Quickly Calibrate Abaqus Cohesive Models
In this post I will show how to quickly calibrate Abaqus cohesive element models, or cohesive surface models using MCalibration. This is a continuation of my discussion on how to work with cohesive materials in Abaqus. If you have not already, I recommend that you read that tutorial first. Also note that the features shown here are only available in MCalibration version 6.0, and later.
As was shown in Example 8 of my previous tutorial, the cohesive model definition can be divided into separate tables for each deformation rate and mixed mode condition (i.e. tension, shear, etc). In this example I will calibrate the parameter values for one rate and mode mixture. If you are interested in multiple rates and mode mixtures, which you should be, then repeat the procedure shown here for each condition, and then combine the parts into a master model for use with Abaqus.
The first step in the calibration is to create an experimental data file that contains three columns: (1) time, (2) displacement/separation, (3) traction. If you use a cohesive thickness of 1.0 (which is the default value in Abaqus), the displacement values become equal to the (engineering) strain in the adhesive.
The first step in the calibration is to read in the cohesive experimental data into MCalibration. Here’s the contents of one data file that I have for a pressure-sensitive adhesive (PSA).
# Time, Displacement_mm, Traction_MPa
0, 0, 0
0.00377432775245, 0.000226459665147, 0.00363983068575
0.00754865550491, 0.000455601128099, 0.00727966102738
0.0113229832574, 0.000733787809998, 0.0109194910808
0.0153207941602, 0.00102769561034, 0.014563896014
... (more lines here)...
Read in the experimental data as any time-strain-stress data file. Make sure you select True Strain, True Stress, and select the loading mode to be Confined Compression (1-dir). Use these settings even if the experimental data is obtained in shear or in a mixed mode.
Then in the main window of MCalibration select Set Material Model and select ABAQUS-COHT1.
The COHT1 (cohesive tension 1 condition) model uses the 9 material parameters shown in the figure below. E is the initial stiffness of the adhesive (in the loading mode in which the test was performed), and stressInit is the traction at which the damage starts. MaxSeparation is the max displacement the adhesive can take before final failure occurs. The damage evolution portion of the the response is captured using 6 cubic B-splines expressed as displacement-traction control points. The displacement control points are evenly distributed over the interval [0, MaxSeparation], and the damage values are given by the incremental values [deltaD1, …, deltaD5].
The parameter NrTerms specifies how many points the cubic B-splines are divided into when exporting the model into an Abaqus model.
Before starting to calibrate Abaqus cohesive models, it can be useful to manually tweak the provided MaxSeparation, E, and stressInit values. The results from my calibration of the exemplar PSA data is shown in the figure below. Note that the x-axis label can also be interpreted as the separation, and the y-axis can be interpreted as the traction.
Once the calibration has been completed you can export the model parameters to Abaqus inp-file format (both cohesive element and cohesive surfaces):
*Material, name=MCal_Mat
** Calibrated with MCalibration
** Calibration file name: simulation.mcal
*Density
1e-09
*Elastic, type=traction
** Enn, Ess, Ett
11.6603004638, 11.6603004638, 11.6603004638
**
*Damage Initiation, criterion=maxs, rate dependent
** Snn, Sss, Stt
0.504309915052, 0.504309915052, 0.504309915052
**
*Damage Evolution, type=displacement, softening=tabular
** damage variable, total displacement
0, 0
0.129775345205, 0.026542627108
0.257400593147, 0.053085254216
0.378849890981, 0.079627881324
0.490100105091, 0.106170508432
0.587704578619, 0.13271313554
0.669502850486, 0.159255762648
0.733508490333, 0.185798389756
0.777854384402, 0.212341016864
0.805311851821, 0.238883643972
0.824677700096, 0.26542627108
0.845151430265, 0.291968898188
0.875127897719, 0.318511525296
0.903507974928, 0.345054152404
0.910962074849, 0.371596779512
0.914296394536, 0.39813940662
0.928025913763, 0.424682033728
0.939740608275, 0.451224660836
0.948311731087, 0.477767287944
1, 0.504309915052
*Surface Interaction, name=coh
*Surface Behavior, pressure-overclosure=hard
*Cohesive Behavior, cohere=original contacts,
type=uncoupled
** Knn, Kss, Ktt [unit: stress/length]
11.6603004638, 11.6603004638, 11.6603004638
*Damage Initiation, criterion=maxs, rate dependent
** Snn, Sss, Stt
0.504309915052, 0.504309915052, 0.504309915052
**
*Damage Evolution, type=displacement, softening=tabular
** damage variable, total displacement
0, 0
0.129775345205, 0.026542627108
0.257400593147, 0.053085254216
0.378849890981, 0.079627881324
0.490100105091, 0.106170508432
0.587704578619, 0.13271313554
0.669502850486, 0.159255762648
0.733508490333, 0.185798389756
0.777854384402, 0.212341016864
0.805311851821, 0.238883643972
0.824677700096, 0.26542627108
0.845151430265, 0.291968898188
0.875127897719, 0.318511525296
0.903507974928, 0.345054152404
0.910962074849, 0.371596779512
0.914296394536, 0.39813940662
0.928025913763, 0.424682033728
0.939740608275, 0.451224660836
0.948311731087, 0.477767287944
1, 0.504309915052
**
*Contact, op=NEW
*Contact Inclusions, ALL EXTERIOR
*Contact Property Assignment
botBlock.top, topBlock.bot, coh
That’s it! If you like to can then repeat these steps for each cohesive rate and loading mode tested.
