Simulating the event of a rigid sphere crushing onto a flat plate using Radioss Explicit Analysis and comparing the results for 7 different cases, each having a different material and failure model defined for the flat plate

Objective:

1. To import the given models in Hypermesh and simulate the event of a rigid sphere hitting against a flat plate for the following cases:
   
   1. Case 1: Simulate with both the Failure plastic strain(Eps_P_max) and fail_johnson failure card enabled.
   2. Case 2: Simulate with failure plastic strain(Eps_P_max) and fail_johnson failure card enabled(put Ishell_sh= 1, Dadv= 1, Ixfem= 1)
   3. Case 3: Simulate after removing the fail_johnson failure card.
   4. Case 4: Simulate after removing both the failure plastic strain(Eps_p_max) and the fail_johnson failure card.
   5. Case 5: Simulate after changing the material law to Law1(Elastic).(Keep the same rho, E, nu values)
   6. Case 6: Simulate the model with material law27(Notice the various Eps based values unlike the Law2 card)
   7. Case 7: Simulate after changing to an aluminum material card(using law36)
2. To discuss the results for each case.
3. To compare the 7 case results by tabulating the values for the following parameters:
   1. The total number of cycles, Energy error, mass error, and simulation time.
   2. Notice the animation of all 5 and describe the animations in brief on the
      basis of whether the elements are being deleted or cracked.
   3. Plot energies and notice any difference.
   4. Based on all the results, which case would represent the on-field
      scenario.

Procedure:

1. Case 1: Simulate with both the Failure plastic strain(Eps_P_max) and fail_johnson failure card enabled.
   1. Import the given solver deck in Hypermesh. Fig 1. Imported model
   2. Go through the solver deck cards and properties and try to understand them. Fig 2(a). Material card Fig 2(b). Material block in Radioss Starter input file Fig 3(a). Failure model card Fig 3(b). Failure model block in Radioss Starter input file
   3. We have to run the analysis without making any changes to the solver deck. Note: In this case, to make the animation more smooth, we have decreased the t_freq value in the ENG/Anim/DT card to 0.05. Now Go to the Radioss option under the Analysis menu and run the deck in Radioss solver after saving the deck as Law2_Epspmax_failure.
   4. After successful completion of the run, open the Radioss Engine out file in notepad and check for energy errors and mass errors present in the simulation. We find that the errors are well within the allowable range(Energy error(5 to -15%) AND Mass error(2 to 3%)) and thus the results are acceptable. Fig 4. Error check(energy err= 0.8%; mass err= 0%)
   5. Now, we can go on and open the animation files in Hyperview. Create the necessary contours and plots needed for the Result study. Fig 5. Von mises stress contour Fig 6. Time vs IE_KE_CE_HGE_TE(mJ) Fig 7. Time vs resultant force(N) on the rigid sphere
2. Case 2: Simulate with failure plastic strain(Eps_P_max) and fail_johnson failure card enabled(put Ishell_sh= 1, Dadv= 1, Ixfem= 1)
   1. Import the given solver deck in Hypermesh.
   2. Go through the solver deck cards and properties and try to understand them. Fig 8(a). Material card Fig 8(b). Material block in Radioss Starter input file Fig 9(a). Failure model card Fig 9(b). Failure model block in Radioss Starter input file
   3. Open the fail_johnson failure card and enter the new values for Ishell_sh(=1), Dadv(=1), and Ixfem(=1). Note: Ishell_sh is the shell failure flag. Its default value is 1. It decides whether the failed elements are to be deleted or cracked. Dadv gives the criterion for crack advancement(Only active when Ixfem value is set as 1). The value of Dadv can be between 0 and 1 with 1 being the default value. Ixfem is the Xfem flag and determines whether xfem formulation has to be used or not. The default value is 0 in which the xfem formulation will not be used.
   4. Go to the Radioss option under the Analysis menu and run the deck in Radioss solver after saving the deck as Law2_Epspmax_crack.
   5. Repeat steps iv and v in Case 1. We find that the errors are well within the allowable range(Energy error(5 to -15%) AND Mass error(2 to 3%)) and thus the results are acceptable. Fig 10. Error check(energy err= 3.7%; mass err= 0%) Fig 11. Von mises stress contour Fig 12. Time vs IE_KE_CE_HGE_TE(mJ) Fig 13. Time vs resultant force(N) on the rigid sphere
3. Case 3: Simulate after removing the fail_johnson failure card.
   1. Import the given solver deck in Hypermesh.
   2. Go through the solver deck cards and properties and try to understand them.
   3. Delete the fail_johnson failure card. Go to the Radioss option under the Analysis menu and run the deck in Radioss solver after saving the deck as Law2_Epspmax_nofail.
   4. Repeat steps iv and v in Case 1. We find that the errors are well within the allowable range(Energy error(5 to -15%) AND Mass error(2 to 3%)) and thus the results are acceptable. Fig 14. Error check(energy err= 0.8%; mass err= 0%) Fig 15. Von mises stress contour Fig 16. Time vs IE_KE_CE_HGE_TE(mJ) Fig 17. Time vs resultant force(N) on the rigid sphere
4. Case 4: Simulate after removing both the failure plastic strain(Eps_p_max) and the fail_johnson failure card.
   1. Import the given solver deck in Hypermesh.
   2. Go through the solver deck cards and properties and try to understand them.
   3. Delete the failure card. Remove the Eps_p_max value from the material card. Go to the Radioss option under the Analysis menu and run the deck in Radioss solver after saving the deck as Law2.
   4. Repeat steps iv and v in Case 1. We find that the errors are well within the allowable range(Energy error(5 to -15%) AND Mass error(2 to 3%)) and thus the results are acceptable. Fig 18. Error check(energy err= 3%; mass err= 0%) Fig 19. Von mises stress contour Fig 20. Time vs IE_KE_CE_HGE_TE(mJ) Fig 21. Time vs resultant force(N) on the rigid sphere
5. Case 5: Simulate after changing the material law to Law1(Elastic).(Keep the same rho, E, nu values)
   1. Import the given solver deck in Hypermesh.
   2. Go through the solver deck cards and properties and try to understand them.
   3. Change the material law to Law1 which is for elastic materials. Enter the values for the density, young's modulus, and Poisson's ratio. Fig 22. Material block in the Radioss starter input file
   4. Go to the Radioss option under the Analysis menu and run the deck in Radioss solver after saving the deck as Law1.
   5. Repeat steps iv and v in Case 1. We find that the errors are well within the allowable range(Energy error(5 to -15%) AND Mass error(2 to 3%)) and thus the results are acceptable. Fig 23. Error check(energy err= 0.3%; mass err= 0%) Fig 24. Von mises stress contour Fig 25. Time vs IE_KE_CE_HGE_TE(mJ) Fig 26. Time vs resultant force(N) on the rigid sphere
6. Case 6: Simulate the model with material law27(check the new Eps based values)
   1. Import the Law27_0000.rad solver deck in Hypermesh.
   2. Go through the solver deck cards and properties and try to understand them. Fig 27(a). Material card Fig 27(b). Material block in Radioss Starter input file
   3. Notice the presence of new Eps based values such as the Eps_t1, Eps_m1, and Eps_f1. These values were not present in the Johnson cool material model.
   4. Go to the Radioss option under the Analysis menu and run the deck in Radioss solver after saving the deck as Law27.
   5. Repeat steps iv and v in Case 1. We find that the errors are well within the allowable range(Energy error(5 to -15%) AND Mass error(2 to 3%)) and thus the results are acceptable. Fig 28. Error check(energy err= 1.1%; mass err= 0%) Fig 29. Von mises stress contour Fig 30. Time vs IE_KE_CE_HGE_TE(mJ) Fig 31. Time vs resultant force(N) on the rigid sphere
7. Case 7: Simulate after changing to an aluminum material card(using law36)
   1. Import the given solver deck in Hypermesh.
   2. Go through the solver deck cards and properties and try to understand them. Fig 32(a). Material card Fig 32(b). Material block in Radioss Starter input file
   3. Change the material law to Law36(Plas_tab). Enter the requested values. We need to input a function curve. Create a new curve with the given data and assign it to the function. Fig 33. Creating a new curve
   4. Now run the analysis after saving it as Law36.
   5. Repeat steps iv and v in Case 1. We find that the errors are well within the allowable range(Energy error(5 to -15%) AND Mass error(2 to 3%)) and thus the results are acceptable. Fig 34. Error check(energy err= -1.4%; mass err= 0%) Fig 35. Von mises stress contour Fig 36. Time vs IE_KE_CE_HGE_TE(mJ) Fig 37. Time vs resultant force(N) on the rigid sphere

Result & discussion:

1. Case 1
   1. In case 1, we have both the Eps_p_max value as well as the fail_johnson Failure model defined. Fail_johnson is a ductile type failure model used in the case of ductile metals, mostly while using material Law2(Johnson cook material model) for the components.
   2. The fail_johnson failure model calculates the failure plastic strain using 5 parameters, D1, D2, D3, D4, and D5. If we neglect the effect of strain rate and temperature, then the relationship becomes, `ε _f = [ D _1 + D _2 exp ( D_ 3 σ ^∗ ) ]`. The values of D1, D2, and D3 are basically calculated in laboratory conditions by performing three typical loadings (example: pure tension, pure shear, or pure compression) and finding the respective failure strains. Thereafter, their values are derived using the above mentioned simple stress-strain relationship.
   3. How the failure happens is decided by the Ixfem value. A value of 0 will lead to the failed element getting deleted and a value of 1 will cause the element to fail by crack propagation. In the latter case, the crack advancement is decided by the Dadv value which can vary from 0 to 1. For this particular simulation, we can see that the elements have failed by element deletion as the Ixfem was defined as 0. We can also observe from the Von-mises stress contour animation that the maximum stress was generated on node 3812 and this was just before the rigid ball punched a hole in the plate(at ~4 ms).
   4. If we look into the Time vs Energy plots, we can clearly observe the internal energy of the plate increasing as the strain in the elements increases due to the impact of the rigid ball. At close to 4 ms, we can observe a dip in the internal energy which is accompanied by a rise in the Kinetic energy. This is because, at ~ 4 ms, the Rigid ball punched a hole in the plate and some of the elements got thrown away from the plate. The decrease in the Internal energy at that point in the simulation can be explained as the energy transferred to these thrown off elements in the form of Kinetic energy( explaining its rise during the same time period). Since the rigid ball has already punched through the plate, we do not see any further increase in both internal energy as well as the total energy. Throughout the simulation, we have recorded 0 Hourglass energy because of our choice to use QEPH shell formulation for the plate elements.
   5. The Time vs Resultant force(experienced by the rigid sphere) plot clearly shows the increase in the rigid wall forces during the impact. The fluctuations in the forces are due to the element deletion during the simulation. The great reduction of the resultant forces at ~4 ms reflects the event of the ball completely punching through the plate and thus experiencing reduced forces. Fig 38. Case 1 Result plots
2. Case 2
   1. In case 2, we have changed the Ixfem value to 1 and therefore the elements are failing by crack propagation. Here, the elements are not getting deleted right away but getting cracked on reaching the failure strain values. Therefore we can observe a delay in the deletion of elements during the simulation. The maximum stress is recorded for the node 4752 just before the elements break off from the plate.
   2. The Time vs Energy plots clearly shows the delay in element deletion. Here, unlike the previous case, the dip in internal energy is observed at ~4.6ms. Similar to case 1, this dip in internal energy can be explained by the gain in Kinetic energy of the elements that broke free from the plate due to failure. After ~ 4.6 ms, the energies have remained nearly constant as the ball has already punched a hole in the plate by this time. The hourglass energy and contact energy remained 0 throughout the simulation due to the choice of recommended shell element properties.
   3. If we look at the Time vs Resultant force(experienced by the rigid sphere) plot, it can be noticed that there was a rise in the resultant force during the impact, and failure of different elements during the simulation is reflected as small dips in the force plot. However, unlike case 1, where we got a single step reduction at ~ 4ms, here, we are observing force reduction in multiple steps and finally reaching the minimum at ~ 4.6ms. This can be explained by the fact that unlike case 1, the elements did not completely get deleted. Instead, cracks were developed. Also, we can see that a lesser number of elements have broken off from the plate in this case. Fig 39. Case 2 Result plots
3. Case 3
   1. In case 3, we have deleted the failure model. So, the elements are going to fails depending upon the Eps_p_max value defined in the material card, which in this case happens to be 0.151 or 15.1 % of plastic strain. Also, there won't be any cracks generated before element deletion. Maximum stress is observed on node 3804.
   2. The Time vs Energy plots clearly indicates the steady rise in Total energy and internal energy until the point in the simulation where elements are breaking off from the plate due to failure by Eps_p_max. After this large failure at ~ 4 ms, all the energies have remained nearly constant. Similar to the previous cases, we can observe a decrease in the internal energy and a corresponding increase in the kinetic energy at the moment the rigid sphere completely punches through the plate. Hourglass energy and contact energy are 0 throughout the run time.
   3. The Time vs Resultant force(experienced by the rigid sphere) plot shows a steep increase in the resultant forces at the beginning and then, as elements begin to fail and get deleted, the plot begins to fluctuate. The dips indicate the deletion of new elements. At ~ 4ms, there is a large dip in the plot as a result of many elements failing and breaking off from the plate. Fig 40. Case 3 Result plots
4. Case 4
   1. In case 4, the Eps_p_max value has also been removed. Thus there are no failure parameters defined for the plate and therefore, it will withstand infinite strain.
   2. The Energy plots have recorded a non-linear increase in both the internal energy and the total energy whereas the Kinetic energy and Hourglass energy have remained 0 throughout the simulation. The maximum stress was observed on node 3984 during the run time.
   3. Unlike the previous cases, the forces on the rigid sphere are seen to have continuously increased all throughout the simulation run time. The rate of increase of forces is larger during the initial stages of the impact. Fig 41. Case 4 Result plots
5. Case 5
   1. In case 5, we have changed the material model to Law1(elastic). In this case, the material is assumed to be undergoing an elastic deformation throughout the simulation. As a result, there is no failure of elements. The maximum stress was recorded on node 3688 during the run time. Note that even though no elements have failed in both cases 4 and 5, the maximum stress in case 5 is significantly higher than in case 4. This can be due to larger deformation in case 5 owing to the elastic behavior of the material.
   2. The energy plots are similar in shape to case 4 but the values are significantly higher. This is due to the higher amount of deformation in case 5 which has increased the internal energy to a much higher value than in case 4. The hourglass energy and contact energy have remained 0 in the run time.
   3. The resultant forces on the rigid sphere have also increased exponentially during the simulation. Fig 42. Case 5 Result plots
6. Case 6
   1. In case 6, we have changed the material model to Law 27. This law combines an isotropic elasto-plastic Johnson-Cook material model with an orthotropic brittle failure model. Material damage is accounted for prior to failure. Failure and damage occur only in tension. This law is applicable only for shells. In this model, the material behaves as a linear-elastic material when the equivalent stress is lower than the plastic yield stress. For higher stress values, the material behavior is plastic and the stress is calculated as: `σ = ( a + b ε_p^ n ) ( 1 + c ln ((ε˙) /(ε˙ _ 0)) )`. Where `ε_p` is the plastic strain and `ε˙` is the strain rate. The plasticity hardening exponent, n must be less than 1.
   2. Due to the brittle nature of the material, the plate can be seen to have cracked from the center to the edges during the simulation. Maximum stress was recorded on the node 3820. The stress contour animation shows a behavior similar to elastoplastic materials in cases 1, 2, and 3 up to nearly 4.1 ms after which the plate starts to show its brittle nature and the plate breaks into two pieces.
   3. The energy plots also justify the elasto-plastic to the brittle transformation of the plate. Here, even after the plate has broken into two pieces, unlike the previous cases, the internal energy and total energy curves did not flatten out. This is because of the existence of opposing elements that will continue to get strained further. HGE and CE have remained 0 throughout.
   4. The resultant forces on the rigid sphere are similar to that in case 1. However, the values have not decreased to zero during the run time. This is again due to the presence of opposing elements even after the plate has broken down into pieces. Fig 43. Case 6 Result plots
7. Case 7
   1. In case 7, we have changed the material to Law 36(Plas_Tab). This law models an isotropic elasto-plastic material using user-defined functions for the work-hardening portion of the stress-strain curve (for example, stress vs. plastic strain) for different strain rates. This material model allows us to use a user-defined function for strain rates.
   2. The maximum stress is recorded on node 3866 which also happens to be the first point of contact during the impact simulation. The element at the center fails and gets deleted. As more elements fail and the plate deforms during the simulation, the row of elements surrounding the rigid ball experiences increased strain and they get deleted abruptly. Now the elements at the center, which have not yet reached the failure plastic strain value are no longer connected to the rest of the plate. This is the reason why many elements are seen to break free from the plate at ~3.2 ms. This explains the similar break free behavior observed in the previous cases as well.
   3. The energy plots show a nearly linear increase in the internal energy and total energy until ~ 3.2 ms, after which there is a dip in the internal energy plot. From ~3.5 ms, the energy plots have flattened and remained constant for the rest of the run time. The hourglass energy and contact energy have remained 0 throughout the simulation in this case as well.
   4. The resultant forces on the rigid wall have increased rapidly up to ~0.6 ms and then we can see a dip which is due to the deletion of the center elements due to plastic strain failure. After this dip, the forces have fluctuated but have kept on increasing until ~ 3.2 ms. This is when a row of elements reached the failure strains and got deleted abruptly. The increase in forces up to this point (from 1 ms to 3.2 ms) can be assumed to be due to the increased resistance from the plate elements due to strain hardening. Thereafter, the forces can be seen to have reduced during rest of the run time. Fig 44. Case 7 Result plots

Result comparison summary:

1. Based on the total number of cycles, Errors, and simulation time.

   	No. of cycles	Energy error(%)	Mass error(%)	Simulation time(s)
   Case 1	49384	0.8	0	94.60
   Case 2	49407	3.7	0	97.51
   Case 3	49405	0.8	0	68.92
   Case 4	48737	3.0	0	69.00
   Case 5	47969	0.3	0	64.83
   Case 6	49356	1.1	0	75.54
   Case 7	53147	-1.4	0	75.45

2. Based on the animation and whether elements area getting deleted or cracked.

   	Animation	Failure method(Deletion or crack)
   Case 1		Deletion
   Case 2		Crack
   Case 3		Deletion
   Case 4		NA
   Case 5		NA
   Case 6		Deletion
   Case 7		Deletion

3. Based on the energy plots.

   	ENERGY PLOTS	Failure method(Deletion or crack)
   Case 1		1. A linear increase in both TE and IE till ~ 4ms. 2. A dip in IE and a corresponding rise in KE at approx. 4ms. 3. Nearly constant energy values after ~ 4ms. 4. HGE and CE remained 0 throughout.
   Case 2		1. A linear increase in both TE and IE till ~ 4.5ms. 2. A dip in IE and a corresponding rise in KE at approx. 4.5ms. There is a delay in this dip when compared to case 1. This is due to the delay in element deletion due to failure by cracking. 3. Nearly constant energy values after ~ 4.5ms. 4. HGE and CE remained 0 throughout.
   Case 3		1. A linear increase in both TE and IE till ~ 4ms. 2. A dip in IE and a corresponding rise in KE at approx. 4ms. 3. Nearly constant energy values after ~ 4ms. 4. HGE and CE remained 0 throughout.
   Case 4		1. A non-linear increase in both TE and IE throughout the simulation. 2. HGE and CE remained 0 throughout. 3. The maximum energy was ~65000 mJ.
   Case 5		1. An exponential increase in both TE and IE during the simulation. 2. HGE and CE remained 0 throughout. 3. The maximum energy was ~850000 mJ.
   Case 6		1. A linear increase in both TE and IE till ~ 4.2ms. 2. A dip in IE and a corresponding rise in KE at approx. 4.2ms. 3. Energy values continue to increase after ~4.2ms. 4. HGE and CE remained 0 throughout.
   Case 7		1. A linear increase in both TE and IE till ~ 3.2ms. 2. A dip in IE and a corresponding rise in KE at approx. 3.2ms. 3. Nearly constant energy values after ~ 3.5ms. 4. The maximum energy was ~45000 mJ. 5. HGE and CE remained 0 throughout.

Conclusion:

1. Successfully simulated all the 7 Cases without any error.
2. Discussed the results with the help of stress contour, Energy, and Resultant forces(experienced by the rigid sphere) plots.
3. Compared the results based on the requested parameters.
4. Which case would be appropriate in the actual physical event of a sphere crushing on to a similar metallic plate will depend upon the kind of plate material we are using. The cases 4 and 5 are not at all recommended as they are seen to have infinite strain failure limits. Case 6 will be the apt scenario if the class of aluminum we are using is having a brittle behavior. Cases 1 and 7 are realistic but if we have laboratory data for the strain loading on the material, Case 7 will give us more control, and thus Case 7 stands closer to the real-life scenario.

Find the completed files for each case by clicking here.