Tutorial for 2D Crack Growth with Hard Circular Inclusion
Creating the Plate Domain
1. Open Abaqus/CAE 6.9 or later.
2. Double click on Parts. Enter name as Plate, Modeling Space is 2D Planar, Type is Deformable, Base Feature is Shell and Approximate Size is 10. Click Continue.
3. Use the rectangle tool to draw a square from (-2,-4) to (2,4). Use the circle tool to draw a circle with radius 1 and center at (0,-2). Click Done.
4. Double click on Materials. Enter name as Mat1. Click on Mechanical, then Elasticity, then Elastic. Enter Young's modulus as 1 MPa and Poisson's ratio as 0.33. Click on Mechanical, then Damage for Traction Separation Laws, then Maxps Damage. Enter a value of 1 kPa. Click on the Suboptions box, then Damage Evolution. Type is Energy, Softening is Linear, Degredation is Maximum, Mixed-Mode Behavior is Mode-Independent, Mode Mix Ratio is Energy. Enter a value of 50 for the Fracture Energy. Click Ok. Click Ok.
5. Double click on Sections. Name as Plate. Accept default settings by clicking Continue. Select Mat1 as material and click box by Plane stress/strain thickness. Enter 1 as thickness. Click Ok.
Creating the Inclusion Domain
1. Double click on Parts. Enter name as Inclusion, Modeling Space is 2D Planar, Type is Deformable, Base Feature is Shell and Approximate Size is 10. Click Continue.
2. Use the circle tool to draw a circle with radius 1 and center at (0,-2). Click Done.
3. Double click on Materials. Enter name as Mat 2. Click on Mechanical, then Elasticity, then Elastic. Enter Young's modulus as 10 MPa and Poisson's ratio as 0.33. Click on Mechanical, then Damage for Traction Separation Laws, then Maxps Damage. Enter a value of 10 kPa. Click on the Suboptions box, then Damage Evolution, Type is Energy, Softening is Linear, Degredation is Maximum, Mixed-Mode Behavior is Mode-Independent, Mode Mix Ratio is Energy. Enter a value of 1000 for the Fracture Energy. Click Ok. Click Ok.
4. Double click on Sections. Name as Inclusion. Accept default settings by clicking Continue. Select Mat2 as material and click box by Plane stress/strain thickness. Enter 1 as thickness. Click Ok.
Creating the Total Uncracked Domain
1. Expand Assembly, then double click on Instances. Select both the plate and inclusion. Click Ok.
2. Merge the two parts together using the merge button on the left of the viewport. Name the part as Total, Merge is Geometry, Options is Suppress and Intersecting Boundaries is Retain. Click Continue. Select the two parts and click Done.
3. Expand Parts then Total. Double click on Section Assignments. Select the plate section from the viewport. Click Done. In Edit Section Assignment window, pick Plate. Click Ok.
4. Double click on Section Assignments. Select the inclusion section from the viewport. Click Done. In Edit Section Assignment window, pick Inclusoin. Click Ok.
5. Double click on Mesh. From the top menu select Seed, then Edge By Number. Select Total. Click Done. Enter 41 as number of elements along the edges. Hit Enter. Click Done.
6. From the top menu Select Mesh, then Controls. Select Total. Select Quad as Element Shape. From the top Menu select Mesh, then Part. Click Yes.
Creating the Cracked Domain
1. Double click on Parts. Enter name as Crack, Modeling Space is 2D Planar, Type is Deformable, Base Feature is Wire and Approximate Size is 5. Click Continue.
2. Draw a line from (-2,0) to (-1.5,0). Click Done.
3. Expand Assembly, then double click on Instances. Select Crack. Accept default settings by clicking Ok.
4. Double click on Interactions. Click Cancel. From top menu click Special, then Crack, then Create. Name as EdgeCrack, Type is XFEM. Click Continue. Select the uncracked domain as the Crack Domain. On the menu which appears, Specify the Crack Location by clicking on the lin signifying the crack. Click Ok.
5. Double click on Interactions. Enter name as Growth. Select Intial Step and Types for Selected Step as XFEM Crack Growth. Click Continue. XFEM Crack should have EdgeCrack. Click Ok.
Create the Boundary Conditions and Loads
1. Double click on Steps. Enter Name as Loading. On Incrementation Tab enter Type as Automatic, Maximum Number of Increments as 100000 and Increment Size as 0.01, 1e-005, 0.01. Click Ok.
2. Double click on Loads. Enter name as TopPressure, Category is Mechanical, Type is Pressure. Click Continue. Select the top edge of the domain. Click Done. Enter -700 as Magnitude, other settings are default. Click Ok.
3. Repeat sept 2 for the bottom edge of the domain, entering the name as BottomPressure.
4. Double click on BCs. Enter name as FixedBREdge, Step is Initial, Category is Mechanical, Types for Selected Step is Displacement/Rotation. Click on the bottom right corner of the domain. Click Done. Set U1, U2 and UR3 to zero. Click Ok.
5. Repeat step 4 for the top right corner of the domain. Enter name as RollerTREdge. Set U1 and UR3 to zero.
6. Expand Field Output Requests, double click on F-Output-1. Expand the Failure/Fracture options and check the box next to PHILSM, Level set value phi. Click Ok. This will allow you to view the level set function defining the crack.
Solving the System of Equations
1. Double click on Jobs. Enter name as IncCrack. Click Continue. Accept defualt settings by clicking Ok.
2. Expand Jobs. Right click on IncCrack and click Submit.
3. Right click on IncCrack, click Results to view results.