6b9b26d93da94caf993c038d9efcdedb.pdf
Framing an Appropriate Research Question 6b9b26d93da94caf993c038d9efcdedb.pdfFraming an Appropriate Research Question 6b9b26d93da94caf993c038d9efcdedb.pdf
Framing an Appropriate Research Question 6b9b26d93da94caf993c038d9efcdedb.pdfUjwalaBharambe
 
MICROBIOLOGY biochemical test detailed.pptx
MICROBIOLOGY biochemical test detailed.pptxMICROBIOLOGY biochemical test detailed.pptx
MICROBIOLOGY biochemical test detailed.pptxabhijeetpadhi001
 
ECONOMIC CONTEXT - LONG FORM TV DRAMA - PPT
ECONOMIC CONTEXT - LONG FORM TV DRAMA - PPTECONOMIC CONTEXT - LONG FORM TV DRAMA - PPT
ECONOMIC CONTEXT - LONG FORM TV DRAMA - PPTiammrhaywood
 
Introduction to AI in Higher Education_draft.pptx
Introduction to AI in Higher Education_draft.pptxIntroduction to AI in Higher Education_draft.pptx
Introduction to AI in Higher Education_draft.pptxpboyjonauth
 
18-04-UA_REPORT_MEDIALITERAСY_INDEX-DM_23-1-final-eng.pdf
18-04-UA_REPORT_MEDIALITERAСY_INDEX-DM_23-1-final-eng.pdf18-04-UA_REPORT_MEDIALITERAСY_INDEX-DM_23-1-final-eng.pdf
18-04-UA_REPORT_MEDIALITERAСY_INDEX-DM_23-1-final-eng.pdfssuser54595a
 
Procuring digital preservation CAN be quick and painless with our new dynamic...
Procuring digital preservation CAN be quick and painless with our new dynamic...Procuring digital preservation CAN be quick and painless with our new dynamic...
Procuring digital preservation CAN be quick and painless with our new dynamic...Jisc
 
Hierarchy of management that covers different levels of management
Hierarchy of management that covers different levels of managementHierarchy of management that covers different levels of management
Hierarchy of management that covers different levels of managementmkooblal
 
Capitol Tech U Doctoral Presentation - April 2024.pptx
Capitol Tech U Doctoral Presentation - April 2024.pptxCapitol Tech U Doctoral Presentation - April 2024.pptx
Capitol Tech U Doctoral Presentation - April 2024.pptxCapitolTechU
 
Alper Gobel In Media Res Media Component
Alper Gobel In Media Res Media ComponentAlper Gobel In Media Res Media Component
Alper Gobel In Media Res Media ComponentInMediaRes1
 
Full Stack Web Development Course for Beginners
Full Stack Web Development Course  for BeginnersFull Stack Web Development Course  for Beginners
Full Stack Web Development Course for BeginnersSabitha Banu
 
Organic Name Reactions for the students and aspirants of Chemistry12th.pptx
Organic Name Reactions  for the students and aspirants of Chemistry12th.pptxOrganic Name Reactions  for the students and aspirants of Chemistry12th.pptx
Organic Name Reactions for the students and aspirants of Chemistry12th.pptxVS Mahajan Coaching Centre
 
How to Make a Pirate ship Primary Education.pptx
How to Make a Pirate ship Primary Education.pptxHow to Make a Pirate ship Primary Education.pptx
How to Make a Pirate ship Primary Education.pptxmanuelaromero2013
 
Difference Between Search & Browse Methods in Odoo 17
Difference Between Search & Browse Methods in Odoo 17Difference Between Search & Browse Methods in Odoo 17
Difference Between Search & Browse Methods in Odoo 17Celine George
 
“Oh GOSH! Reflecting on Hackteria's Collaborative Practices in a Global Do-It...
“Oh GOSH! Reflecting on Hackteria's Collaborative Practices in a Global Do-It...“Oh GOSH! Reflecting on Hackteria's Collaborative Practices in a Global Do-It...
“Oh GOSH! Reflecting on Hackteria's Collaborative Practices in a Global Do-It...Marc Dusseiller Dusjagr
 
Earth Day Presentation wow hello nice great
Earth Day Presentation wow hello nice greatEarth Day Presentation wow hello nice great
Earth Day Presentation wow hello nice greatYousafMalik24
 
Painted Grey Ware.pptx, PGW Culture of India
Painted Grey Ware.pptx, PGW Culture of IndiaPainted Grey Ware.pptx, PGW Culture of India
Painted Grey Ware.pptx, PGW Culture of IndiaVirag Sontakke
 

Recently uploaded (20)

Presiding Officer Training module 2024 lok sabha elections
Presiding Officer Training module 2024 lok sabha electionsPresiding Officer Training module 2024 lok sabha elections
Presiding Officer Training module 2024 lok sabha elections
 
Proudly South Africa powerpoint Thorisha.pptx
Proudly South Africa powerpoint Thorisha.pptxProudly South Africa powerpoint Thorisha.pptx
Proudly South Africa powerpoint Thorisha.pptx
 
Model Call Girl in Bikash Puri Delhi reach out to us at 🔝9953056974🔝
Model Call Girl in Bikash Puri  Delhi reach out to us at 🔝9953056974🔝Model Call Girl in Bikash Puri  Delhi reach out to us at 🔝9953056974🔝
Model Call Girl in Bikash Puri Delhi reach out to us at 🔝9953056974🔝
 
call girls in Kamla Market (DELHI) 🔝 >༒9953330565🔝 genuine Escort Service 🔝✔️✔️
call girls in Kamla Market (DELHI) 🔝 >༒9953330565🔝 genuine Escort Service 🔝✔️✔️call girls in Kamla Market (DELHI) 🔝 >༒9953330565🔝 genuine Escort Service 🔝✔️✔️
call girls in Kamla Market (DELHI) 🔝 >༒9953330565🔝 genuine Escort Service 🔝✔️✔️
 
Framing an Appropriate Research Question 6b9b26d93da94caf993c038d9efcdedb.pdf
Framing an Appropriate Research Question 6b9b26d93da94caf993c038d9efcdedb.pdfFraming an Appropriate Research Question 6b9b26d93da94caf993c038d9efcdedb.pdf
Framing an Appropriate Research Question 6b9b26d93da94caf993c038d9efcdedb.pdf
 
MICROBIOLOGY biochemical test detailed.pptx
MICROBIOLOGY biochemical test detailed.pptxMICROBIOLOGY biochemical test detailed.pptx
MICROBIOLOGY biochemical test detailed.pptx
 
ECONOMIC CONTEXT - LONG FORM TV DRAMA - PPT
ECONOMIC CONTEXT - LONG FORM TV DRAMA - PPTECONOMIC CONTEXT - LONG FORM TV DRAMA - PPT
ECONOMIC CONTEXT - LONG FORM TV DRAMA - PPT
 
Introduction to AI in Higher Education_draft.pptx
Introduction to AI in Higher Education_draft.pptxIntroduction to AI in Higher Education_draft.pptx
Introduction to AI in Higher Education_draft.pptx
 
18-04-UA_REPORT_MEDIALITERAСY_INDEX-DM_23-1-final-eng.pdf
18-04-UA_REPORT_MEDIALITERAСY_INDEX-DM_23-1-final-eng.pdf18-04-UA_REPORT_MEDIALITERAСY_INDEX-DM_23-1-final-eng.pdf
18-04-UA_REPORT_MEDIALITERAСY_INDEX-DM_23-1-final-eng.pdf
 
Procuring digital preservation CAN be quick and painless with our new dynamic...
Procuring digital preservation CAN be quick and painless with our new dynamic...Procuring digital preservation CAN be quick and painless with our new dynamic...
Procuring digital preservation CAN be quick and painless with our new dynamic...
 
Hierarchy of management that covers different levels of management
Hierarchy of management that covers different levels of managementHierarchy of management that covers different levels of management
Hierarchy of management that covers different levels of management
 
Capitol Tech U Doctoral Presentation - April 2024.pptx
Capitol Tech U Doctoral Presentation - April 2024.pptxCapitol Tech U Doctoral Presentation - April 2024.pptx
Capitol Tech U Doctoral Presentation - April 2024.pptx
 
Alper Gobel In Media Res Media Component
Alper Gobel In Media Res Media ComponentAlper Gobel In Media Res Media Component
Alper Gobel In Media Res Media Component
 
Full Stack Web Development Course for Beginners
Full Stack Web Development Course  for BeginnersFull Stack Web Development Course  for Beginners
Full Stack Web Development Course for Beginners
 
Organic Name Reactions for the students and aspirants of Chemistry12th.pptx
Organic Name Reactions  for the students and aspirants of Chemistry12th.pptxOrganic Name Reactions  for the students and aspirants of Chemistry12th.pptx
Organic Name Reactions for the students and aspirants of Chemistry12th.pptx
 
How to Make a Pirate ship Primary Education.pptx
How to Make a Pirate ship Primary Education.pptxHow to Make a Pirate ship Primary Education.pptx
How to Make a Pirate ship Primary Education.pptx
 
Difference Between Search & Browse Methods in Odoo 17
Difference Between Search & Browse Methods in Odoo 17Difference Between Search & Browse Methods in Odoo 17
Difference Between Search & Browse Methods in Odoo 17
 
“Oh GOSH! Reflecting on Hackteria's Collaborative Practices in a Global Do-It...
“Oh GOSH! Reflecting on Hackteria's Collaborative Practices in a Global Do-It...“Oh GOSH! Reflecting on Hackteria's Collaborative Practices in a Global Do-It...
“Oh GOSH! Reflecting on Hackteria's Collaborative Practices in a Global Do-It...
 
Earth Day Presentation wow hello nice great
Earth Day Presentation wow hello nice greatEarth Day Presentation wow hello nice great
Earth Day Presentation wow hello nice great
 
Painted Grey Ware.pptx, PGW Culture of India
Painted Grey Ware.pptx, PGW Culture of IndiaPainted Grey Ware.pptx, PGW Culture of India
Painted Grey Ware.pptx, PGW Culture of India
 

Struct element types

  • 1. TIPS 鲁班人 (http://www.lubanren.com/weblog/) www.ansys.belcan.com Picking an Element Type For Structural Analysis: by Paul Dufour Picking an element type from the large library of elements in ANSYS can be an intimidating thing for a beginner. Out of the almost 200 available which one should I select? Why are there so many? Are there 181 kinds of shell elements? This article will address this issue for a structural analysis. The table below shows the most commonly used element types for stress analysis. Element 2D Solid 3D Solid 3D Shell Line Elements Order PLANE42 SOLID45 SHELL63 BEAM3/44 Linear PLANE182 SOLID185 SHELL181 BEAM188 PLANE82/183 SOLID95/186 SHELL93 BEAM189 Quadratic PLANE2 SOLID92/187 Element Naming Conventions: Elements are organized into groups of similar characteristics. These group names make up the first part of the element name (PLANE, SOLID, SHELL,etc). The second part of the element name is a number that is more or less (but not exactly) chronological. As elements have been created over the past 30 years the element numbers have simply been incremented. The earliest and simplest elements have the lowest numbers (LINK1, BEAM3, etc), the more recently developed ones have higher numbers. The “18x, 20x, and 22x” series of elements (SHELL181, SOLID187, etc) are the newest and most modern in the ANSYS element library. Some FEA codes (NASTRAN comes to mind) have just a handful of elements that do everything. There are several reasons why there are such a large number of elements in ANSYS. First, there was a conscious plan from the beginnings of the program that, for example, if you want to do a thermal analysis, there is no reason to use an element with structural degrees of freedom. That just requires an element to carry a bunch of baggage around that it is not using. While ANSYS does have coupled field elements that can do both, generally speaking if you want to do a thermal analysis you use an element with a temperature degree of freedom only, and structural elements do not drag around an unused temperature degree of freedom. This was done in the name of computational efficiency. Secondly, old elements are rarely deleted out of the program library for the sake of compatibility with older models. When a new and improved BEAM4 element was created, BEAM4 was not revised but left alone, and the BEAM44 was introduced. So the library keeps getting larger as new and more capable elements are formulated. The last reason is that ANSYS is a huge program with integrated capabilities in many physics fields. So there are elements for fluids, electromagnetics, electric field, acoustics, and explicit dynamics analyses as well.  Copyright 2003 Belcan Engineering Group, Inc. 1
  • 2. 鲁班人 (http://www.lubanren.com/weblog/) Element Order: Element order refers to the interpolation of an element’s nodal results to the interior of the element. This determines how results can vary across an element, and is important if you have high gradients of strain. A beam or plate in bending is a good example of this phenomenon, where the strain is changing sign over a potentially very small distance. Element order can be linear or quadratic. Linear elements do not have midside nodes. In general the strain can only vary linearly from one node to another. This is complicated in ANSYS with many “linear” elements having so called “extra shapes” or being “fully integrated”. This makes the elements behave more like a quadratic element, but not completely so. Naturally a linear element is computationally faster than a quadratic element. Quadratic elements have midside nodes. The shape function for strains varies in some nonlinear fashion between the corner nodes. Whereas linear elements are flat on both the sides and in-plane, a quadratic element can follow a curvature in both directions and is more accurate for a given number of nodes in the model. For example, in a tube with a hole, the curvature is maintained around the edges of the hole as well as on the curved edge of the panel; it is not a faceted representation as illustrated below. SHELL93 Quadratic Elements (8 nodes) SHELL181 Linear Elements (4 nodes) Some considerations in picking an element order: • For in-plane bending type problems, quadratic elements are much better than linear elements. Even several linear elements with “extra shapes” or “full integration” turned on are not as good one quadratic element. σ theo = 4318 psi 1 % error < % 2  Copyright 2003 Belcan Engineering Group, Inc. 2
  • 3. 鲁班人 (http://www.lubanren.com/weblog/) • Linear elements are more sensitive to non-perfect element shapes (i.e., have more error). A linear element is probably better in a mapped mesh than a free mesh. • For out-of-plane, plate type bending, there isn’t much difference between linear and quadratic elements. • Linear bricks give good results due to the “extra shapes” (full integration) if the elements are regularly shaped. If the volume has a shape complex enough to make skewed elements, mesh it with 20 node bricks or tetrahedral elements. An important side note here…linear triangles and tets give poor results since they are actually constant-strain elements (one value of strain calculated for the whole element. No gradient at all. These elements are no longer even available in ANSYS except as degenerate elements.). • As a general rule of thumb, one quadratic element containing three nodes should be more accurate than two linear elements having a total of three nodes across the same dimension. • In nonlinear analysis, a finer mesh of linear elements is computationally more efficient, robust, stable and more accurate than a coarser quadratic mesh with a comparable number of nodes. Make very simple models and experiment! Lame “advice”, I know…but it will never fail you! 2D Solid Elements: How can a 2D element be a “solid”? That’s a question most new ANSYS users ask. There are two reasons in ANSYS-speak. First, they are considered solid because they are not a shell or a beam element. Shells and beams are structural abstractions that will be discussed in the following sections. Secondly, they are solids because they fully represent a solid chunky part by modeling a cross section of that part. There are three main kinds of 2D solid elements: Plane Strain: In a plane strain analysis we are modeling something that is so long that there is no strain in the thickness direction. A cross section of a long beam or a dam holding back water would be examples of this kind of behavior. Stresses in the thickness direction are significant. Axisymmetric: In this type of analysis we are modeling a cross section of a structure that is fully defined by rotating the cross section around a central axis. A pressure vessel or bottle would be examples of this kind of structure. The thickness direction here represents the circumferential (hoop) direction and those out-of-plane stresses are very significant (picture a tank under pressure). Plane Stress: This is not really a “solid” element per say but still falls into this category (since it doesn’t really fit anywhere else). A plane stress analysis is a 2D model of a thin sheet with a small thickness and in- plane loading. You would get the same results with a shell model with in-plane loads only and the out-of- plane displacement constrained. All 2D solid elements can be any one of these three types by changing the element key options.  Copyright 2003 Belcan Engineering Group, Inc. 3
  • 4. 鲁班人 (http://www.lubanren.com/weblog/) PLANE42: Basic 2D solid element. PLANE82: 8 noded version of PLANE42. Also has a triangular option. PLANE182: Similar to PLANE42 except has capability for simulating deformations of nearly incompressible elastoplastic materials, and fully incompressible hyperelastic materials. PLANE183: 8 noded version of PLANE182. 3D Solid Elements: These types of elements have their geometry fully defined by the element nodes. They are elements used to mesh volumes in ANSYS. These volumes could be created in the ANSYS preprocessor or imported from a CAD system. Hexahedral elements (bricks) can be used to mesh regularly shaped rectangular type volumes, while tetrahedral elements (tets) can be used to mesh any volume. Even linear bricks (if they are not distorted much) can model a thin plate in out-of-plane bending with one element through the thickness since they all by default have the “extra shapes” turned on. SOLID45: Basic linear brick. SOLID95: 20 noded version of SOLID45. It can tolerate irregular shapes without as much loss of accuracy. Well suited to model curved boundaries. These elements can also be tetrahedral and can automatically transition between hexahedral and tetrahedral using pyramids. SOLID185: Newer version of SOLID45. Also has mixed formulation capability for simulating deformations of nearly incompressible elastoplastic materials, and fully incompressible hyperelastic materials. SOLID186: Newer version of SOLID95. Also has mixed formulation capability for simulating deformations of nearly incompressible elastoplastic materials, and fully incompressible hyperelastic materials. SOLID92: Tetrahedral only element (10 noded quadratic). SOLID187: Newer version of SOLID92. Similarly to other 18x elements also has mixed formulation capability for simulating deformations of nearly incompressible elastoplastic materials, and fully incompressible hyperelastic materials.  Copyright 2003 Belcan Engineering Group, Inc. 4
  • 5. 鲁班人 (http://www.lubanren.com/weblog/) 3D Shell Elements: A shell element is a surface type element. It is really a 2D element that is called 3D because it is not restricted to the XY plane like a 2D solid element; it can be located anywhere in three-dimensional space and it can deform out-of-plane. Shell elements are engineering “abstractions” because a geometric surface has no physical thickness. An ANSYS real constant is used to assign a thickness to a shell element. Shell elements are also called plate elements, and are used to model panel type structures where the thickness is small compared to the other dimensions of the part. They can carry in-plane loads (also called membrane loads) and also out-of-plane bending moments and twisting. SHELL63: This is an older but still very widely used shell element. It can analyze large deflections but not plasticity. SHELL93: Quadratic version of SHELL63. In addition it can analyze plasticity. SHELL181: Newest linear shell element. Has plasticity and can also be used to model laminated composites and sandwich panels. Note: There is no eight noded 18x series shell element. Line Elements: Line elements are a further engineering abstraction from shells; they are physically idealized as a simple line, which represents a long slender structure that can carry axial, bending, shear and twisting forces. Real constants define the cross sectional properties of the beam element. BEAM3: Simple 2D beam element. Must be created in XY plane. BEAM4: Beam element that can be modeled in 3D space. Has large deflection. BEAM44: Tapered beam element. Can use the beam tool to define a section and have real constants automatically calculated. BEAM188: Timoshenko beam that includes shear deformation. Can handle plasticity and can define a section with the beam tool. Can have a built-up cross section with more than one material. By default this is a true linear element. You need a lot of them to give the same results as one BEAM3/4/44/189. In release 8.0 turn on KEYOPT(3) = 2 to give an internal quadratic shape function to eliminate this problem. Can display stresses on the actual beam shape like it was solid. BEAM189: Three noded quadratic version of BEAM188. This is pretty much the ultimate beam element that can do everything well. Conclusion: ANSYS has many elements in its library, but it’s fast to narrow them down to just a few for your structural analysis once you select an analysis approach. Try to stick with the 18x/20x series of elements when possible because they incorporate the latest technology.  Copyright 2003 Belcan Engineering Group, Inc. 5