INTRODUCTION
This tutorial provides step-by-step instructions to begin cohesive crack modeling using FRANC2D and the defined crack path strategy. A familiarity with CASCA and FRANC2D is assumed in the presentation of information. For information on the basics of using CASCA and FRANC2D, please refer to the FRANC2D primer. There are some differences between FRANC2D and FRANC2D/L, these will be discussed at the end.
Tulio Bittencourt performed much of the work to allow cohesive crack modeling in FRANC2D as part of his Ph.D. research. For more technical information and background on the cohesive crack modeling capabilities in FRANC2D, please refer to his thesis,
Bittencourt, T. N., 1993,
"Computer Simulation of Linear and Nonlinear Crack Propagation in
Cementitious Materials," Ph. D. Dissertation, Department of Civil and
Environmental Engineering, Cornell University, Ithaca, NY.
The cohesive capabilities in FRANC2D are applicable to any material exhibiting cohesive crack behavior. In this tutorial, cohesive crack behavior means that once the stress ahead of the crack tip reaches a limiting tensile value, stress is transferred across the crack according to a function of the crack opening. This generic model can be considered a general Dugdale-Barenblatt model.
To illustrate the steps required to implement the defined crack path strategy in FRANC2D, this tutorial focuses on a concrete single edge notched beam in three point bending (Figure 1).
Figure 1. Single edge notched beam.
At this time, the cohesive cracking aspects of FRANC2D are not very user friendly. Until this is updated, follow the steps outlined in this tutorial closely. The "NOTE:" comments relate to especially important information to avoid problems.
Save the model often, and use different checkpoint names so that you can go
back to a particular step if there is an irrecoverable mistake.
MODELING THE BEAM
Use the CASCA program to generate the geometry and mesh information for the model. Ensure that the crack path consists of element boundaries. If the path is a straight line, a "subregion" line will ensure that the path is a boundary between finite elements.
For the beam in this example, the dimensions are as follows:
L = 27.5 d = 6.0
S = 24.0 ao = 2.0
b = 3.125 t = 0.125
FRANC2D uses the zoom level in the main program window to determine
the tolerance distance for nearest nodes and edges. Because of this, I initially
had difficulty generating two different points to be the tip of the notch. By
zooming in, I was able to create the two points by typing in coordinates.
Figure 2b. Single edge beam mesh.
FRANC2D PRE-PROCESSING
The main menu that displays when FRANC2D starts is shown in Figure 3a.From this menu, select the "Pre-process" button.The menu in Figure 3b will appear.
Figure 3. (a) Main menu. (b) Pre-process menu.
The first two pre-processing tasks are set the boundary conditions and input the material properties.It does not matter which task comes first.The boundary conditions are set through the "Fixity" menu. This is described in the FRANC2D primer.The material properties are set through the "Material" menu.
After selecting the "Material" button, the menu changes to the one shown in Figure 4 and an auxiliary window activates.By default the model has the properties of Material 1.By selecting the "E", "Nu" and "Thickness" buttons, you can change the properties of Material 1.
Figure 4. Material menu.
For this example, I set the properties to E = 4e6, Nu = 0.18 and Thickness = 3.125.Once I set the properties, the text in the auxiliary window read as follows.
Total number of materials : 1
Material number : 1
Material type : Isotropic
Young's Modulus : 0.400E+07
Poisson ratio : 0.180
Thickness : 3.13
KIc : 1.00
Density : 0.868E-1
Alpha : 0.000E+00
For the cohesive interface, we generate a new material by selecting the "New Mat" button.The new material menu is shown in Figure 5a.From it, select the "NL Interface" button.The non-linear interface menu is shown in Figure 5b.
Figure 5. (a) New material menu. (b) Non-linear interface menu.
Initially, the cohesive laws for shear and normal stresses are not defined.To set the shear, select the "Shear" button to get the non-linear shear material menu shown in Figure 6a.For this example, use a "linear" law with a stiffness of 7e7.You input the stiffness in the terminal window.After inputting the stiffness, the program provides the following information in the terminal window.
**********************************************
>>>>>>>>>>>>>>>>>> SHEAR <<<<<<<<<<<<<<
Display of parameters for linear elastic behavior
in a non-linear Interface
**********************************************
Stiffness : 7.0000000E+07
Figure 6. (a) Non-linear shear material menu. (b) Non-linear normal material menu.
To input the cohesive relationship for normal stresses, select the "Normal" button in the non-linear material menu.The menu changes to the one shown in Figure 6b.For this example, use a linear softening relationship.After selecting the "Linear" button, the program prompts you for input in the terminal window.The first question is,
$Is this a symmetry interface
[Yes-1,No-0]:
350
$What is the Critical Opening displacement :
5.58e-3
$What is the Compressive stiffness :
7e7
The program then provides a summary of the interface properties in the terminal window.
**********************************************
>>>>>>>>>>>>>>>>>> SHEAR <<<<<<<<<<<<<<
Display of parameters for linear elastic behavior
in a non-linear Interface
**********************************************
Stiffness : 7.0000000E+07
************************************************
>>>>>>>>>>>>>>>>>> NORMAL <<<<<<<<<<<<<<<<<
Display of parameters for linear softening
behavior in a non-linear Interface with Linear
elastic compressive behavior
***********************************************
Symmetry flag : 0.0000000E+00
Tensile strength : 350.0000
Critical opening : 5.5800001E-03
Compressive stiffness: 7.0000000E+07
The last step in this process is to set the thickness of the
interface.Use the same thickness as the global thickness, 3.125 for our
example.Once this is complete, the text in the auxiliary window reads as
follows.
Material number : 2
Material type : Nonlinear Interface
Shear Model: Linear
Normal Model: Linear Softening
Thickness: 3.13
NOTE: Careful selection of the compressive stiffness
value, kc, entered for the Normal Model will avoid numerical
instability problems. It is desired to have a high compressive stiffness
to model the linear response of the interface element. However if the peak of
the curve becomes to narrow convergences problems may be encountered.
Divergence during the solution procedure may indicate that the peak of the
interface material model is too narrow.
Figure 7. (a) Linear Softening
Interface Model with wide peak. (b) Linear Softening Interface Model with
narrow peak that may cause numerical instability.
The last pre-processing task is to apply the "load". From the pre-processing menu, select the "Loads" button.The loads menu is shown in Figure 8a.If we actually apply loads to the model, we can only capture behavior up to the peak load. In order to track post peak behavior, we apply displacements to the model.Therefore, select the "Appld Disp" button to get to the applied displacement menu shown in Figure 8b.For this example, we apply a point displacement.After selecting the "Pt. Disp." button, the point displacement menu shown in Figure 8c appears.
Figure 8. (a) Loads menu. (b) Applied displacement menu. (c) Point displacement menu.
NOTE: The applied displacement must be the 1st load case.
NOTE: If you need to change the location of an applied displacement or otherwise need to remove an applied displacement, you must also go back to the "Fixity" menu, remove the fixities and reapply them.
NOTE: The program converts the applied displacement to nodal equivalent loads.Therefore, the material properties must be specified before applying the displacement.
The solution scheme used in FRANC2D does not "propagate" the
crack.The dynamic solver finds the equilibrium configuration for the model for
the applied displacement.To "propagate" the crack, apply a larger
displacement and rerun the analysis.This method can be used to generate points
on the load versus displacement or load versus CMOD graph.The solution to each
applied displacement is one data point.
ADD THE NL INTERFACE
Once the pre-processing is complete, we are ready to add the non-linear interface.From the main menu, select the "Modify" button.The modify menu is shown in Figure 9.From the modify menu, select the "Add NL Intfc" button.
Figure 9. Modify menu.
This is the most temperamental part of the program.Follow these next instructions exactly.Input the interface one element at a time.Begin at the outer edge of the model and build the elements in the direction that the crack will grow.
After selecting the "Add NL Intfc" button, the program window will give you the command to "Select the first node of the first int elem".Select the first node of the interface.It must be the node at the outer face where the crack begins (node "A" in Fig. 10).Hit the "Done" button.
The program window will give you the command to "Specify end node of elem & hit DON".Select the node at the other end of the first element (node "B" in Fig. 10).Hit the "Done" button.
The program window will give you the command
"To end interface, specify previous node".At this point if you wish
the interface to continue select the corner node of the next element (node
"D" in Fig 10) and then hit "Done". Continue
selecting adjacent corner nodes until you have selected all of the desired
elements. To end the interface reselect the last node you selected (node
"C" in Fig. 11) and hit "Done". If everything worked
correctly, you will be automatically taken to the "Modify" menu
again.
Figure 10. Sequence of node selection
for the first and continuing NL interface element.
Figure 11. Sequence of node selection for the last NL interface element.
Interfaces can be placed all the way to the edge of body. When the interfaces elements are fully opened this will break the body.Check to see if adding the load first will work with a full interface.
To check that the interface has been inserted, return to the "Main" menu and select the "Boundary" button.This button toggles off the mesh.The nonlinear interface should be shown as a thin line inside the geometry borders (Fig. 12).You may select the "Mesh" button to toggle the mesh back on. The interface can also be check from the "Modify" menu by selecting "Intrfc: On". This changes the color of the mesh to orange and the boundaries and interfaces to white. Selecting "Intrfc: Off" returns the entire model to being displayed in white.
Figure 12. Correctly inserted interface shown by toggling off the "Boundary" button.
NOTE: Do not put interface elements through the entire height of the model such that the last element reaches a free surface.This may become unstable.
Once you insert the interface, it remains.Therefore, you do not need to
replace the interface after changing the applied displacement for subsequent
solutions.
ANALYSIS
To begin solving the model, select the "Analysis" button from the main menu.From the analysis menu (Fig. 13a) select the "Linear" button.From the linear solution menu (Fig. 13b) select the "Dyn Relax" button.
Figure 13. (a) Analysis menu. (b) Linear menu.
The program provides the following cues in the terminal window and waits for your responses.Once you have input the solver criteria, the program begins the solution.Once the solution residual becomes less than the tolerance you input or the solver exceeds the maximum number of iterations you specified, the program provides a summary of the solution.
DYNAMIC RELAXATION ANALYSIS:
Enter the tolerance (fraction of appl. load):
1e-3
Enter the max number of iterations:
5000
Starting iterations:
Iteration Max Acc*Mass Residual Norm Target Max
delta u
100
0.1947E+05
0.1924E+05
90.69
0.3754E-04
200
6306.
6241.
90.69
0.2064E-04
300
2607.
2587.
90.69
0.1301E-04
400
1352.
1344.
90.69
0.9112E-05
500
815.1
811.5
90.69
0.6713E-05
600
548.5
546.6
90.69
0.5265E-05
700
402.7
401.6
90.69
0.4399E-05
800
317.7
317.0 90.69
0.3882E-05
900
270.4
270.4
90.69
0.3620E-05
1000
277.8
277.9
90.69
0.3547E-05
1100
281.8
281.9
90.69
0.3618E-05
1200
283.0
283.0
90.69
0.3805E-05
1300
283.7
283.7
90.69
0.4134E-05
1400
283.0
283.0
90.69
0.4495E-05
1500
279.8
279.7
90.69
0.4843E-05
1600
274.6
274.5
90.69
0.5189E-05
1700
267.8
267.7
90.69
0.5534E-05
1800
259.6
259.5
90.69
0.5843E-05
1900
250.4
250.3
90.69
0.6114E-05
2000
240.3
240.2
90.69
0.6343E-05
2100
229.5
229.4
90.69
0.6527E-05
2200
218.3 218.2
90.69
0.6662E-05
2300
206.8
206.6
90.69
0.6748E-05
2400
195.1
194.9
90.69
0.6782E-05
2500
183.3
183.2
90.69
0.6767E-05
2600
171.6
171.4
90.69
0.6708E-05
2700
160.2
160.1
90.69
0.6599E-05
2800
149.0
148.9
90.69
0.6445E-05
2900
138.2
138.1
90.69
0.6257E-05
3000
1
27.8
127.7
90.69
0.6034E-05
3100
117.8
117.7
90.69
0.5786E-05
3200
108.4
108.3
90.69
0.5518E-05
3300
99.42
99.34
90.69
0.5234E-05
3400
91.04
90.96
90.69
0.4942E-05
Converged in 3406 iterations
Load Residual Norm = 90.96
**********************************************************************
FRANC Analysis Report
2538 Equations
0 Nonlin Interface Eq.
Total Time (inc overhead) : 763 seconds
**********************************************************************
Analysis done
If the dynamic relaxation analysis crashes with a "floating error" or the residual error keeps growing while the solver is working, the "shear" stiffness is probably too high. Try a lower value. You do not need to rebuild the interface, just change the material property.
If the dynamic relaxation analysis oscillates and does not converge or is
slow to converge, the compressive stiffness of the "normal" stresses
law is probably too high. Try a lower value. You do not need to rebuild the
interface, just change the material property.
POST PROCESSING
To review the results, select the "Post-Process" button on the main menu.Select "Deformed Mesh" to see the displaced shape. Unlike deformed meshes with explicit cracks, the opening of the interface elements does not necessarily mean that the interface elements have broken forming a crack.
Figure 14. Deformed mesh
To view the opening and stresses along the interface elements return to the Post-Processing Menu and select "Fract Mech." For plots along the interface elements select "Interfc Plts." The program will prompt you to "Specify the starting nodal point." Select the first node of the interface. Next you will be prompted to "Specify the adjacent corner nodal point. This is the next corner node along the interface, not the next node that would be a med-side node. Finally the program will ask you to "Specify the ending corner nodal point." This is the last node along the interface that again should be a corner node. If you cannot select the entire length of the non-linear interface to display crack opening while post processing, you may have a discontinuous interface.
Once you have selected the interface the side menu will change giving a list of plots that can be made along the interface. To view the crack development along the interface select "Opening." The Opening vs. Position plot will appear in the auxiliary window. For this example the opening displacement exceeds the critical opening displacement specified of 5.58e-3 specified in the interface material model. This indicates that the interface has been broken forming a crack.
Figure 15. Opening vs. Position along centerline interface elements.
The portion of the interface that has opened can also be determined by selecting "Normal Stress" to view the stress being carried across the interface. If the interface has opened it will no longer transfer stress across it. The Normal Stress vs. Position plot also illustrates the softening occurring along the interface.
Figure 16. Normal Stress vs. Position along interface elements.
To observe the stress distributions in the rest of the body return to the
"Post-Process" menu and select "Contour." Also from
available from the "Post-Process" menu is the "Line
Plot." This plots the stress for line you specify. This option
is usefully for plotting stresses either side of the interface.
The original version of FRANC2D/L created by James included
a limited implementation of interface elements.The elements were implemented,
however, only a limited number of models were included.The models were
uncoupled linear and user defined models for both normal and shear.Through the
work of Iesulauro the models were expanded to included linear-softening for the
normal model and the linear-softening coupled model.Other models can be added
to the current implementation.Details on the implementations added please refer
to her thesis.
There are a few things to consider when conduction a
simulation using interface elements.One is which solver is to be used.If
linear-elastic materials are being used then either Dynamic Relaxation solver
demonstrated above or the Material Non-Linear solver may be
appropriate.However, is elastic-plastic materials are being used then the
Dynamic Relaxation solver will not be appropriate due to the history dependence
of the material.In this case the Newton-Raphson solver should be used.Once the
solver has been chosen this will determine how the interface elements may be
placed with in the model.
The post-processing available in FRANC2D/L includes deformed
meshes, stress and strain contours, line plots, the ability to calculate
several fracture mechanics related quantities, and interface plotting just as
in FRANC2D.The interface plots allow quantities along a single line of
interface elements to be plotted.Quantities that can be plotted include normal
and shear stresses and normal and shear displacement.