74

Chapter7: Beam problems (Element :BEAM3-2D- Elastic Beam)

BEAM3 - 2-D Elastic Beam geometry

Element Description

BEAM3 is a uniaxial element with tension, compression, and bending capabilities. The element has three degrees of freedom at each node: translations in the nodal x and y directions and rotation about the nodal z-axis.

Assumptions and Restrictions

• The beam element must lie in an X-Y plane and must not have a zero length or area. • The beam element can have any cross-sectional shape for which the moment of inertia can be

computed. However, the stresses are determined as if the distance from the neutral axis to the extreme fiber is one-half of the height.

• The element height is used only in the bending and thermal stress calculations. • The applied thermal gradient is assumed linear across the height and along the length. • The moment of inertia may be zero if large deflections are not used.

BEAM3 Input Data

Figure 7.1: "BEAM3 Geometry" shows the geometry, node locations, and the coordinate system for this element. The element is defined by two nodes, the cross-sectional area, the area moment of inertia, the height, and the material properties. The initial strain in the element (ISTRN) is given by ∆/L, where ∆ is the difference between the element length, L (as defined by the I and J node locations), and the zero strain length. The initial strain is also used in calculating the stress stiffness matrix, if any, for the first cumulative iteration.

75

You can use the element in an axisymmetric analysis if hoop effects are negligible, such as for bolts, slotted cylinders, etc. The area and moment of inertia must be input on a full 360° basis for an axisymmetric analysis. The shear deflection constant (SHEARZ) is optional. You can use a zero value of SHEARZ to neglect shear deflection. See Shear Deflection for details. The shear modulus (GXY) is used only with shear deflection. You can specify an added mass per unit length with the ADDMAS real constant.

Node and Element Loads describes element loads. You can specify pressures as surface loads on the element faces, shown by the circled numbers in Figure 7.1: "BEAM3 Geometry". Positive normal pressures act into the element. You specify lateral pressures as a force per unit length. End "pressures" are input as a force. KEYOPT(10) allows tapered lateral pressures to be offset from the nodes. You can specify temperatures as element body loads at the four "corner" locations shown in Figure 7.1: "BEAM3 Geometry". The first corner temperature T1 defaults to TUNIF. If all other temperatures are unspecified, they default to T1. If only T1 and T2 are input, T3 defaults to T2 and T4 defaults to T1. For any other input pattern, unspecified temperatures default to TUNIF.

KEYOPT(9) is used to request output at intermediate locations. It is based on equilibrium (free body of a portion of the element) considerations and is not valid if:

• stress stiffening is turned on [SSTIF,ON] • more than one component of angular velocity is applied [OMEGA ] • any angular velocities or accelerations are applied with the CGOMGA , DOMEGA , or DCGOMG

commands.

"BEAM3 Input Summary" summarizes the element input. Element Input contains a general description of element input.

BEAM3 Input Summary Nodes I, J Degrees of Freedom UX, UY, ROTZ Real Constants

AREA - Cross-sectional area

IZZ - Area moment of inertia

HEIGHT - Total beam height

SHEARZ - Shear deflection constant

ISTRN - Initial strain

ADDMAS - Added mass per unit length

Note :SHEARZ goes with the IZZ. If SHEARZ = 0, there is no shear deflection in the element Y direction.

Material Properties :EX, ALPX (or CTEX or THSX), DENS, GXY, DAMP Surface Loads

Pressure -- face 1 (I-J) (-Y normal direction)

face 2 (I-J) (+X tangential direction)

face 3 (I) (+X axial direction)

face 4 (J) (-X axial direction) (use a negative value for loading in the opposite direction)

76

Body Loads Temperatures -- T1, T2, T3, T4

BEAM3 Output Data

The solution output associated with the element is in two forms:

• Nodal displacements included in the overall nodal solution • Additional element output as shown in Table 3.1: "BEAM3 Element Output Definitions".

Figure 7.2: "BEAM3 Stress Output" illustrates several items. Solution Output gives a general description of solution output. See the ANSYS Basic Analysis Guide for ways to view results.

The Element Output Definitions table uses the following notation:

A colon (:) in the Name column indicates the item can be accessed by the Component Name method [ETABLE , ESOL]. The O column indicates the availability of the items in the file Jobname.OUT. The R column indicates the availability of the items in the results file.

In either the O or R columns, Y indicates that the item is always available, a number refers to a table footnote that describes when the item is conditionally available, and a - indicates that the item is not available.

Table 3.1 BEAM3 Element Output Definitions

Name Definition O R

EL Element Number Y Y

NODES Element nodes - I, J Y Y

MAT Element material number Y Y

VOLU: Element volume N Y

XC, YC Location where results are reported Y 3

TEMP Temperatures T1, T2, T3, T4 Y Y

PRES Pressure P1 at nodes I,J; OFFST1 at I,J; P2 at I,J; OFFST2 at I, J; P3 at I; P4 at J Y Y

SDIR Axial direct stress 1 1

SBYT Bending stress on the element +Y side of the beam 1 1

SBYB Bending stress on the element -Y side of the beam 1 1

SMAX Maximum stress (direct stress + bending stress) 1 1

SMIN Minimum stress (direct stress - bending stress) 1 1

EPELDIR Axial elastic strain at the end 1 1

EPELBYT Bending elastic strain on the element +Y side of the beam 1 1

EPELBYB Bending elastic strain on the element -Y side of the beam 1 1

EPTHDIR Axial thermal strain at the end 1 1

EPTHBYT Bending thermal strain on the element +Y side of the beam 1 1

77

Name Definition O R

EPTHBYB Bending thermal strain on the element -Y side of the beam 1 1

EPINAXL Initial axial strain in the element 1 1

MFOR(X, Y) Member forces in the element coordinate system X and Y direction 2 Y

MMOMZ Member moment in the element coordinate system Z direction 2 Y

1. The item repeats for end I, intermediate locations (see KEYOPT(9)), and end J. 2. If KEYOPT(6) = 1. 3. Available only at centroid as a *GET item.

The following tables list output available through the ETABLE command using the Sequence Number method. See The General Postprocessor (POST1) of the ANSYS Basic Analysis Guide and The Item and Sequence Number Table of this manual for more information. Table 3.2: "BEAM3 Item and Sequence Numbers (KEYOPT(9) = 0)" through Table 3.7: "BEAM3 Item and Sequence Numbers (KEYOPT(9) = 9)" all use the following notation:

Name output quantity as defined in the Table 3.1: "BEAM3 Element Output Definitions" Item predetermined Item label for ETABLE command E sequence number for single-valued or constant element data I,J sequence number for data at nodes I and J IL N sequence number for data at Intermediate Location N

Table 3.2 BEAM3 Item and Sequence Numbers (KEYOPT(9) = 0)

Output Quantity Name ETABLE and ESOL Command Input

Item E I J

SDIR LS - 1 4

SBYT LS - 2 5

SBYB LS - 3 6

EPELDIR LEPEL - 1 4

EPELBYT LEPEL - 2 5

EPELBYB LEPEL - 3 6

EPTHDIR LEPTH - 1 4

EPTHBYT LEPTH - 2 5

EPTHBYB LEPTH - 3 6

EPINAXL LEPTH 7 - -

SMAX NMISC - 1 3

SMIN NMISC - 2 4

MFORX SMISC - 1 7

MFORY SMISC - 2 8

MMOMZ SMISC - 6 12

78

Table 3.3 BEAM3 Item and Sequence Numbers (KEYOPT(9) = 1)

Output Quantity Name ETABLE and ESOL Command Input

Item E I ILI J

SDIR LS - 1 4 7

SBYT LS - 2 5 8

SBYB LS - 3 6 9

EPELDIR LEPEL - 1 4 7

EPELBYT LEPEL - 2 5 8

EPELBYB LEPEL - 3 6 9

EPTHDIR LEPTH - 1 4 7

EPTHBYT LEPTH - 2 5 8

EPTHBYB LEPTH - 3 6 9

EPINAXL LEPTH 10 - - -

SMAX NMISC - 1 3 5

SMIN NMISC - 2 4 6

MFORX SMISC - 1 7 13

MFORY SMISC - 2 8 14

MMOMZ SMISC - 6 12 18

P1 SMISC - 19 - 20

OFFST1 SMISC - 21 - 22

P2 SMISC - 23 - 24

OFFST2 SMISC - 25 - 26

P3 SMISC - 27 - -

P4 SMISC - - - 28

Pseudo Node

1 2 3 4

TEMP LBFE 1 2 3 4

79

SOLVED EXAMPLE ON BEAM ELEMENT

Problem24: Effect of Self Weight on a Cantilever Beam

Loads will not be applied to the beam shown below in order to observe the deflection caused by the weight of the beam itself. The beam is to be made

of steel with a modulus of elasticity of 200 GPa. L=1000mm, W=50mm, h=10mm

Preprocessing: Defining the Problem

1. Give example a Title:

Utility Menu > File > Change Title ... /title, Effects of Self Weight for a Cantilever Beam

2. Open preprocessor menu:

ANSYS Main Menu > Preprocessor /PREP7

3. Define Keypoints:

Preprocessor > Modeling > Create > Keypoints > In Active CS... K,#,x,y,z We are going to define 2 keypoints for this beam as given in the following

table:

Keypoint Coordinates

(x,y,z)

1 (0,0)

2 (1000,0)

4. Create Lines:

Preprocessor > Modeling > Create > Lines > Lines > In Active Coord L,1,2 Create a line joining Keypoints 1 and 2

5. Define the Type of Element

Preprocessor > Element Type > Add/Edit/Delete...

For this problem we will use the BEAM3 (Beam 2D elastic) element. This element has 3 degrees of freedom (translation along the X and Y axes, and rotation about the Z axis).

80

6. Define Real Constants

Preprocessor > Real Constants... > Add... In the 'Real Constants for BEAM3' window, enter the following geometric

properties: 1. Cross-sectional area AREA: 500

2. Area moment of inertia IZZ: 4166.67 3. Total beam height: 10

This defines a beam with a height of 10 mm and a width of 50 mm.

7. Define Element Material Properties

Preprocessor > Material Props > Material Models > Structural > Linear > Elastic > Isotropic

In the window that appears, enter the following geometric properties for steel: 1. Young's modulus EX: 200000

2. Poisson's Ratio PRXY: 0.3

8. Define Element Density

Preprocessor > Material Props > Material Models > Structural >

Linear > Density In the window that appears, enter the following density for steel:

1. Density DENS: 7.86e-6

9. Define Mesh Size

Preprocessor > Meshing > Size Cntrls > ManualSize > Lines > All Lines...

For this example we will use an element edge length of 100mm.

10. Mesh the frame

Preprocessor > Meshing > Mesh > Lines > click 'Pick All'

Solution Phase: Assigning Loads and Solving

1. Define Analysis Type

Solution > Analysis Type > New Analysis > Static ANTYPE,0

2. Apply Constraints

Solution > Define Loads > Apply > Structural > Displacement > On Keypoints

Fix keypoint 1 (ie all DOF constrained)

3. Define Gravity

It is necessary to define the direction and magnitude of gravity for this problem.

o Select Solution > Define Loads > Apply > Structural > Inertia > Gravity...

81

o The following window will appear. Fill it in as shown to define an

acceleration of 9.81m/s2 in the y direction.

Note: Acceleration is defined in terms of meters (not 'mm' as used

throughout the problem). This is because the units of acceleration and mass must be consistent to give the product of force units (Newtons in this case).

Also note that a positive acceleration in the y direction stimulates gravity in the negative Y direction.

There should now be a red arrow pointing in the positive y direction. This indicates that acceleration has been defined in the y direction. DK,1,ALL,0, ACEL,,9.8

The applied loads and constraints should now appear as shown in the figure

below.

4. Solve the System Solution > Solve > Current LS SOLVE

Postprocessing: Viewing the Results 1. Hand Calculations

Hand calculations were performed to verify the solution found using ANSYS: The maximum deflection was shown to be 5.777mm

82

2. Show the deformation of the beam

General Postproc > Plot Results > Deformed Shape ... > Def + undef edge PLDISP,2

As observed in the upper left hand corner, the

maximum displacement was found to be 5.777mm. This is in

agreement with the theortical value.

PROBLEMS ON TRANVERSE LOADING/Beam Element (BEAM3)

25. Find the shear force and bending moment diagram for the foll0wing problem. Rectangular c/s depth 20 mm,thickness 10mm

v= 0.3 E= 2x105N/mm2

SOLUTION: 1. File>change job name > Enter “Beam1” 2. Ansys Main Menu > Preferences > structural > Ok 3. Ansys Main Menu > Preprocessor > ELEMENT type > Add/edit/delete > add > Beam-

2D Elastic3 > OK

83

4. Ansys Main Menu > Preprocessor > Real constants > Add/edit/delete >Add>OK> set real Constant No: = 1 cross sectional Area = 200, Area Moment of Inertia=10x20e3/12,

Height=20 > OK > Close 5. Ansys Main Menu > Preprocessor > Material Properties > Material Models > Structural

> Linear > Elastic > Isotropic> Specify Material No: = 1> OK> Young’s modulus= 2E5, Poisson’s ration Minor= 0.3 > OK

6. Ansys Main Menu > Preprocessor >Modeling> Create > Nodes > In active CS > Set

Node No: = 1, X=0,Y=0, Z=0 > Apply > Set Node No: =2, X= 500, Y=0, Z=0 > Apply >

Set Node No: =3, X= 1000, Y=0, Z=0 > Apply > Set Node No: =4, X= 1500, Y=0, Z=0 > Apply >

Set Node No: =5, X= 2000, Y=0, Z=0 > OK

7. Ansys Main Menu > Preprocessor > Modeling > Create > elements > Auto Numbered > Thru Nodes > Pick 1 & 2 nodes > Apply > Pick 2 & 3 nodes > Apply > Pick 3 & 4 nodes

> Apply > Pick 4 & 5 nodes > OK 8. Ansys Main Menu > Preprocessor > Loads > Define Loads > apply > Structural

Displacement > On Nodes > Pick 1 > Ok > all DoF > OK

9. Ansys Main Menu > Preprocessor >loads > Define Loads > apply > Structural > Force/Moment > On Nodes > Pick 2nd Node > Ok > Select Fy – Apply as Constant Value

and Select Value of Force/Moment = -400N > Apply > Pick 3rd Node > Fy = -300N > Apply > Pick 4th Node > Fy = -800N > Apply > Pick 5th Node >

Fy = -500N > OK 10. Ansys Main Menu > solution >Solve Current LS >OK Soln Done > Close

11. Ansys main menu > general post processor > Element table > Define table > Add > set user label for item = SFD2, select item, comp, results data item = by sequence

number- select SMISC, 2 (Type 2 after selecting SMISC) > Apply > set user label for item = SFD8, select item, comp, results data item = by sequence number- select SMISC, 8 (Type 8 after selecting SMISC) > Apply >

set user label for item = BMD6, select item, comp, results data item = by sequence number- select SMISC, 6 (Type 6 after selecting SMISC) > Apply >

set user label for item = BMD12, select item, comp, results data item = by sequence

number- select SMISC, 12 (Type 12 after selecting SMISC) > Apply > OK > Close 12. Ansys Main Menu > General Post Processor > Element Table > List Element Table >

Select SFD2, SFD8 > OK > Note the stress in elements (Note the shear Forces) 13. Ansys Main Menu > General Post Processor > Element Table > List Element Table >

Select BMD6, BMD12 > OK > Note the stress in elements (Note the Bending Moments) 14. Ansys Main Menu > General Post Processor > Plot Results > Deformed Shape > Select

Def +Unreformed > OK (Blue line indicates deformed shape and white line indicates

original shape 15. Ansys Main Menu > General Post Processor > Plot Results > Contour Plots –Line

Element Results > Select Lab1=SFD2 and LabJ= SFD8 > Ok (see the shear forces in the members)

16. Ansys Main Menu > General Post Processor > Plot Results > Contour Plots –Line

Element Results > Select Lab1=BMD6 and LabJ= BMD12 > Ok (see the Bending Moment Diagram)

17. File > Save as > Select the user directory > Beam1 > OK

84

Results: ELEMENTAL SOLUTION- Shear Force and Bending Moment:

Max stress:____________ Location:____________ Max deflection:________________ Location:____________ Slope at tip:

Shear force diagram

Bending moment diagram Compare solutions from SOM.Also find deflections using SOM approach.

Node No. Shear Forces on Elements Bending Moment Values SFD2 SFD8 BMD6 BMD12

1 2 3 4

85

PROBLEMS ON TRANVERSE LOADING Beam Element(BEAM3)

26.Find the shear force and bending moment diagram for the following problem. Data: Rectangular c/s depth 120 mm,thickness 10mm,v= 0.3,

E= 2x105N/mm2 SOLUTION: 1. File>change job name > Enter “Beam2” 2. Ansys Main Menu > Preferences > structural > Ok

3. Ansys Main Menu > Preprocessor > ELEMENT type > Add/edit/delete > add > Beam-

2D Elastic3 > OK 4. Ansys Main Menu > Preprocessor > Real constants > Add/edit/delete > Add > OK > set

real Constant No: = 1 cross sectional Area = 1200, Area Moment of Inertia=10x120e3/12, Height=120 > OK > Close

5. Ansys Main Menu > Preprocessor > Material Properties > Material Models > Structural > Linear > Elastic > Isotropic> Specify Material No: = 1> OK> Young’s modulus= 2E5, Poisson’s ration Minor= 0.3 > OK

6. Ansys Main Menu > Preprocessor >Modeling> Create > Nodes > In active CS > Set Node No: = 1, X=0,Y=0, Z=0 > Apply >

Set Node No: =2, X= 2000, Y=0, Z=0 > Apply > Set Node No: =3, X= 4000, Y=0, Z=0 > Apply > Set Node No: =13, X= 8000, Y=0, Z=0 > OK

7. Ansys Main Menu > Preprocessor > Modeling > Create > Nodes > Auto Numbered > Fill Between Nodes > Pick 3 & 13 nodes > OK

8. Ansys Main Menu > Preprocessor > Modeling > Create > elements > Auto Numbered > Thru Nodes > Pick 1 & 2 nodes > Apply > Pick 2 & 3 nodes > Apply > Pick 3 & 4 nodes

> OK 9. Ansys Main Menu > Preprocessor > Modeling > Copy> Elements Auto numbered > Pick

3rd Element> OK Set Total Number of Copies = 10, Node Number increment = 1 > OK

10. Ansys Main Menu > Preprocessor > Loads > Define Loads > apply > Structural Displacement > On Nodes > Pick 1 and 13 > Ok > Select Uy > OK

11. Ansys Main Menu > Preprocessor >loads > Define Loads > Apply > Structural > Force/Moment > On Nodes > Pick 2nd Node > Ok > Select Fy – Apply as Constant Value and Select Value of Force/Moment = -30000N > Apply > Pick 3rd Node > Fy =-20000N

> OK 12. Ansys Main Menu > Preprocessor >loads > Define Loads > apply > Pressure > on

Beams > Pick > Select all the elements between node 3 and 13(Use box option to select the elements) > OK > Set LKEY=1, VALI=10>OK

13. Ansys Main Menu > solution >Solve Current LS >OK Soln Done > Close

86

14. Ansys main menu > general post processor > Element table > Define table > Add > set user label for item = SFD2, select item, comp, results data item = by sequence

number- select SMISC, 2 (Type 2 after selecting SMISC) > Apply > set user label for item = SFD8, select item, comp, results data item = by sequence

number- select SMISC, 8 (Type 8 after selecting SMISC) > Apply > set user label for item = BMD6, select item, comp, results data item = by sequence

number- select SMISC, 6 (Type 6 after selecting SMISC) > Apply >

set user label for item = BMD12, select item, comp, results data item = by sequence number- select SMISC, 12 (Type 12 after selecting SMISC) > Apply > OK > Close

15. Ansys Main Menu > General Post Processor >Element Table >List Element Table > Select SFD2, SFD8 > OK > Note the stress in elements (Note the shear Forces)

16. Ansys Main Menu > General Post Processor > Element Table > List Element Table >

Select BMD6, BMD12 > OK > Note the stress in elements (Note the Bending Moments) 17. Ansys Main Menu > General Post Processor > Plot Results > Deformed Shape > Select

Def + Undeformed > OK (Blue line indicates deformed shape and white line indicates original shape

18. Ansys Main Menu > General Post Processor > Plot Results > Contour Plots –Line Element

Results > Select Lab1=SFD2 and LabJ= SFD8 > Ok (see the shear forces in the members)

19. Ansys Main Menu > General Post Processor > Plot Results > Contour Plots –Line Element Results > Select Lab1=BMD6 and LabJ= BMD12 > Ok (see the Bending Moment

Diagram)

20. File > Save as > Select the user directory > Beam2 > OK

Results: ELEMENTAL SOLUTION- Shear Force and Bending Moment:

Also obtain maximum stress,maximum deflection and locations

Node No. Shear Forces on Elements Bending Moment Values

SFD2 SFD8 BMD6 BMD12

1 2 3 4 5 6 7 8 9 10 11 12

87

Exercises : BEAM PROBLEMS Problem – 27 A long cantilever beam with 30 mm square cross-section and 1000 mm length (see figure below) is subjected to (a) Concentrated tip force (b) Concentrated tip moment (c) Distributed pressure load Each loading is applied separately. Loading Deflection (mm) Bending Moment

(N-mm) Max. Bending Stress (N/mm2)

ANSYS Theory ANSYS Theory ANSYS Theory

Case A F=10KN

Case B M=10KN-m

Case C P=5Mpa

Problem – 28 A long cantilever beam with 30 mm square cross-section and 1000 mm length is subjected to an off-centered axial force of 1000 N (see figure below). The force is offset by 100 mm.

Result Node

No. Deflection (mm)

Node No. Bending Moment (N-mm)

Element No.

Max. Bending Stress (N/mm2)

ANSYS Analysis

Theory

88

Problem – 29 Determine the end forces of a clamped-clamped beam due to a 25 mm settlement at the right end. A = 50 X 50 Sq. E = 200 Gpa l = 2 m

Result Node

No. Deflection (mm)

Node No. Bending Moment (N-mm)

Element No.

Max. Bending Stress (N/mm2)

ANSYS Analysis

Theory

Problem – 30 Determine the end forces of a clamped-clamped beam due to a 1 radian imposed rotation at the right end. A = 50 X 50 Sq. E = 200 Gpa l = 2 m

Result Node

No. Deflection (mm)

Node No. Bending Moment (N-mm)

Element No.

Max. Bending Stress (N/mm2)

ANSYS Analysis

Theory

89

Problem – 31 A beam of length L and height h is built-in at one end and loaded at free end with (A) a shear force F, and (B) a moment M. Determine the deflection at the free end. A = 50 X 50 Sq. E = 200 Gpa l = 2 m

Result Node

No. Deflection (mm)

Node No. Bending Moment (N-mm)

Element No.

Max. Bending Stress (N/mm2)

ANSYS Analysis

Theory Problem – 32 The figure shows a loaded beam subjected to various types of loading E = 200 Gpa I = 4 X 106 mm4

Result Max Deflection (mm)

Node No. Bending Moment (N-mm)

Element No.

Max. Bending location Stress (N/mm2)

ANSYS Analysis

Theory

90

Problem – 33 Using the beam elements to model a steel beam structure as shown in figure, find the deflected shape and the reaction forces.

Result Deflection

(mm) Node No.

Node No. Bending Moment (N-mm)

Element No.

Max. Bending Stress (N/mm2)

ANSYS Analysis

Theory Problem – 34 Using three elements to model a steel beam structure as shown in figure, find the deflected shape and the reaction forces at the ends.

Result Deflecti

on (mm)

Node No. Bending Moment (N-mm)

Node No. Max. Bending Stress (N/mm2)

Element No.

ANSYS Analysis

Theory

91