The document describes the steps to create a finite element model in ABAQUS. It involves pre-processing tasks like creating individual parts for the model, assigning material properties, assembling parts, applying loads and boundary conditions, and generating a mesh. Specific steps are provided to create each of the five parts that make up the model - the ceramic, cap, solder, copper, and PC board. Detailed instructions are given on creating the geometry of each part using the part module in ABAQUS. The document also outlines other pre-processing tasks like defining interactions and jobs before solving the model.

1. Finite-Element Project
ABAQUS Tutorial
Mohith Manjunath
July 30, 2009
1

2. Contents
1 Introduction 3
2 Problem Description 3
3 Pre-processing 4
3.1 Part . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 5
3.1.1 Ceramic . . . . . . . . . . . . . . . . . . . . . . . . . . 5
3.1.2 Cap . . . . . . . . . . . . . . . . . . . . . . . . . . . . 6
3.1.3 Solder . . . . . . . . . . . . . . . . . . . . . . . . . . . 10
3.1.4 Copper . . . . . . . . . . . . . . . . . . . . . . . . . . . 16
3.1.5 PC Board . . . . . . . . . . . . . . . . . . . . . . . . . 18
3.2 Property . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 19
3.2.1 Assign Sections . . . . . . . . . . . . . . . . . . . . . . 20
3.3 Assembly . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 21
3.4 Step . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 22
3.5 Interaction . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 24
3.6 Load . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 24
3.7 Mesh . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 26
3.7.1 Partitioning . . . . . . . . . . . . . . . . . . . . . . . . 26
3.7.2 Meshing . . . . . . . . . . . . . . . . . . . . . . . . . . 37
3.8 Job . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 44
4 Postprocessing 45
4.1 Visualization . . . . . . . . . . . . . . . . . . . . . . . . . . . 45
4.1.1 Selecting the field output to display . . . . . . . . . . . 45
4.1.2 Plotting . . . . . . . . . . . . . . . . . . . . . . . . . . 45
2

3. 1 Introduction
ABAQUS is a finite-element analysis software. Abaqus/CAE provides a pre-
processing and postprocessing environment for the analysis of models. It is
used in a wide range of industries like automotive, aerospace etc., and also is
extensively used in academic and research institutions due to its capability
to address non-linear problems. The Abaqus interface is shown in figure 1.
Figure 1: Abaqus Interface
Get familiar with the icons in the tool bar especially the zoom icons which
are absolutely necessary in the modeling process.
2 Problem Description
Lifetime equations for micro-electronic solder needs to be predicted in order
to guarantee reliable in-field operation of micro-electronic components. Typ-
ical micro-electronic solder is shown in figure 2. The solder joints are under
thermo-mechanical stress due to the change in temperature during in-field
operation. Basically, there is a mismatch in coefficient of thermal expansion
between boards and components. This might lead to thermal fatigue failures
3

4. and can be very catastrophic. Figure 3 shows the failure of solder joint after
many cycles in operation.
Figure 2: Microelectronic Solder
Figure 3: Microelectronic Solder after 3000 cycles of operation
3 Pre-processing
Pre-processing is the initial phase of a finite element analysis program. This
phase includes various modules for creating a model, defining material prop-
erties, specifying boundary conditions and external loads and meshing the
assembly of the model.
1. Start Abaqus CAE.
2. Click Create Model Database to create a new model.
3. The previous chapter explains the different sections of Abaqus.
4. Continue with the next section for creating various parts of the model.
4

5. 3.1 Part
Part module is used to build different parts of the model. So, for convenience,
divide the whole model into various parts and create each part using this
module. Later all the parts can be assembled to form the entire model.
Here, the model is divided into five parts - Ceramic, Cap, Solder, Copper
and PC Board. What follows now is a step-by-step procedure to create each
of these parts.
3.1.1 Ceramic
1. In the menu bar, click Part -> Create. Enter the name Ceramic and
select 3D, Deformable, Solid->Extrusion and enter Approximate size
as 10 (See Figure 4).
Figure 4: Create Ceramic Part
2. Click Rectangle icon to create a rectangle. On the grid draw an arbi-
trary rectangle. Click Add Dimension tool and click the left side and
5

6. left-click to enter the dimension. Enter 0.25 and press enter. Select
the bottom side, left-click and enter 1.0 for the dimension and press
enter. Cancel procedure by pressing the ”X” mark in the ”prompt
area”(remember to do this every time you want to come out of a pro-
cedure and you can also press Esc key to exit an operation).
3. At the bottom click Done (Sketch the section for the solid extrusion).
Enter depth of 0.625 and click OK.
4. From the menu bar, click Shape -> Blend -> Round/Fillet. Select
the five edges as shown in Figure 5(Multiple edges can be selected by
holding shift key). Click Done. Enter radius of 0.03. Click Done.
Figure 5: For ceramic - Select the edges as shown
3.1.2 Cap
1. In the menu bar, click Part -> Create. Enter the name Cap and select
3D, Deformable, Solid->Extrusion and enter Approximate size as 10.
2. Click Rectangle icon to create a rectangle. On the grid draw an arbi-
trary rectangle. Click Add Dimension tool and click the left side and
left-click to enter the dimension. Enter 0.25 and press enter. Select the
bottom side, left-click and enter 0.3 for the dimension and press enter.
6

7. 3. In the menu bar, click Add -> Fillet. Enter fillet radius as 0.03 and
press enter. Now, select the top and right side edges of the rectangle.
Fillet has been created.
4. Click Add -> Point and create three points, one on the top left corner
of the rectangle and two on the corners of the arc of the fillet(See Figure
6). Click Edit -> Transform -> Translate and click Copy. Now, select
the points 1 and 2(holding shift key) and click Done. Enter 0,0 for the
start position, press enter and then enter 0,0.005 for the endpoint and
press enter again. Repeat the same procedure for point 3 and enter
0.005,0 for the endpoint. Repeat the same procedure for point 1 and
enter 0.135,0.01 for the endpoint. Repeat the same procedure for point
3 and enter 0,-0.095 for the endpoint. Repeat the same procedure for
point 3 and enter 0.01,-0.095 for the endpoint.
Figure 6: Section sketch for cap - Three points created
5. See Figure 7. Connect points 1 and 4 using Add -> Line -> Connected
Lines. Also, draw a line through points 8 and 9 as shown in the figure.
Suppose, while performing any of these operations if a point vanishes
then you have to undo and zoom in to the area and complete the
operation(keep this in mind). Now, click Add -> Spline and draw a
spline through the points 4, 5 and 6(you might have to zoom in a bit).
Repeat the same procedure for the points 7 and 8(first click point 7
then click somewhere in the middle(as shown) and then click point 8).
Now click Add -> Arc -> Center/Endpoints. Select the center of the
circle(for the arc) and then select the two endpoints of the arc.
7

8. Figure 7: Create spline through the points 4-5-6 and 7-8
6. Click Edit -> Split, select the right edge of the rectangle and then the
horizontal line passing through the center of it. Now, click Edit ->
Delete and select the left edge, bottom edge and the bottom half of the
right edge(hold shift while selecting all three). Click Done. Now, click
Edit -> Transform -> Mirror and click Copy. Then, pick the center
horizontal line as the mirror line. Now select all the entities above the
mirror line. Click Done. A mirror image is created. Now delete the
center horizontal line. Click Done to exit the section sketch. Enter
0.595 for depth and press OK.
7. In the menu bar, click Shape -> Solid -> Revolve. Select the plane
section(C-Section) at the back(see figure 8) of the cap. Select one of
the edges in the middle portion(vertical line in the C-Section). Section
sketch appears(inverted C). Now click Edit -> Transform -> Translate
and click Copy. Select all the edges in the middle portion and also
the arcs at the top and bottom. Click Done. Enter 0,0 for the start
position, press enter and then enter 0.1,0 for the endpoint and press
enter again. In the section which was copied to the right, draw straight
lines at top and bottom ends to make it a closed figure. Click Edit
8

9. Figure 8: Cap - After the section sketch has been extruded
-> Transform -> Translate and click Move. Now select all the entities
which were just copied(closed figure) and click Done. Enter 0,0 for the
start position, press enter and then enter -0.1,0 for the endpoint and
press enter again. Now, click Add -> Construction -> Vertical and
click on one of the centers of the arcs. Cancel the operation(X mark).
Click Done to exit the section sketch. Enter angle as 90 degrees and
press OK.
8. In the menu bar, click Shape -> Solid -> Revolve. Select the top
section. Select the edge on the right. Section sketch appears. Now
click Edit -> Transform -> Translate and click Copy. Select all the
edges in the top portion(3 edges). Click Done. Enter 0,0 for the start
position, press enter and then enter 0,0.1 for the endpoint and press
enter again. Click Edit -> Transform -> Translate and click Move.
Now select all the entities which were just copied(closed figure) and
click Done. Enter 0,0 for the start position, press enter and then enter
0,-0.1 for the endpoint and press enter again. In the section which was
copied, draw a straight line at the left end to make it a closed figure.
Now, click Add -> Construction -> Horizontal and click on the center
of the arcs(top). Click Done to exit the section sketch. Enter angle as
90 and press OK. Repeat the above procedure for the bottom section.
Finally, it should look like as shown in figure 6.
9. Click Shape -> Wire -> Sketch. Select the face marked one(the face
facing east) in the figure 6 and select one of the right edges. Using
9

10. Figure 9: Cap - After the edges have been revolved
connected lines tool draw the rectangle as shown in figure 7(wire sketch
number 1). Now, click Shape -> Wire -> Point to point, select Chained
wires and click Add. All the points will be shown. Now select two points
at a time and complete the crooked rectangle number 2 as shown in
figure 7. Now, click Shape -> Solid -> Loft and click Insert Before.
Select all the edges of plane 3(six edges to make it a closed loop) in
figure 7. Then, click Insert After and select all the edges in the plane 1.
Now, click the tab Transition and select method as Select path. click
Add. Now, select the edges one by one going from plane 3 to plane
1(two edges in plane 2, 4 and 5). Click OK when done. See figure 8.
3.1.3 Solder
1. In the menu bar, click Part -> Create. Enter the name Solder and
select 3D, Deformable, Solid->Extrusion and enter Approximate size
as 10.
2. Click Rectangle icon to create a rectangle. On the grid draw an arbi-
trary rectangle. Click Add Dimension tool and click the left edge and
left-click to enter the dimension. Enter 0.6 and press enter. Select the
bottom edge, left-click and enter 0.6 for the dimension and press enter.
3. At the bottom click Done (Sketch the section for the solid extrusion).
Enter depth of 1.0 and click OK.
4. In the context bar, click Module -> Assembly. Now, click Instance
10

11. Figure 10: Cap - Creating wires
Figure 11: Cap - Part created
-> Create. Select Ceramic, Cap and Solder and toggle on auto-offset
from other instances and click OK. Now, click Constraint -> Coincident
Point and select the center of the top arc in the ceramic and the cor-
responding point in the cap so that they fit together(figure 12). Click
Constraint -> Coincident Point and select the two points as shown in
the figure. Now, click Instance -> Translate and select the solder in-
stance. Click Done. Enter 0,0,0 for starting point and -0.27,0,0 for the
11

12. end point. Click Yes.
Figure 12: Solder - Coincident points
Figure 13: Solder - Cut the geometry of cap in the rectangular solid
5. Click Instance -> Merge/Cut. Give part name as Solder-1. Select Cut
geometry and click Continue. Now, select the solder for the instance
to be cut and select the other two(ceramic and cap) for the instances
that will make the cut(holding down the shift key). Click Done. Select
Part -> Solder-1 in the context bar. See figure 14.
6. Click Shape -> Cut -> Extrude. Select the front facing plane and then
the right edge. Now, click Add -> Point and click on the top-left point.
Click Edit -> Transform -> Translate and click Copy. Select the point
12

13. Figure 14: Solder - After using Merge/Cut instance
that was just created and enter 0,0 for start point and 0,-0.02 for the
end point. Now, draw a rectangle(covering the entire area towards the
bottom and towards the right) with the copied point as its top-left
corner. Click done and then click OK in the window that opens.
7. Click Shape -> Cut -> Extrude. Select the front facing plane and then
the right edge. Now, draw a spline(Add -> Spline) as shown in figure
15 and make it a closed figure by drawing lines 1,2 and 3. Click Done.
In the window that opens select type as blind and enter depth as 0.595
and click OK.
8. Click Shape -> Cut -> Extrude. Select the left facing plane and then
the right edge. Now, draw a spline(Add -> Spline) as shown in figure
16 and make it a closed figure by drawing lines 1,2 and 3. Click Done.
In the window that opens select type as blind and enter depth as 0.270
and click OK. See figure 17.
9. Click Tools -> Partition and select Face -> Sketch. Select the bottom
face. Click Done and select the edge which is on the right. Now, draw
a spline as shown in figure 18 and click Done.
10. Click Shape -> Cut -> Loft. Click Insert before. Now, select the
edges holding down shift button as shown in figure 19 and click Done.
Then, click Insert after and select the edges as shown in figure 20 and
click Done. Now, click the tab Transition and select method as Select
13

14. Figure 15: Solder - Front view, section sketch to extrude solid
Figure 16: Solder - Side view, section sketch to extrude solid
Figure 17: Solder - Top view, after the extrusion on both sides
path. Click Add. Select the top curve and the bottom curve(one after
another, by clicking add) which was created using partition method
and click OK. Now, remove the part that got cut by using Shape ->
Cut -> Extrude and by selecting any face and any edge draw a closed
14

15. Figure 18: Solder - Bottom view, section sketch
figure around it. Click Done and click OK. Finally, the solder should
look something like figure 21.
Figure 19: Solder - Insert before operation(select the edges as shown)
11. Click Tools -> Geometry Repair and select Edge -> Remove redundant
entities. Now, select the edges(holding shift) as shown in figure 22 and
click Done. The edges are now merged into one.
15

16. Figure 20: Solder - Insert after operation(select the edges as shown)
Figure 21: Solder - Part created
3.1.4 Copper
1. In the menu bar, click Part -> Create. Enter the name Copper and
select 3D, Deformable, Solid->Extrusion and enter Approximate size
as 10.
16

17. Figure 22: Remove redundant entities on the edge shown
2. Click Rectangle icon to create a rectangle. On the grid draw an arbi-
trary rectangle. Click Add Dimension tool and click the left edge and
left-click to enter the dimension. Enter 0.06 and press enter. Select
the bottom edge, left-click and enter 0.63 for the dimension and press
enter.
3. At the bottom click Done (Sketch the section for the solid extrusion).
Enter depth of 0.8 and click OK. See figure 23.
Figure 23: Copper - Part created
17

18. 3.1.5 PC Board
1. In the menu bar, click Part -> Create. Enter the name PC Board and
select 3D, Deformable, Solid->Extrusion and enter Approximate size
as 10.
2. Click Rectangle icon to create a rectangle. On the grid draw an arbi-
trary rectangle. Click Add Dimension tool and click the left edge and
left-click to enter the dimension. Enter 1.6 and press enter. Select the
bottom edge, left-click and enter 3.5 for the dimension and press enter.
3. At the bottom click Done (Sketch the section for the solid extrusion).
Enter depth of 2 and click OK. See figure 24.
Figure 24: PC Board - Part created
18

19. 3.2 Property
Property module is used to define properties of various materials used in the
model. Then, sections are created and materials are assigned to each section.
This section of creating the properties of materials can be done later also, if
required to do so.
1. In the context bar click Module -> Property to enter into property
module.
2. In the menu bar, click Material -> Manager.
3. A new window opens. Now click the button Create to create new
material.
4. Enter the material name Ceramic and click Mechanical -> Elasticity
-> Elastic. Now, enter the value 220000 MPa in the box below Young’s
Modulus and 0.3 for Poisson’s Ratio. Click Mechanical -> Expansion
and enter 8E-6 for Expansion Coeff alpha. Click OK.
5. Click Create. Enter the material name Cap and click Mechanical -
> Elasticity -> Elastic. Now, enter the value 120000 MPa in the box
below Young’s Modulus and 0.31 for Poisson’s Ratio. Click Mechanical
-> Expansion and enter 1.6E-5 for Expansion Coeff alpha. Click OK.
6. Click Create. Enter the material name Solder-SnAgCu and click Me-
chanical -> Elasticity -> Elastic. Now, enter the value 35000 MPa in
the box below Young’s Modulus and 0.34 for Poisson’s Ratio. Click
Mechanical -> Expansion and enter 2.3E-5 for Expansion Coeff alpha.
Click Mechanical -> Plasticity -> Creep. In the drop-down menu for
Law select Hyperbolic-Sine and enter the values shown in the table
below. Hyperbolic-sine law is given by:
−Q
n
ε = C sinh(aσ )e RT
˙ (1)
Where ε is the strain rate, C is the power law multiplier, a the hyper-
˙
bolic law multiplier, n the stress order, Q the activation energy and R
the universal gas constant. The values of these parameters have been
taken from reference 2.
Power Law Hyperb Law Eq Stress Activation Universal Gas
Multiplier(/s) Multiplier(/MPa) Order Energy(J/mol/K) Const(J/mol/K)
4.41E5 0.005 4.2 4.5E4 8.314
19

20. Click OK.
7. Click Create. Enter the material name Copper and click Mechanical
-> Elasticity -> Elastic. Now, enter the value 90000 MPa in the box
below Young’s Modulus and 0.32 for Poisson’s Ratio. Click Mechanical
-> Expansion and enter 1.65E-5 for Expansion Coeff alpha. Click OK.
8. Click Create. Enter the material name FR4-PC Board and click Me-
chanical -> Elasticity -> Elastic. In the drop-down menu for Type se-
lect Engineering Constants and tick the checkbox next to Use temperature-
dependent data and enter the following values. Directions 1,2 and 3
refer to the X, Y and Z directions respectively in the material. The
values have been taken from reference 3.
E1(MPa) E2(MPa) E3(MPa) Nu12 Nu13 Nu23
19300 8300 19300 0.4 0.15 0.4
G12(MPa) G13(MPa) G23(MPa) Temp(K)
8400 8400 8400 293
Click Mechanical -> Expansion and select Type as Orthotropic and
enter the following values.
alpha11 alpha22 alpha33
1.5E-5 8.4E-5 1.5E-5
Click OK.
3.2.1 Assign Sections
After the materials have been creates we need to assign these materials to
the parts which were previously created.
1. Click Section -> Create. Enter name as Ceramic. Select Solid ->
Homogenous and click Continue. From the material list select Ceramic
and click OK.
2. Click Section -> Create. Enter name as Cap. Select Solid -> Homoge-
nous and click Continue. From the material list select Cap and click
OK.
3. Click Section -> Create. Enter name as Solder. Select Solid -> Ho-
mogenous and click Continue. From the material list select Solder-
SnAgCu and click OK.
20

21. 4. Click Section -> Create. Enter name as Copper. Select Solid -> Ho-
mogenous and click Continue. From the material list select Copper and
click OK.
5. Click Section -> Create. Enter name as PC Board. Select Solid ->
Homogenous and click Continue. From the material list select FR4-PC
Board and click OK.
6. In the context bar select part as Ceramic. Click Assign -> Section.
Select the ceramic by clicking on it and click Done. In the window that
opens, select Ceramic from the list and click OK.
7. In the context bar select part as Cap. Click Assign -> Section. Select
the cap by clicking on it and click Done. In the window that opens,
select Cap from the list and click OK.
8. In the context bar select part as Solder-1. Click Assign -> Section.
Select the solder by clicking on it and click Done. In the window that
opens, select Solder from the list and click OK.
9. In the context bar select part as Copper. Click Assign -> Section.
Select the copper by clicking on it and click Done. In the window that
opens, select Copper from the list and click OK.
10. In the context bar select part as PC Board. Click Assign -> Section.
Select the PC Board by clicking on it and click Done. In the window
that opens, select PC Board from the list and click OK.
Now, the sections have been assigned to the parts with corresponding mate-
rial.
3.3 Assembly
In this module, all the parts created earlier can be put together(assembly)
to get the required model. After doing this we can apply the necessary
constraints and loads on the assembly.
1. Select Module -> Assembly. Click Instance -> Create. Select Ceramic
and Cap holding down Ctrl. Now, click Constraint -> Coincident point
and select the center of the top arc in the ceramic and the corresponding
point in the cap so that they fit together.
2. Click Instance -> Create, select Solder-1 and toggle on auto-offset from
other instances. Repeat the same procedure as before to make the
solder fit right under the cap. See figure 21.
21

22. Figure 25: Three instances assembled
3. Click Instance -> Create, select Copper and toggle on auto-offset from
other instances. Now, click Constraint -> Coincident point and select
the top-left corner of copper and bottom-left corner of solder.
4. Click Instance -> Create, select PC Board and toggle on auto-offset
from other instances. Now, click Constraint -> Coincident point and
select the top-left corner of PC Board and bottom-left corner of copper.
Then, click Instance -> Translate and select PC Board instance. Enter
0,0,0 for the start point and -0.7,0,0 for the end point and click yes and
then OK. Now, all the instances have been assembled and take a look
at the assembled model by rotating the figure. See figure 26.
5. Click Instance -> Merge/Cut. Enter part name as Full-Model, select
Merge -> Geometry and select Retain in intersecting boundaries section
and click Continue. Now, select all the instances and click Done. All
the instances are now merged and a new part by name Full-Model has
been created.
3.4 Step
This module is used to perform many tasks, mainly to create analysis steps
and specify output requests.
1. Select Module -> Step. Click Step -> Create. Type Extra-Step for
name and select Procedure type -> General -> Visco and click Con-
tinue. In the description field enter Abkhlung and enter time period as
30. Go to incrementation tab and enter the following. Type:Automatic,
22

23. Figure 26: All instances(Ceramic, Cap and Solder) assembled
Maximum number of increments:10000, Increment size:Initial=0.5, Min=1E-
6, Max=30, Tolerance=0.005 and Integration:Explicit/Implicit. Go to
Other tab and select Iterative method and select ramp linearly over
step. Click OK.
2. Select Module -> Step. Click Step -> Create. Type Step-1-Abkhlung
for name and select Procedure type -> General -> Visco and click Con-
tinue. Enter time period as 10. Go to incrementation tab and enter the
following. Type:Automatic, Maximum number of increments:10000,
Increment size:Initial=0.5, Min=1E-6, Max=10, Tolerance=0.005 and
Integration:Explicit/Implicit. Go to Other tab and select Iterative
method and select ramp linearly over step. Click OK.
3. Select Module -> Step. Click Step -> Create. Type Step-2-Halten-
40C for name and select Procedure type -> General -> Visco and
click Continue. Enter time period as 900. Go to incrementation tab
and enter the following. Type:Automatic, Maximum number of incre-
ments:10000, Increment size:Initial=0.5, Min=1E-6, Max=900, Toler-
ance=0.005 and Integration:Explicit/Implicit. Go to Other tab and
select Iterative method and select ramp linearly over step. Click OK.
23

24. 4. Select Module -> Step. Click Step -> Create. Type Step-3-Aufheizen
for name and select Procedure type -> General -> Visco and click Con-
tinue. Enter time period as 10. Go to incrementation tab and enter the
following. Type:Automatic, Maximum number of increments:10000,
Increment size:Initial=0.5, Min=1E-6, Max=10, Tolerance=0.005 and
Integration:Explicit/Implicit. Go to Other tab and select Iterative
method and select ramp linearly over step. Click OK.
5. Select Module -> Step. Click Step -> Create. Type Step-4-Halten-
auf-125C for name and select Procedure type -> General -> Visco and
click Continue. Enter time period as 900. Go to incrementation tab
and enter the following. Type:Automatic, Maximum number of incre-
ments:10000, Increment size:Initial=0.5, Min=1E-6, Max=900, Toler-
ance=0.005 and Integration:Explicit/Implicit. Go to Other tab and
select Iterative method and select ramp linearly over step. Click OK.
3.5 Interaction
As the name suggests, this module is used to define various interactions
within the model or interactions between regions of the model and its sur-
roundings. The interactions can be mechanical or/and thermal. Analysis
constraints can also be applied between regions of the model.
3.6 Load
Load module is used to define and manage various conditions like loads,
boundary conditions and predefined fields.
1. Select Module -> Load. Click BC -> Create. Select Displacement/Rotation
and click Continue. Select the whole of left section(plane) and hold
down control key to deselect the bottom-left point(see figure 27). Click
Done and then just tick the box next to U1 to constrain that degree of
freedom.
2. Click BC -> Create. Select Displacement/Rotation and click Continue.
Select the corner point which was previously not selected and click
Done and then just tick the box next to U2 to constrain that degree of
freedom.
3. Click BC -> Create. Select Displacement/Rotation and click Continue.
Select the whole of front section(plane X-Y)(for easier selection click
the icon in the ”prompt area” and select faces from the list and then
24

25. Figure 27: Boundary Condition on the left face - U1 constrained
select ”by angle” from the list in the prompt area) and click Done and
then just tick the box next to U3 to constrain that degree of freedom.
Figure 28: Boundary Condition on the front face - U3 constrained
4. Click Predefined Field -> Create. Select Other -> Temperature and
click Continue. Select the whole assembly and click Done and then
enter 421 for the magnitude of temperature. Click OK.
25

26. Figure 29: Predefined Field - Initial temperature for the entire model
3.7 Mesh
This is one of the most important modules since accuracy of the results
will depend on the meshing of the assemblies. This module can be used to
generate meshes and even verify them.
3.7.1 Partitioning
1. Select Part -> Full-Model from the list in the left window. Select
Module -> Mesh. See figure 30.
2. Click Tools -> Partition. Select Cell -> Extend face, select the entire
model and click Done. Select the face as shown in the figure 31 and
click Create partition. A partition should be created and it should
turn green(structured mesh). Repeat the same procedure for the faces
as shown in the figure 32 and 33 and now entire PC Board should turn
green(figure 33).
3. Select Cell -> Extrude/Sweep edges, select the entire model and the
edge 1(choose by edge angle) as shown in figure 34. Click Done. Select
Extrude Along Direction and select the edge 2(pointing down) as shown
in the same figure. Check for direction and flip if required. Click Create
partition. See figure 35.
26

27. Figure 30: Partitions are required for the whole model(for orange colored
ones, it is mandatory)
Figure 31: Partition - Extend face
27

28. Figure 32: Partition - Extend face
Figure 33: Partition - Extend face
28

29. Figure 34: Partition - Extrude edges
29

30. Figure 35: Partition - The edges have been extruded
30

31. 4. Select Cell -> Define cutting plane, select the entire model and click
Done. Then, click Point and Normal. And select point and normal as
shown in the figure 36 and click Create partition. See figure 37.
Figure 36: Partition - Select the point as pointed by the arrow and the line
in pink
5. Select Cell -> Define cutting plane, select the entire model and click
Done. Then, click Point and Normal. And select point and normal as
shown in the figure 38 and click Create partition. See figure 39.
6. Select Cell -> Define cutting plane, select the entire model and click
Done. Then, click Point and Normal. And select point and normal as
shown in the figure 40 and click Create partition. At the end of this
operation, the model should look similar to figure 41.
31

32. Figure 37: Partition - At the end of previous operation
32

33. Figure 38: Partition - Select the point as pointed by the arrow and the line
in pink
Figure 39: Partition - At the end of previous operation
33

34. Figure 40: Partition - Select the point as pointed by the arrow and the line
in pink
Figure 41: Partition - At the end of previous operation
34

35. 7. Select Cell -> Define cutting plane, select the entire model and click
Done. Then, click Point and Normal. And select point and normal as
shown in the figure 42 and click Create partition. At the end of this
operation, the model should look similar to figure 43.
Figure 42: Partition - Select the point as pointed by the arrow and the line
in pink
Figure 43: Partition - At the end of previous operation
35

36. 8. Select Cell -> Define cutting plane, select the entire model and click
Done. Then, click Point and Normal. And select point and normal as
shown in the figure 44 and click Create partition. At the end of this
operation, the model should look similar to figure 45.
Figure 44: Partition - Select the point as pointed by the arrow and the line
in pink
Figure 45: Partitioning done - Everything is green!
36

37. Now, you can proceed to the meshing section but it is suggested that you
try different partitioning methods and analyze the results. In the process
you will be able to learn how to partition any complicated geometry with
minimum partitioning.
3.7.2 Meshing
1. Click Mesh -> Controls. Select the entire model, click Done and select
Structured from the list and click OK.
2. Click Mesh -> Element Type. Select the entire model, accept the
default options and click OK.
3. Click Seed -> Part. In the approximate global size field enter 0.01 and
click OK.
4. Click Seed -> Edge Biased. Switch to wire-frame view. Select the
edges(click near the left end of the edges) as shown in the figure 46 and
click Done. Enter bias ratio as 10 and number of elements as 18.
Figure 46: Edges biased towards the solder(left)
5. Click Seed -> Edge Biased. Select the edges(click near the top end of
the edges) as shown in the figure 47 and click Done. Enter bias ratio
as 10 and number of elements as 18.
37

38. Figure 47: Edges biased towards the solder(top)
38

39. 6. Click Seed -> Edge Biased. Select the edges(click near the right end of
the edges) as shown in the figure 48 and click Done. Enter bias ratio
as 10 and number of elements as 8.
Figure 48: Edges biased towards the solder(right)
7. Click Seed -> Edge Biased. Select the edges(click near the bottom end
of the edges) as shown in the figure 49 and click Done. Enter bias ratio
as 10 and number of elements as 16.
Figure 49: Edges biased(Top view) towards the solder
39

40. 8. Click Seed -> Edge Biased. Select the edges(click near the top end of
the edges) as shown in the figure 50 and click Done. Enter bias ratio
as 10 and number of elements as 8.
Figure 50: Edges biased(Top view) towards the solder
9. Now, click the create display group icon, select ceramic from the list
of sets and click replace. Click Seed -> Edge By Number. Select the
edges as shown in the figure 51 and enter 14 for the number of elements.
Figure 51: Ceramic - ”Edge by number” operation for the edges shown
10. Click Mesh -> Controls and select all the cells except the ones in the
corner edge(see figure 52). Click Done and in the window that opens
select Sweep and click OK. Then, click Mesh -> Region and select all
the cells(the whole ceramic) and click Done. See figure 53.
40

41. Figure 52: Ceramic - Select all except the cells in green
Figure 53: Ceramic Mesh
11. Now, click the create display group icon, select cap from the list of sets
and click replace. Click Mesh -> Region and select all the cells and
click OK.
41

42. 12. Now, click the create display group icon, select solder from the list of
sets and click replace. Click Seed -> Edge By Number. Select the edges
as shown in the figure 54 and enter 14 for the number of elements.
Figure 54: Solder - ”Edge by number” operation for the edges shown
13. Click Mesh -> Controls and select all the cells except the ones in the
corner edge(see figure 55). Click Done and in the window that opens
select Sweep and click OK. Then, click Mesh -> Region and select all
the cells(the whole solder) and click Done. See figure 56.
Figure 55: Solder - Select the cells as shown
42

43. Figure 56: Solder Mesh
14. Now, click the create display group icon, select PC Board from the list
of sets and click replace. Click Mesh -> Region and select all the cells
and click OK.
15. Now, click the create display group icon, select copper from the list of
sets and click replace. Click Mesh -> Controls and select all the cells.
Click Done and in the window that opens select Sweep and click OK.
Then, click Mesh -> Region and select all the cells and click OK.
Figure 57: Complete Mesh of the model
43

44. It should be noted that the mesh created above is not a perfect mesh.
There are quite a few dark patches which should not have been there.
I would suggest, since you have gained a little experience in Abaqus
now, you to experiment with the mesh by playing around with the mesh
controls, seeding etc., so that you will become familiar with different
kinds of meshes. Then, you can try to create a better mesh than this
one and be proud of doing it.
3.8 Job
Job module can be used to create and manage analysis jobs and submit them
for analysis.
1. Select Module -> Job.
2. Click Job -> Manager. In the window that opens, click Create. Enter
job name as 3DSolder and click Continue. Now, just explore all the
tabs and leave the default options as it is. Click OK. Now, select the
current job and click Submit. After the job has been submitted, the
analysis can be monitored by clicking Monitor.
44

45. 4 Postprocessing
The results generated from the analysis can be enormous so it requires ad-
ditional processing which is termed postprocessing.
4.1 Visualization
Here the model can be viewed and various plots can be generated.
4.1.1 Selecting the field output to display
1. Select Result -> Field Output from the main menu bar. Here, one of
the various parameters like CEEQ, PEEQ, stress components etc. can
be selected. Click OK.
4.1.2 Plotting
1. To plot undeformed shape select Plot -> Undeformed Shape from the
main menu bar.
2. To plot deformed shape select Plot -> Deformed Shape from the main
menu bar.
Here, not all the modules of postprocessing are explained. You can explore
different modules and try to generate plots for different parameters and get
meaningful results out of them.
45

46. Bibliography
1. Abaqus 6.7-4 Documentation.
2. Improving Solder Joint Reliability of WLP by Means of a Compliant
Layer , Lee Hun Kwang et al., International Electronic Manufacturing
Technology 2006
3. FEM-Simulationen und Zuverlssigkeit von Advanced Packages LWF,
Uni Paderborn, IFM, TU Berlin
46