Analysis of Rupture Plate with Different Material Model Laws

Objective:

• To analyze the rupture plate with 7 different cases of material cards, and compare all the results.
• The 7 different cases of material cases are as follows:

1. Run the given model as it is and name it as ‘Law2_epsmax_failure.
2. In /FAIL/JOHNSON, change Ifail_sh=1, Dadv=1, Ixfem=1. Run the model as ‘Law2_epsmax_crack’.
3. Delete the /FAIL/JOHNSON card as run the model with the name ‘Law2_epsmax_nofail’.
4. Delete the values of eps_p_max and run the model with the name ‘Law2’.
5. Convert this material model to Law 1 elastic with the same density, E, nu, and run. Check the results.
6. Open Law27_0000.rad. Change the shell properties to recommended shell properties. Run the model with the name Law27.
7. Change the material model to Law36_PLAST_TAB and run the model as ‘Law36’.

Introduction:

• The simulation of any model or component is depended on the type of material specified during preprocessing. Different material properties are given as input depending on the requirement of the model, i.e. the type of material that would be used for manufacturing, and the type of simulation that has to be carried out.
• There are various types of material laws present in HyperMesh which govern different types of materials, ranging from metals like steel, aluminum, alloys, to foam, rubbers, etc. All these laws have their separate properties which define that specific material, along with its behavior under various loads, and temperature.
• Out of all these laws, the most important and commonly used laws are:

Law 1 – Elastic

Law 2 – Johnson-Cook

Law 25 – Composite

Law 27 – Elastic-Plastic Brittle

Law 28 – Honeycomb

Law 36 – Elastic-Plastic Tabulated

Law 42 – Ogden (Hyperelastic)

Law 69 – Ogden & Mooney-Rivlin (Hyperelastic)

Law 70 – Foam

• Law 1 of Isotropic Elasticity, /MAT/ELAST, is available for trusses, beam (only type 3), shell, and solid elements. This law is not suitable for a large number of deformations and hence has limited applications.
• Law 2 Isotropic Elasto-Plastic (Johnson-Cook), as the name suggests, has both elastic and plastic natures of deformation, unlike the 1^st law which has only elastic properties and follows Hooke’s law. This is most suitable for large deformations and the user has control over the behavior of the material. This model expresses material stress as a function of strain, strain rate, and temperature.
• Law 27 /MAT/PLAS_BRIT is used for Elasto-Plastic material with brittle material like glass, and some cases of aluminum, etc. This law combines an isotropic elastoplastic Johnson-Cook material model with an orthotropic brittle failure model. In this law, failure and damage occur only in tension and is only applicable for shell elements.
• Law 36 PLAST_TAB (/MAT/PLAS_TAB) Elastic-Plastic Piecewise Linear Material is the most commonly used law in the industry as of now. This law models an isotropic elastoplastic material using user-defined functions for the work-hardening portion of the stress-strain curve (for example, plastic strain vs. stress) for different strain rates. This law is available for brick and shell elements.

Procedure and Observation:

• For all the cases, 0000.rad file has been imported using the ‘import solver deck’ option.

Case 1: Run the given model as it is and name it as ‘Law2_epsmax_failure.

• The ‘FAILURE_JOHNSON_0000.rad’ was imported and was run as it is. The run time and the animation frequency were present in the file. The material card and its properties looked like below.
  
  
• To run the file, the ‘Radioss’ option from the ‘analysis’ tab was selected and the path for the result files was specified. Keeping the ‘options’ value as ‘-nt 4’ the Radioss button was hit.
• This created the .out files, the animation files, and the template file. The 0001.out file from these files was opened with the notepad and the cycles, energy error, and mass error were observed as follows:

Cycles: 49479

Energy error: 0.2% (within limit of 15%)

Mass error: 0.000.

• The following image shows the energy and the mass errors along with the cycle frequency
  
  
• By clicking onto the HyperMesh icon, the module was switched to HyperView. The ‘.h3d’ file was opened from the ‘load results’ option and was ‘applied’.
• The animation of the model was observed, and it was evident that the elements in the model are getting deleted after a certain amount of strain has been reached.
• From the ‘contour’ option, the ‘von-misses’ stress simulation results were loaded by keeping the averaging method on ‘simple’. This loaded the animation of the Von-Misses stress, and it was noted that the maximum amount of stress generated in the rupture plate was 2.876e⁺⁰²N/mm². The animation gif below shows the von-misses stress simulation.
  
  

• After this, the results were changed to plastic-strain, and the maximum plastic strain reached in the rupture plate was 1.502e^-01. Since the value of eps_p_max was set as 0.151, meaning that the failure occurs at 15% of the total strain value, the elements got deleted when the strain of 1.502e^-01 was reached. The following gif shows the plastic strain simulation.
  
  
• Later, the graphs for internal energy, kinetic energy, hourglass energy, etc. were plotted. But since the Ishell was selected as QEPH in the properties, which has material level stabilization, the hourglass energy came out to be 0 throughout the simulation. The image below shows the internal energy and kinetic energy graphs.
  
  
• As it is evident for the kinetic energy graph, there is a sudden surge in the value around the 4^th This is because the element is being deleted at the same time which can also be seen in the gif of plastic strain. The maximum amount of internal stored in the plate is around 27500mJ since aluminum is a ductile material and can absorb a high amount of energy. While the kinetic energy has its peak at 550mJ approximately.

Case 2: In /FAIL/JOHNSON, change Ifail_sh=1, Dadv=1, Ixfem=1. Run the model as ‘Law2_epsmax_crack’.

• The same previous model was imported and from the ‘failure’ collector, the above-mentioned properties were changed. Ifail_sh is the shear failure flag, Dadv is the crack advancement criterion (=1 is the default value). Ixfem is the xfem formulation (for crack). When ixfem is set as 1, the failure of the element is more realistic, and crack propagation occurs initially instead of the elements getting deleted.
• All these values were entered in the failure collector as shown below.
  
  
• ‘Radioss’ was done from the ‘analysis’ tab and all the files were saved. The 0001.out file was opened with the notepad and the energy and mass errors, and the cycles were as follows.
  Cycles: 49396
  Energy error: 4.0%
  Mass error: 0.000
  
  

• Here, though the energy error came out higher than the previous case, it was within the limits of 15%. Later, the different simulations were viewed in the HyperView module by opening the .h3d file.
• The Von-Misses stress was observed to be 2.947e⁺⁰² N/mm², slightly above that of the previous case. Here, the crack formation was clearly visible. This was due to the xfem formulation factor. The image below shows the crack formation.
  
  
• The elements in the central portion where the strain was maximum, first cracked and then they were deleted. The gif below shows Von-Misses stress.
  
  
  
  
• Another gif below shows the Plastic Strain formulation where the maximum value is 1.489e^-01.
  
  

• When both the Cases 1 and 2 were compared and the difference was clearly visible. In the 1^st case, the elements ruptured and got deleted at the 4^th ms, whereas in the 2^nd case, the plate absorbed more stress, cracks were formed, and the deletion process delayed a little. The kinetic energy graph plot in the 2^nd case showed a spike slightly after 4.5^th ms when the elements got deleted. The gif and image below show the comparison.
  
  
  
  
• Graphs of internal and kinetic energy for case 2:
  
  

Case 3: Delete the /FAIL/JOHNSON card as run the model with the name ‘Law2_epsmax_nofail’.

• In this case, the failure card had to be deleted and had to be run without any failure model. The following images show the default material model and properties.
  
  
• The ‘Radioss’ was done from the ‘analysis’ tab and the values of cycles, energy error, and mass error were as follows:
  Cycles: 49404
  Energy error: 0.8%
  Mass error: 0.000
  
  
  
  
• The energy error was well within the limit and hence the further analysis was carried out. HyperView was opened and the .h3d file was imported. The simulation for Von-Misses stress was loaded which showed a maximum value of 2.705e⁰² N/mm².
  
  
• The elements are getting deleted at the 4^th ms, which can be seen in the gif above. Later, the plastic strain was plotted which had the highest value of 1.494e^-01.
  
  
• From the HyperGraph2D, the template T01 was loaded, and the graphs for internal energy and kinetic energy were plotted by splitting the screen as shown below.
  
  
• Here, in this case, the failure of the model occured at the 4^th ms and the elements got deleted. Therefore there was a spike in the kinetic energy due to the failure, while the internal energy graph of the model got flat and became stable, due to the fracture. The peak kinetic energy was just above 350mJ, while the internal energy went till 27000mJ. In this case, too, the hourglass energy was 0 as the properties were unchanged keeping Ishell as QEPH type.

Case 4: Delete the values of eps_p_max and run the model with the name ‘Law2’.

• Keeping all the parameters as the previous case, without Johnson failure card, only the eps_p_max value was deleted. Since the failure plastic strain was deleted, there was no governing or the boundary value which would define the failure of the model.
  
  
• ‘Radioss’ was done from the ‘analysis’ tab and all the files were saved. The 0001.out file was opened with the notepad and the energy and mass errors, and the cycles were as follows.
  Cycles: 48736
  Energy error: 3.0%
  Mass error: 0.000
  
  
• The animation for the Von-Misses stress results was loaded in the HyperView from the ‘load results’ option which had the maximum value of 4.247e⁰² N/mm².
  
  
  
  
• The maximum value of plastic strain obtained was 1.205e⁰ which was also much higher than the other cases.
  
  
• The stresses absorbed in the plate were almost double than those of the previous cases. This was because the plastic failure strain was deleted. The elements were also not failing as there was no limit for the failure. This case resembled the elastic case as the rupture plate was returning to its original position after removal of the load.
• Later, from the HyperGraph2D, the graph plots for the internal and kinetic energy were loaded. Since the elements were not fracturing or getting deleted, the kinetic energy generated was very low, the maximum value was 3.6 mJ, while the internal energy was rising exponentially till 65000mJ. The internal energy was a lot higher as compared to the other cases. The reason for this was the plate was absorbing more energy and stresses than the others due to the absence of the plastic failure strain limit.
• The image below shows the internal and kinetic energy graphs.
  
  

Case5: Convert this material model to Law 1 elastic with the same density, E, nu, and run. Check the results.

• Later, the material model for the same conditions was changed to Law 1 i.e. /MAT/ELAST (isotropic elasticity). This material model is available for shells and solid elements, along with trusses, and type 3 beams. It follows Hooke’s law and is used to model purely elastic materials. This law shows a linear relationship between stress and strain.
• In the same model, the material law was changed to M1_ELAST from the ‘card image’, and entering the same values of density, Young’s modulus, and kinematic viscosity. The images below show the material and the property card for this case.
  
  
• The analysis was done from the ‘Radioss’ option, and from the 0001.out file, it was found that the total cycles were 47968, while the energy and mass errors were 0.3% and 0.000 respectively. Since the value of energy error was acceptable, further analysis was carried out.
  
  
• From HyperView, the animation plot for the Von-Misses stress was analyzed and the maximum value of it reached up to 1.086e⁰⁴N/mm² as seen in the animation gif below. This was the highest value of all the cases since the material was behaving in a purely elastic manner. The reason being the /MAT/ELAST law applied.
  
  
• There was no failure of any of the elements of the rupture plate. The elements just got elongated and returned to their initial or the original position after removal of the load. Therefore, the body was able to absorb a large number of stresses, and also there was 0 plastic strain in the elements.
• Later, the graphs for the internal energy and kinetic energy were plotted in the HyperGraph2D. Since the material was purely elastic in nature and absorbed a large number of stresses, the internal energy in the body was also high and peaked at 850000mJ.
• On the other hand, the kinetic energy in the body was low due to less deformation and a lack of failure of elements. The maximum value of kinetic energy in the body found to be around 4650mJ. It had a surge at the end of the simulation when the deformation was the highest as seen in the image below.
  
  
  

Case 6: Open Law27_0000.rad. Change the shell properties to recommended shell properties. Run the model with the name Law27.

• For this case, the LAW27_0000.rad file was imported, and the properties were changed to the recommended shell properties which are generally used in the industry for a realistic approach. ‘Ishell’ was set on 24: QEPH shell formulation,
  Ismstr = 2: Full geometric non-linearities..,
  Ithick and Iplas =1
  
  
  
  
• After performing the ‘Radioss’ operation, the cycles and errors were checked in 0001.out file. Following were the values:
  Cycles: 49335
  Energy error: 1.0%
  Mass error: 0.000
  
  

• Since the value of energy error was acceptable, further analysis was done. The HyperView window was opened and the animation was loaded by importing the .h3d file. The failure and deletion of the elements occurred around 4.25^th The Von-Misses stress simulation was loaded, and the maximum value of the V-M stress was found to be 2.771e⁰²N/mm² as seen below.
  
  
• Later, the Plastic-strain simulation was loaded, and the maximum value of the plastic strain in the model reached up to 1.761e^-01. Since the value of the eps_p_max was set at 0.16 (i.e. elements to fail and get deleted at 16% of the total plastic strain), the elements in which the plastic strain exceeded this value got deleted from the system as seen in the gif.
  
  
  
  
• The graphs for the internal and the kinetic energy were then plotted in the HyperGraph2D.
  
  
• The maximum value of internal energy reached up to 40000mJ till the end of the simulation, while the kinetic energy has its peak at a lower value of 145mJ. The elements fail and get deleted at 4.25^th Therefore there is a spike during that timeframe.

Case7: Change the material model to Law36_PLAST_TAB and run the model as ‘Law36’.

• Now, the material model had to be changed to Law 36. Law 36 is the law for Tabulated piecewise linear with the card name as /PLAS_TAB. This law is the most commonly used law in the industry. This law is available for brick and shell elements.
• In this, the user can define the parameter values for the work hardening portion in the stress-strain curve and can create the curve and its function as per their requirement. The parameters entered in the material model are as follows:
  
  
  
  
• Keeping the value of N_funct as 1, the ‘test_curve_law36’ was created by defining the X and Y values for the strain and stress respectively. This generated a curve automatically as shown below.
  
  
• The ‘Radioss’ operation was performed and from the engine output file (0001.out) following values for cycles, energy error, and mass error were noted:
  Cycles: 52202
  Energy error: -1.5%
  Mass error: 0.000
  
  
  
  
• The animation for the Von-Misses stress was loaded and the maximum value was found to be 7.535e⁰²N/mm².
  
  
• Along with this, the plastic strain animation was also plotted.
  
  
• Later from the HyperGraph2D, the graphs for internal and kinetic energy were loaded from the T01 template file.
  
  
• Since the elements are getting deleted at 3.3^rd ms, there is a spike in the kinetic energy in that time frame.

Results and Conclusion:

Case No.	Material Card	Failure Card	Elements	Cycles	Energy Error	Mass Error	Von-Misses stress
Case 1	M2_PLAS_JOHN_ZERIL	FAIL_JOHNSON	Deleted	49479	0.2%	0.000	2.876e02
Case 2	M2_PLAS_JOHN_ZERIL	FAIL_JOHNSON	Cracked, Deleted	49396	4.0%	0.000	2.947e02
Case 3	M2_PLAS_JOHN_ZERIL	Deleted	Deleted	49404	0.8%	0.000	2.705e02
Case 4	M2_PLAS_JOHN_ZERIL	Deleted	Not Deleted	48736	3.0%	0.000	4.247e02
Case 5	M1_ELAST	n/a	Stretched	47968	0.3%	0.000	1.086e04
Case 6	M27_PLAS_BRIT	n/a	Deleted	49335	1.0%	0.000	2.771e02
Case 7	M36_PLAS_TAB	n/a	Deleted	52202	-1.5%	0.000	7.535e02

• Out of all the above cases, the 2^nd case is the most suitable and is more realistic. In this case, the Johnson-Cook failure card is used. Along with this, the xfem formulation is also active. The Ixfem value was set as 1. This shows a more realistic behavior of the material during the failure. Instead of getting deleted directly from the system, cracks are generated initially.
• Unlike the 2^nd case, the elements get deleted directly in the 1^st case without the formation of crack. The next most suitable case would the one with the /MAT/PLAST_BRIT material model, i.e. the 6^th The stresses in this case also resemble those of the aluminum after the 2^nd case.
• Case 5 with the elastic model, may give lower values of stresses, the elements behave as purely elastic but they don’t have a failure.
• Apart from this, all the other cases have very large values of the Von_Misses stress which do not resemble the original value of the aluminum of around 300-310MPa. But the only disadvantage of the PLAS_BRIT material card is that it can only be used for shell elements.
• The 7^th case, though can be used for brick and shell elements, it gives a huge amount of stresses (around 753 MPa in this case). Therefore, it’s also not suitable.
• Therefore, by understanding all the important and mostly used material laws, their advantages, disadvantages, and applications, and implementing them on the given models, this assignment was completed successfully.

Additional link for files: Material model files