You might like to start reading this worked example from the beginning:
Continuum Damage Mechanics: Worked Example
In this phase of the calibration, one must first determine the location of damage initiation in each of the specimens used. This is typically done by using information from both the test and a simulation of the test. Visual inspection of the test helps to identify the general region of failure and further FE analysis is used to identify the specific location, especially since the failure location is often in the interior of the part. For some specimen geometries, this location is well documented in the scientific literature. In each FE model, one must identify (specify) this location by defining a one-element elset with the specific name of "damage_location". For all of the specimens listed below, they were run with the material model that came out of Step 1c. These runs are not performed in the calibration app, since user inspection will be needed to identify the damage initiation location (element). That location is the location of maximum PEEQ.
Smooth Round Specimen: This specimen geometry, when pulled in uniaxial tension, develops the peak PEEQ and TRIAX at the center of the specimen. See image above. The LODE angle parameter in this specimen geometry is 1.0 This specimen will fail beginning at the center of the specimen. In our models this is identified by
*Elset, elset=damage_location
1175
For that element, at the end of the analysis we see
PEEQ = 1.049 TRIAX = 1.003 LODE = 1 (runtime = 37 secs)
smR10 Specimen: (round bar with 10mm radius circular notch) In this specimen the TRIAX maximum is always at the center. The PEEQ maximum begins at the root of the notch but progresses to the center of the specimen as the deformation evolves.
In the model provided in this post, the center element is identified by:
*Elset, elset=damage_location
1335
For that element, at the end of the analysis we see
PEEQ = 0.652 TRIAX = 1.319 LODE = 1 (runtime = 30 secs)
smR43 Specimen: (round bar with 43mm radius circular notch) In this specimen the TRIAX maximum is always at the center. The PEEQ maximum begins at the root of the notch but progresses to the center of the specimen as the deformation evolves. The purpose of the different size notches is to vary the state of triaxiality. Most metals will fail at a lower PEEQ as the TRIAX is higher.
In the model provided in this post, the center element is identified by:
*Elset, elset=Center
1804
For that element, at the end of the analysis we see
PEEQ = 0.835 TRIAX = 1.148 LODE = 1 (runtime = 167 secs)
GrvR1_5 Specimen: (Flat Bar with 1.5 mm groove) This specimen is modeled in Abaqus with plane strain elements. The bar is 5mm thick and 40mm in depth. In this specimen geometry the PEEQ spatial maximum is always at the root of the groove. The peak TRIAX is in the interior of the part, beneath the root of the groove. Failure initiates on the surface at the root of the groove.
In the model provided in this post, the element at the root of the groove is identified by:
*Elset, elset=damage_location
283
For that element, at the end of the analysis we see
PEEQ = 0.606 TRIAX = 0.601 LODE = 0.0004 (runtime = 4 secs)
GrvR2_5 Specimen: (Flat Bar with 2.5mm groove) This specimen is modeled in Abaqus with plane strain elements. The bar is 5mm thick and 40mm in depth. The peak PEEQ is initially at the root of the groove on the surface, but progresses to the center of the specimen as the deformation evolves. The peak TRIAX is always at the center of the specimen. Damage initiates at the center of the specimen.
In the model provided in this post, the center element is identified by:
*Elset, elset=damage_location
490
For that element, at the end of the analysis we see
PEEQ = 0.323 TRIAX = 1.344 LODE = 0.0025 (runtime = 15 secs)
Shear Specimen: This is sometimes called a rail shear specimen. A shear band of peak PEEQ forms in the shear web. The peak TRIAX is well away from the peak PEEQ. The LODE angle peaks just outside this shear band, or at the edge of this band. Element 3496 is chosen as the location of maximum PEEQ, thus the location where failure initiates.
In the model provided in this post, the damage location element is identified by:
*Elset, elset=damage_location
3496
For that element, at the end of the analysis we see
PEEQ = 0.868 TRIAX = 0.354 LODE = 0.755 (runtime = 131 secs)
The process of determining the Hosford-Coulomb *damage initiation parameters is philosophically just determining the parameters that will fit a surface through the six different PEEQ, TRIAX, LODE data points that we listed above. We have built a special purpose feature for this in the calibration app. In R2022x, this special feature is invoked by using this checkbox under Optimization Controls :
In R2023x, FD01, we moved this selection to the material model, Calibration Setup area
A zip file is provided at the bottom of this post containing all the files needed to carry out a calibration as per this narrated video. This is a newer version of the video with better audio. This video was created on 4-7-2023 using R2023x FD01 (HotFix 1.22)
This is the older version of the video created with R2022x, with poor audio quality (will delete this later).
Here is an image at the end of the video. I should have mentioned that in Plot.8, which is plotted as Triaxiality (TRIAX) on the Y-axis, you could use the plot controls and change that to show the PEEQ or the LODE variable.
Zip file contains a total of 9 files:
1) six run-ready .inp files for each specimen geometry. These six files were run to completion using version 2022 of Abaqus. All FE models contain the "damage_location" elset.
2) The file "Material_Model_Calibration_Step1c_Final.inp contains the material snippet produced by step1c. This is not used in the video, just attached for reference.
3) The file "synthetic_data_all.xlsx" is the same Excel file of data as was posted in earlier steps.
4) The file "CDM_Step1c_20pts_final_2022-06-29.3dxml" is the result of the earlier step1c.
The zip file below contains just a single file, the 3dxml file at the very end of the video.
This 3dxml file was generated using R2022x HotFix 2.21 of the 3DExperience platform.
Back to: Continuum Damage Mechanics: Worked Example
Back to: Continuum Damage Mechanics: References
Back to: Sharing Material Test Data
Back to: Material Modeling and Calibration - An Overview and Curriculum
