Finite Element Project Abaqus Tutorial

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

1

Contents 1 Introduction

3

2 Problem Description

3

3 Pre-processing 3.1 Part . . . . . . . . . . 3.1.1 Ceramic . . . . 3.1.2 Cap . . . . . . 3.1.3 Solder . . . . . 3.1.4 Copper . . . . . 3.1.5 PC Board . . . 3.2 Property . . . . . . . . 3.2.1 Assign Sections 3.3 Assembly . . . . . . . 3.4 Step . . . . . . . . . . 3.5 Interaction . . . . . . . 3.6 Load . . . . . . . . . . 3.7 Mesh . . . . . . . . . . 3.7.1 Partitioning . . 3.7.2 Meshing . . . . 3.8 Job . . . . . . . . . . .

. . . . . . . . . . . . . . . .

. . . . . . . . . . . . . . . .

. . . . . . . . . . . . . . . .

. . . . . . . . . . . . . . . .

. . . . . . . . . . . . . . . .

. . . . . . . . . . . . . . . .

. . . . . . . . . . . . . . . .

. . . . . . . . . . . . . . . .

. . . . . . . . . . . . . . . .

. . . . . . . . . . . . . . . .

. . . . . . . . . . . . . . . .

. . . . . . . . . . . . . . . .

. . . . . . . . . . . . . . . .

. . . . . . . . . . . . . . . .

. . . . . . . . . . . . . . . .

. . . . . . . . . . . . . . . .

. . . . . . . . . . . . . . . .

. . . . . . . . . . . . . . . .

. . . . . . . . . . . . . . . .

. . . . . . . . . . . . . . . .

. . . . . . . . . . . . . . . .

. . . . . . . . . . . . . . . .

4 5 5 6 10 16 18 19 20 21 22 24 24 26 26 37 44

4 Postprocessing 45 4.1 Visualization . . . . . . . . . . . . . . . . . . . . . . . . . . . 45 4.1.1 Selecting the field output to display . . . . . . . . . . . 45 4.1.2 Plotting . . . . . . . . . . . . . . . . . . . . . . . . . . 45

2

1

Introduction

ABAQUS is a finite-element analysis software. Abaqus/CAE provides a preprocessing 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. Typical 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

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 properties, 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

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 arbitrary rectangle. Click Add Dimension tool and click the left side and 5

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 procedure 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 arbitrary 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

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

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

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

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 arbitrary 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

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 corresponding 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 instance. Click Done. Enter 0,0,0 for starting point and -0.27,0,0 for the

11

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

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

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

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

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

Figure 22: Remove redundant entities on the edge shown 2. Click Rectangle icon to create a rectangle. On the grid draw an arbitrary 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

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 arbitrary 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

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 Mechanical -> 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 ε˙ = C sinh(aσ )e RT n

(1)

Where ε˙ is the strain rate, C is the power law multiplier, a the hyperbolic 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 Multiplier(/s) Multiplier(/MPa) Order 4.41E5 0.005 4.2 19

Activation Universal Gas Energy(J/mol/K) Const(J/mol/K) 4.5E4 8.314

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 Mechanical -> Elasticity -> Elastic. In the drop-down menu for Type select Engineering Constants and tick the checkbox next to Use temperaturedependent 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 -> Homogenous and click Continue. From the material list select Cap and click OK. 3. Click Section -> Create. Enter name as Solder. Select Solid -> Homogenous and click Continue. From the material list select SolderSnAgCu and click OK. 20

4. Click Section -> Create. Enter name as Copper. Select Solid -> Homogenous 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 material.

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

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 Continue. In the description field enter Abkhlung and enter time period as 30. Go to incrementation tab and enter the following. Type:Automatic,

22

Figure 26: All instances(Ceramic, Cap and Solder) assembled Maximum number of increments:10000, Increment size:Initial=0.5, Min=1E6, 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 Continue. 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-Halten40C 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 increments:10000, Increment size:Initial=0.5, Min=1E-6, Max=900, Tolerance=0.005 and Integration:Explicit/Implicit. Go to Other tab and select Iterative method and select ramp linearly over step. Click OK. 23

4. Select Module -> Step. Click Step -> Create. Type Step-3-Aufheizen for name and select Procedure type -> General -> Visco and click Continue. 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-Haltenauf-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 increments:10000, Increment size:Initial=0.5, Min=1E-6, Max=900, Tolerance=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 surroundings. 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

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

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

Figure 30: Partitions are required for the whole model(for orange colored ones, it is mandatory)

Figure 31: Partition - Extend face

27



28

Figure 34: Partition - Extrude edges

29

Figure 35: Partition - The edges have been extruded

30

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

Figure 37: Partition - At the end of previous operation

32

Figure 38: Partition - Select the point as pointed by the arrow and the line in pink


33



34

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.



35

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 45: Partitioning done - Everything is green!

36

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

Figure 47: Edges biased towards the solder(top)

38

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

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

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

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

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

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

4

Postprocessing

The results generated from the analysis can be enormous so it requires additional 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

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

Finite Element Project Abaqus Tutorial

Recommend Documents