FINAL PROJECT

Finite Element Techniques I: FINAL PROJECT
Due on Wednesday, December 14, 2016
Report and Manual for code
Ebenesh Rabiraj
1

Finite Element Techniques I (Report and Manual for code)
Contents
Problem statement 3
Questions to answer . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 3
Ansys Implementation 4
General procedure . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 4
Extract files required for MATLAB . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 5
Sample input . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 5
Matlab Implementation 8
T3 element . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 8
Q4 element . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 9
Results 11
T3 element . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 11
Coarse mesh . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 11
Medium mesh . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 13
Fine mesh . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 14
Very fine mesh . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 15
Q4 element . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 16
Coarse mesh . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 16
Medium mesh . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 18
Fine mesh . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 19
Very fine mesh . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 20
Discussion 21
Convergence Study . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 21
Error Study . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 22
Code 23
How to run it . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 23
Page 2 of 29

Problem statement
The figure above represents a simply supported beam with the following given conditions,
l = 20m
h = 2m
w = 2000N/m
ν = 0.3
E = 2e11 Pa
Questions to answer
• Use Ansys Q4 element to analyze a plane-stress beam.
• In the second part of this project, you will use the matlab program based on linear triangular element
(T3 element) solve the same problem. You need to modify the code so that it can input the triangular
mesh generated from ANSYS. The best way is to create an input file that contains all the nodal and
connectivity information and let you code read it.
• In this part of the project, you will develop a matlab program using Q4 element for solving the same
problem. To implement this, you will need to modify the code on T3 to implement the formulation
discussed in class for Q4. To apply it to the problem above, you can generate the mesh using ANSYS
and then input them to your own code. Use 2 by 2 Gauss quadrature for evaluating the stiffness
matrix.
1) A short write-up on implementation (similar to the Ansys assignments)
2) The FEM model (mesh), and deformed shape and stress.
3) For each types of element, prescribe three types of mesh (coarse, fine and very fine) densities. Compare
maximum deflection with the analytical solution and compute the error as a function of the mesh spacing
on a log-log scale plot.
4) Similar to 3), but compare the stress value σ xx at x= 0, y =h / 2 .
Page 3 of 29

Ansys Implementation
General procedure
In the ansys implementation we follow the procedure given below keeping in mind that the version of Ansys
may be different from the ine I have used and there may be minor variations.
• Perferences
→ Structural
• Preprocessor
→ Element Type→ Add/Edit/Delete→ Add→ Solid→ Quad 4 node 182
→ Material Properties→ material models → Structural→ Linear→ Elastic→ Isotropic
→ EX=2e11
→ PRXY=0.3
→ Modelling→ Create→ Areas→ Rectangle → By 2 Corners
→ WP X→ -20
→ WP Y→ -1
→ Width→ 40
→ Height→ 2
→ Meshing→ MeshTool
→ Check the smart size button
→ Set the slider to,
→ 9→ coarse
→ 6→ medium
→ 4→ fine
→ 2→ very fine
→ Set Mesh to Area
→ Select the shape as tri
→ Click Mesh
• Solution
→ Define Loads→ → Apply→ Structural
→ Displacement
→ Select node(-20,-1)→ UX,UY
→ Select node(20,-1)→ UY
→ Pressure→ Select the upper nodes along y=1→ Constant value=2000
→ Solve→ Current LS→ OK
• General Postproc→ Plot Results (as and what is displayed)
Page 4 of 29

Extract files required for MATLAB
The meshing of the given beam is done in Ansys and imported into MATLAB. For a sucessfull run, Ansys
will have to output 4 files
• NLIST.lis (Provides the Nodal coordinates)
• MAIN MENU⇒ List→ Nodes
• ELIST.lis (Provides the elements and the nodes in them)
• MAIN MENU⇒ List→ Elements→ on all nodes
• DLIST.lis (Provides the Nodal DOF)
• MAIN MENU⇒ List→ Loads→ DOF constraints → On all nodes
• SFLIS.lis (Provides the pressure applied on a surface with the constant load value across the nodes on
the surface)
• MAIN MENU⇒ List→ Loads→ Surfaces→ On all nodes
Sample input
The following input is generated by ansys for a T3 element with a coarse mesh. These files are imported
into the MATLAB main program through the code attached in an upcoming section.
INPUT to MATLAB
LIST ALL SELECTED NODES. DSYS= 0
SORT TABLE ON NODE NODE NODE
NODE X Y Z
1 -20.0000000000 -1.00000000000 0.00000000000
2 20.0000000000 -1.00000000000 0.00000000000
3 20.0000000000 1.00000000000 0.00000000000
4 -20.0000000000 1.00000000000 0.00000000000
5 -18.0000000000 -1.00000000000 0.00000000000
6 -14.2000000000 -1.00000000000 0.00000000000
7 -10.4000000000 -1.00000000000 0.00000000000
8 -6.60000000000 -1.00000000000 0.00000000000
9 -1.00000000000 -1.00000000000 0.00000000000
10 2.80000000000 -1.00000000000 0.00000000000
11 6.60000000000 -1.00000000000 0.00000000000
12 10.4000000000 -1.00000000000 0.00000000000
13 14.2000000000 -1.00000000000 0.00000000000
14 18.0000000000 -1.00000000000 0.00000000000
15 18.0000000000 1.00000000000 0.00000000000
16 14.2000000000 1.00000000000 0.00000000000
17 10.4000000000 1.00000000000 0.00000000000
18 6.60000000000 1.00000000000 0.00000000000
19 1.00000000000 1.00000000000 0.00000000000
20 -2.80000000000 1.00000000000 0.00000000000
NODE X Y Z
21 -6.60000000000 1.00000000000 0.00000000000
22 -10.4000000000 1.00000000000 0.00000000000
23 -14.2000000000 1.00000000000 0.00000000000
24 -18.0000000000 1.00000000000 0.00000000000
Page 5 of 29

25 19.0000000000 0.00000000000 0.00000000000
26 -19.0000000000 0.00000000000 0.00000000000
INPUT to MATLAB
LIST ALL SELECTED ELEMENTS. LIST NODES
ELEM MAT TYP REL ESY SEC NODES
1 1 1 1 0 1 15 13 14 14
2 1 1 1 0 1 15 16 13 13
3 1 1 1 0 1 24 26 5 5
4 1 1 1 0 1 5 26 1 1
5 1 1 1 0 1 26 4 1 1
6 1 1 1 0 1 24 4 26 26
7 1 1 1 0 1 2 25 14 14
8 1 1 1 0 1 14 25 15 15
9 1 1 1 0 1 25 3 15 15
10 1 1 1 0 1 2 3 25 25
11 1 1 1 0 1 13 16 12 12
12 1 1 1 0 1 12 17 11 11
13 1 1 1 0 1 16 17 12 12
14 1 1 1 0 1 11 18 10 10
15 1 1 1 0 1 17 18 11 11
16 1 1 1 0 1 19 10 18 18
17 1 1 1 0 1 19 9 10 10
18 1 1 1 0 1 9 20 8 8
19 1 1 1 0 1 19 20 9 9
20 1 1 1 0 1 8 21 7 7
ELEM MAT TYP REL ESY SEC NODES
21 1 1 1 0 1 20 21 8 8
22 1 1 1 0 1 7 22 6 6
23 1 1 1 0 1 21 22 7 7
24 1 1 1 0 1 6 23 5 5
25 1 1 1 0 1 22 23 6 6
26 1 1 1 0 1 24 5 23 23
INPUT to MATLAB
LIST CONSTRAINTS FOR SELECTED NODES 1 TO 26 BY 1
CURRENTLY SELECTED DOF SET= UX UY
NODE LABEL REAL IMAG
1 UX 0.00000000 0.00000000
1 UY 0.00000000 0.00000000
2 UY 0.00000000 0.00000000
INPUT to MATLAB
Page 6 of 29

The surface loads listed are the current database values and are not
necessarily the values corresponding to the current results data set.
Tabular boundary conditions, however, do list values corresponding to
the current results set.
LIST NODAL SURFACE LOAD PRES FOR ALL SELECTED NODES
ELEMENT LKEY FACE NODES REAL IMAGINARY
2 1 16 2000.00000 0.00000000
15 2000.00000 0.00000000
6 1 4 2000.00000 0.00000000
24 2000.00000 0.00000000
9 2 15 2000.00000 0.00000000
3 2000.00000 0.00000000
13 1 17 2000.00000 0.00000000
16 2000.00000 0.00000000
15 1 18 2000.00000 0.00000000
17 2000.00000 0.00000000
16 4 19 2000.00000 0.00000000
18 2000.00000 0.00000000
19 1 20 2000.00000 0.00000000
19 2000.00000 0.00000000
21 1 21 2000.00000 0.00000000
20 2000.00000 0.00000000
23 1 22 2000.00000 0.00000000
21 2000.00000 0.00000000
25 1 23 2000.00000 0.00000000
22 2000.00000 0.00000000
ELEMENT LKEY FACE NODES REAL IMAGINARY
26 4 24 2000.00000 0.00000000
23 2000.00000 0.00000000
Page 7 of 29

Matlab Implementation
T3 element
From the implementation in the previous assignment, developed from the code provided, we have a working
code that helps us solve the problem by utilizing a T3 mesh element.
Figure 1: T3 element representing 3 nodes at the vertices of a triangle numbered in a clockwise direction.
Courtesy of University of Rome class notes
The T3 element is made up of 3 nodes at the vertices of a triangle numbered in a clockwise direction. Each
vertex has 2 degrees of freedom, a displacement in the the x and y direction [3]. This displacement can be
expressed as,
u
v
=
N1 0 N2 0 N3 0
0 N1 0 N2 0 N3



u1
v1
u2
v2
u3
v3



where N1, N2 and N3 are the shape functions. The stiffness matrix can be written as,
k = V
BT
EBdV
where,
B =


y23 0 y31 0 y12 0
0 x32 0 x13 0 x21
x32 y23 x13 y31 x21 y12


and,
xij = xi − xj; yij = yi − yj;
Keeping this in mind an algorithm can be developed where the stiffness matrix for the entire element
is calculated as a superpositioning of the elemental stiffness matrix. The integration is carried out in a
numerical fashion.
Page 8 of 29

Q4 element
Figure 2: Q4 element representing 4 nodes at the vertices of a isoparametric quadrilateral. Courtesy of
University of colorado class notes.
The Q4 element is a 4 node isoparametric element. In the case of the Q4 element we need to use a different
strategy for numerical integration of the quadrature points. Gauss integration method is the most standard
practice followed [5]. The stiffness matrix is represented as,
k = A
BT
EBtdxdy
The stiffness matrix in this case is an 8x8 matrix. It is similar to that of the T3 element, however, the B
martix is modified as,
B =


1 0 0 0
0 0 0 1
0 1 1 0

 τ
τ




N1,ξ 0 N2,ξ 0 N3,ξ 0 N4,ξ 0
N1,η 0 N2,η 0 N3,η 0 N4,η 0
0 N1,ξ 0 N2,ξ 0 N3,ξ 0 N4,ξ
0 N1,η 0 N2,η 0 N3,η 0 N4,η




where τ = J−1
. J is the jacobian matrix that is represented as,
J =
N1,ξ N2,ξ N3,ξ N4,ξ
N1,η N2,η N3,η N4,η




x1 y1
x2 y2
x3 y3
x4 y4




Gauss quadrature based integration is used to integrate the stiffness equation. The 1D form of the gauss
quadrature is represented as,
k =
1
−1
F(ξ)dξ ≈
p
i=1 ωiF(ξi)
Page 9 of 29

Here we can understand that p represents the sample points for integration, ωi represents the weights for
integration and ξ is the sample point within the interval [-1,1].
To extend this to the 2D formulation we reduce the integration to it’s canonical form to better show the
process. The integration is thus represented as,
k =
1
−1
1
−1
F(ξ, η)dξdη ≈
p1
i=1
p2
i=1 ωiωjF(ξi, ηj)
According to our question we intend to use the 2x2 gauss quadrature to evaluate the stiﬀness matrix.
Figure 3: 2D gauss product rule implementation where p=2 depicted over a straight-sided quadrilateral
region. The sample points are represented as black dots. Courtesy of University of colorado class notes.
The sample points as see in Figure 3 are taken in the counter clockwise direction from the segment in the 1st
quadrature as, [ 1√
3
, 1√
3
], [− 1√
3
, 1√
3
], [− 1√
3
, − 1√
3
], [ 1√
3
, − 1√
3
]. These values are plugged into the weight terms
ωi and ωj
The matlab code that has been developed does the calculations based on the nodal and elemental information
provided by the Ansys export as discussed earlier. The matlab script imports the desired nodal and elemental
information from the .lis ﬁles mentioned and arranges them in the required form.
NOTE: The code remains unchanged even if the mesh of the beam is changed. However, if the inputs such
as young’s modulus and poisson’s ratio need to be updated in the code if changed.
Page 10 of 29

Results
This section shows teh results obtained from Matlab and Ansys. Every coarse mesh shows the deflection and
the stress induced on the beam. The deflection is exagerated such that the beam passes the bottom length
of the beam. The nodes of beam are represented as scatter points. The element data is not shown. The
stress plots are not separately shown, however the points where the stress is maximum and minimum are
plotted. The red node shows a point of maximum stress and the green shows the point of minimum stress.
Since the stress in the x direction is uniform and a much lower value, it is neglected. The stress in the y
direction is only depicted. The ansys plot shows the deflection and sheer stress or σxy.
T3 element
Coarse mesh
Page 11 of 29

Page 12 of 29

Medium mesh
Page 13 of 29

Fine mesh
Page 14 of 29

Very ﬁne mesh
Page 15 of 29

Q4 element
The Q4 plots are also similare to the T3. It is important to note that the in the Q4 analysis each quadrilateral
has a node of minimum stress and a node of maximum stress. Only the node that has the least stress in
depicted in the diagram. The coarse mesh, as will be seen in a later section is innacurate or shows that the
node of maximum stress and minimum stress to be the same. This point then spreads to more reasonable
points as the mesh densities increase.
Coarse mesh
Page 16 of 29

Page 17 of 29

Medium mesh
Page 18 of 29

Fine mesh
Page 19 of 29

Very ﬁne mesh
Page 20 of 29

Discussion
Convergence Study
There are many ways to conduct convergence analysis [1] [2]. In essence we need to show how the solution,
whether it be displacement or stress approaches the analytical solution. We have been provided the solution
for the displacements and the stresses in the question. First we will look at the convergence of the maximum
displacement of the beam using a coarsely meshed beam. This solution is plotted as a function of increasing
refinement in the mesh. In the figure below we analyse the mesh at 4 points. The curve is interpolated
between the 4 points for clarity. The bold dots show the actual measurements from the matlab code or
Ansys result.
As seen above the x axis represents the density of the mesh across the beam. The graph shows that over
the given range of meshes ranging from 26 nodes to 635 nodes the obtained results quickly move toward the
analytical solution. In the case of the displacement graph we can also see how well the Ansys and Matlab
simulations agree with each other at the different mesh points. Seeing how well the results match we can
move to the stress plot without checking the similarities between the Ansys and Matlab plots. Instead we
will focus on the change in accuracy over the mesh density range.
The stresses in these kind of beams are also an important factor to look at. A clear explanation of the
stresses in a beam is provided by David Roylance in his notes [4]. The stresses are calculated using the
analytical solution provided in the question and then the code is run to calculate the principal stress. The
output is then plotted as shown below.
Page 21 of 29

The plots also shows an important trait of the T3 and Q4 elements. Both the T3 and the Q4 elements
converge at different rates. The T3 element as expected is more stiff. The stiffness causes a less accurate
deflection but is closer in terms of stress.
It is important to note that for both the stress and displacement convergence studies, the curve is a contin-
uous, interpolated curve drawn over the points derived from those in the Matlab/Ansys simulations.
Error Study
The error is nothing but a difference in the actual solution and the solution obtained using the finite element
techniques. The error plotted in a log log scale to enhance the nuances in the curve. The change in density
shows a steep decline in the error in the Q4 element although the T3 element remains a little stiffer as it
approaches the 0 error point.
Page 22 of 29

Code
How to run it
• The first step is to determine the mesh density.
• The mesh density ranges from 1-4 which points the code to different directories to grab the input files.
• There are separate scripts that import the nodes, Elements, DOF and Nodal force information
mesh=4;
if mesh==1
5 mesh=’Q4coarse’;
end
if mesh==2
mesh=’Q4medium’;
end
10 if mesh==3
mesh=’Q4fine’;
end
if mesh==4
mesh=’Q4very fine’;
15 end
%------------------------------------
% raw data
%------------------------------------
20 fprintf(’Importing nodes’);
ImportQ4nodes;
fprintf(’Done n’);
fprintf(’Importing Elements’);
ImportQ4ele;
25 fprintf(’Done n’);
fprintf(’Importing DOF Information’);
ImportQ4DOF;
fprintf(’Importing Nodal Force Information’);
30 ImportQ4Lnode;
• The code then fixes errors in the nodes
fix1=Quad1;
fix2=Quad2;
fix3=Quad3;
fix4=Quad4;
5 fix5=LISTCONS;
fix6=LNode;
for ifixNoN=1:length(Node)
10 actualnode=Node(ifixNoN);
Page 23 of 29

flag=1;
if actualnode˜=ifixNoN
if flag==1
fprintf(’Nodal numbering error found’);
15 flag=flag+1;
end
fprintf(’.’);
loc=find(fix1==actualnode);
loclength=length(loc);
20 for replace=1:loclength
fix1(loc(replace))=ifixNoN;
end
end
end
end
end
end
end
if flag==2
50 fprintf(’nNodal numbering error fixedn’);
flag=flag+1;
end
end
55 quad1=fix1;
quad2=fix2;
quad3=fix3;
quad4=fix4;
LISTCONS=fix5;
60 LNode=fix6;
if flag==1
fprintf(’nNo nodal numbering issues foundn’);
flag=flag+1;
Page 24 of 29

end
• This part is important.
• The inputs of the beam are provided here.
• These are used in subsequent calculations.
%------------------------------------
% input data for control parameters
%------------------------------------
fprintf(’nInput data for control parametersn’);
5 nel=length(quad1); % number of elements
nnel=4; % number of nodes per element
ndof=2; % number of dofs per node
nnode=length(Node); % total number of nodes in system
sdof=nnode*ndof; % total system dofs
10 edof=nnel*ndof; % degrees of freedom per element
emodule=2e11; % elastic modulus
poisson=0.3; % Poisson’s ratio
fprintf(’n================================================’);
fprintf(’n Number of elements are %g’,nel);
15 fprintf(’n Number of nodes per element are %g’,nnel);
fprintf(’n Number of dofs per node are %g’,ndof);
fprintf(’n Number of of nodes in system are %g’,nnode);
fprintf(’n Number of system dofs are %g’,sdof);
fprintf(’n Number of degrees of freedom per element are %g’,edof);
20 fprintf(’n Elastic modulus is %g N/mmˆ2’,emodule);
fprintf(’n Poissons ratio is %g’,poisson);
fprintf(’n================================================nn’);
%---------------------------------------------
% input data for nodal coordinate values
25 % gcoord(i,j) where i->node no. and j->x or y
%---------------------------------------------
fprintf(’n Mapping nodal coordinates’);
gcoord=[X,Y];
30 %---------------------------------------------------------
% input data for nodal connectivity for each element
% nodes(i,j) where i-> element no. and j-> connected nodes
%---------------------------------------------------------
fprintf(’n Connecting nodes’);
35 nodes=[quad1,quad2,quad3,quad4];
• The next thing to look at is the force matrix.
• Here were need to understand that Ansys provides only the nodes on which the pressure is applied and
the force per unit area.
%----------------------------
% force vector
%----------------------------
5
Page 25 of 29

fprintf(’n Force vector’);
for i=1:2:length(LNode)
distxyloc=[gcoord((LNode(i+1)),1),gcoord((LNode(i+1)),2);gcoord((LNode(i)),1),
gcoord((LNode(i)),2)];
distxy=pdist(distxyloc);
10 ff((LNode(i)*2))=ff((LNode(i)*2))+(LNodeVal(i)*(distxy)/2);
%ff((LNode(i)*2))=LNodeVal(i)*(distxy)/2;
ff((LNode(i+1)*2))=ff((LNode(i+1)*2))+(LNodeVal(i+1)*(distxy)/2);
end
sum(ff)
• For the Q4 variation is mostly centered about the next piece of code.
• As mentioned in a previous section we use 2x2 gauss integration to solve the problem.
• This is done in this code.
for ielp=1:nel % loop for the total number of elements
nd(1)=nodes(ielp,1); % 1st connected node for (iel)-th element
5 nd(2)=nodes(ielp,2); % 2nd connected node for (iel)-th element
nd(3)=nodes(ielp,3); % 3rd connected node for (iel)-th element
nd(4)=nodes(ielp,4); % 4th connected node for (iel)-th element
x1=gcoord(nd(1),1); y1=gcoord(nd(1),2);% coord values of 1st node
10 x2=gcoord(nd(2),1); y2=gcoord(nd(2),2);% coord values of 2nd node
x3=gcoord(nd(3),1); y3=gcoord(nd(3),2);% coord values of 3rd node
x4=gcoord(nd(4),1); y4=gcoord(nd(4),2);% coord values of 3rd node
15 index=feeldof(nd,nnel,ndof);% extract system dofs associated with element
% Put the nodes’ coordinates in a matrix
ncoord = [x1 y1;
x2 y2;
20 x3 y3;
x4 y4];
% matrix related to shape function
A = [1 0 0 0;
25 0 0 0 1;
0 1 1 0];
% Gauss Quadrature Matrix
gmtrx = [-1/sqrt(3) -1/sqrt(3);
30 1/sqrt(3) -1/sqrt(3);
1/sqrt(3) 1/sqrt(3);
-1/sqrt(3) 1/sqrt(3)];
% Initialization
35 % Jacobian Matrix
J = zeros(2,2);
% Derivative of the
Page 26 of 29

drvtN = zeros(2,4);
% Gamma matrix
40 Gamma2 = zeros(4,4);
% element stiffness matrix
k = zeros(8,8);
%-----------------------------------
% Compute Element Stress and Strain
45 %-----------------------------------
Nu = 0; eta = 0;
drvtN = 0.25*[ eta-1 1-eta 1+eta -1-eta;
Nu-1 -1-Nu 1+Nu 1-Nu];
J = drvtN * ncoord;
50 valueJ = norm(J);
Gamma = Jˆ-1;
Gamma2(1,1) = Gamma(1,1); Gamma2(1,2) = Gamma(1,2);
55 Gamma2(4,3) = Gamma(2,1); Gamma2(4,4) = Gamma(2,2);
DrvtN = 0.25*[eta-1 0 1-eta 0 1+eta 0 -1-eta 0;
Nu-1 0 -1-Nu 0 1+Nu 0 1-Nu 0;
0 eta-1 0 1-eta 0 1+eta 0 -1-eta;
0 Nu-1 0 -1-Nu 0 1+Nu 0 1-Nu];
60 B = A * Gamma2 * DrvtN;
for i=1:edof
eldisp(i)=Displacement(index(i));
end
estrain=B*eldisp; % compute element strains
65 estress=matmtx*estrain; % compute element stresses
for i=1:3
strain(iel,i)=estrain(i); % store for each element
stress(iel,i)=estress(i); % store for each element
end
70 %-----------------------------------
% Compute Nodal Stress and Strain
%-----------------------------------
for j = 1:4
Nu = gmtrx(j,1); eta = gmtrx(j,2);
75 drvtN = 0.25*[ eta-1 1-eta 1+eta -1-eta;
Nu-1 -1-Nu 1+Nu 1-Nu];
J = drvtN * ncoord;
valueJ = det(J);
Gamma = Jˆ-1;
80 Gamma2(1,1) = Gamma(1,1); Gamma2(1,2) = Gamma(1,2);
DrvtN = 0.25*[eta-1 0 1-eta 0 1+eta 0 -1-eta 0;
85 Nu-1 0 -1-Nu 0 1+Nu 0 1-Nu 0;
0 eta-1 0 1-eta 0 1+eta 0 -1-eta;
0 Nu-1 0 -1-Nu 0 1+Nu 0 1-Nu];
B = A * Gamma2 * DrvtN;
ndisp = eldisp;
90 nstrain=B*ndisp; % compute nodal strains
Page 27 of 29

nstress=matmtx*nstrain; % compute nodal stresses
for i=1:3
nodalstrain(nd(j),i)=nstrain(i); % store for each node
nodalstress(nd(j),i)=nstress(i); % store for each node
95
end
end
end
• Finally we get the maximum values, actual values and ﬁnal results.
scalex=10000;
scaley=4/max(Displacement);
for i=2:2:length(Displacement)
5 NewX(i/2)=X(i/2)-(scalex*Displacement(i-1));
NewY(i/2)=Y(i/2)-(scaley*Displacement(i));
end
Maxdisp=max(Displacement);
Maxdisp=max(Displacement);
10 SMX=max(nodalstress);
SMX=max(SMX);
SMXnd=find(nodalstress==SMX);
SMXndno=nodes(SMXnd);
SMXndloc=gcoord(SMXndno,:);
15 SMN=min(nodalstress);
SMN=min(SMN);
SMNnd=find(nodalstress==SMN);
SMNndno=nodes(SMNnd);
SMNndloc=gcoord(SMNndno,:);
20 figure()
scatter(X,Y,’b’);
axis equal ;
grid on;
title(’Deformed + Undeformed nodes’)
25 hold on
scatter(NewX,NewY,’filled’,’k’)
scatter(SMXndloc(1),SMXndloc(2),’filled’,’r’,’d’)
scatter(SMNndloc(1),SMNndloc(2),’filled’,’g’,’d’)
legend(’Undeformed’,’Deformed’,’Maxstress’,’MinStress’)
30 %Text on plot
txt1=sprintf(’Total number of nodes = %g’,nnode);
txt2=sprintf(’Total number of elements = %g’,nel);
txt4=sprintf(’Maximum Displacement = %g’,Maxdisp);
txt3=sprintf(’%s mesh’,mesh(5:end));
35 txt5=sprintf(’Maximum Stress is %g’,SMX);
txt6=sprintf(’Minimum Stress is %g’,SMN);
text(-2,-7,txt1)
text(-2,-9,txt2)
text(-20,12,txt3)
40 text(-2,-11,txt4)
text(-2,-13,txt5)
text(-2,-15,txt6)
Page 28 of 29

45
fprintf(’nn================================================’);
fprintf(’nMaximum deformation is %g’,Maxdisp)
fprintf(’n================================================n’);
50 %% ACTUAL SOLUTION
%[U,V,sigx,sigy,tauxy]=actualsol(0,0)
scalex=10000;
scaley=4/5e-4;
for i=1:length(Node)
55 [actU(i),actV(i),actSigx(i),actSigy(i),actTauxy(i)]=actualsol(gcoord(i,1),
gcoord(i,2));
actX(i)=X(i)-(scalex*actU(i));
actY(i)=Y(i)-(scaley*actV(i));
end
60 %scatter(actX,actY);
axis equal ;
grid on;
max(actV);
max(NewX);
65 max(actSigx)
max(actSigy)
max(actTauxy)
hold off
References
[1] Autodesk. How to Perform a Mesh Convergence Study. https://knowledge.autodesk.
com/support/simulation-mechanical/troubleshooting/caas/sfdcarticles/
sfdcarticles/How-to-Perform-a-Mesh-Convergence-Study.html, 2015. [Online; ac-
cessed 11-December-2016].
[2] Bethany Nine. How to Implement a Mesh Reﬁnement Study. https://www.comsol.com/blogs/
how-to-implement-mesh-refinement-study/, 2013. [Online; accessed 11-December-2016].
[3] University of Rome. Finite Elements for 2-D Problems-General Formula for the Stiﬀness Matrix. http:
//www.uniroma2.it/didattica/TCM/deposito/2-D_elements.pdf, 2016. [Online; accessed
10-December-2016].
[4] David Roylance. How to Perform a Mesh Convergence Study. http://web.mit.edu/course/3/3.
11/www/modules/bstress.pdf, 2000. [Online; accessed 11-December-2016].
[5] Boulder University of Colorado. FEM - Chapter 17 Isoparametric Quadrilaterals. http://www.
colorado.edu/engineering/CAS/courses.d/IFEM.d/IFEM.Ch17.d/IFEM.Ch17.pdf, 2016.
[Online; accessed 10-December-2016].
Page 29 of 29

FINAL PROJECT

More Related Content

Viewers also liked (10)

Similar to FINAL PROJECT (20)

FINAL PROJECT