Comparision between different Material Laws in Radioss

Objective:-To simulate and compare the results of punching of a rigid ball against a rupture plate using different material laws using the following cases.

• Case 1;-Simulate the model without making any changes.[(Eps_P_max) and failure johnson cards enabled].

• Case 2:- Simulate the case, 1 model, by putting Ishell=1,Dadv=1,IXFEM=1 in the failure johnson card.

• Case 3:- Simulate case 2 by removing the failure johnson card.

• Case 4:- Simulate case 3 by removing the Eps_P_max card.

• Case 5:- SImulate case 4 by changing the material card to Law 1 keeping the same (Rho,Nu & E values).

• Case 6:- Simulate the model with Material Law 27.

• Case 7:- Simulate the model using Material Law 36.

Material laws used during this assignment.

• Law 1 (Linear Elastic Material) -{M1_ELAST}

1. This material law is used to model purely elastic materials. These materials fall in the complete elastic range. They obey Hooke's law, which states that stress is directly proportional to strain within elastic limits.

• Law 2 (Johnson-Cook Plasticity Model) -{M2_PLAS_JOHNS_ZERIL}

1. This material law is used to model elasto-plastic materials.These materials have linearly elastic behaviour when the equivalent stress is less than the yield stress.When the equivalent stress is exceeded by the yield stress they exhibit plastic behavior.Following the relation describing stress.

σ=(a+bεpn)(1+c1nε˙ε˙0)(1−T*m)

• Law 27 (Brittle Damage:Johnson-Cook Plasticity Model)-{M27_PLAS_BRIT}

1. This material law is used to model brittle failure.e.g (Crack Orientation,Layer Cracking). Following is the relation describing stress,

σn=σeff(1−d)

• Law 36 (Tabulated Piecewise Linear and Quadratic Elasto-plastic Law) -{M36_PLAS_TAB).

1. This material law is used to model elastic-plastic behaviour with a user defined work hardening curve.The hardening behaviour of the material is defined in function of plastic strain for a given strain rate.Following is the relation describing stress,

σγ=σγ0 (εp)×f(p)

Procedure:-

• Case 1:- Simulate the model without making any changes.[(Eps_P_max) and failure johnson cards enabled].

1. Import the FAILURE_JOHNSON_0000.rad solver deck into hypermesh.
2. Check the material properties of the model.
3. Once all the properties are checked, rename the file as Law2_Epspmax_Failure.Run the analysis of the model.[Analysis<Radioss].
4. Once solving is completed to check the energy errors open the Law2_Epspmax_Failure_0001.out file.

1. For the animation of the model import the h3d file of the model in Hyperview.Further contour can be set to von-mises to find out equivalent stress contour. Select the averaging method as simple.

1. For 2D energy and punch force plots import the T01 file into HyperGraph 2D.

What is Eps_P_max value?

EPS_P_Max is the maximum plastic strain value.If the value is increased beyond this value then element deletion takes place.

• Case 2:- Simulate the case, 1 model, by putting Ishell=1,Dadv=1,IXFEM=1 in the failure johnson card.

1. Import the solver deck into hypermesh & check the material properties.
2. In the failure johnson card update the following values Ishell=1,Dadv=1,IXFEM=1.
3. Rename & save the file as Law2_Epspmax_crack.
4. Follow steps 4-6 from case 1.

What is Ishell,Dadv,IXFEM?

1. Ishell is the shell failure value.Its value decides whether the failure should occur by element deletion orv crack.
2. Dadv is the crack advancement parameter. This parameter is active only when IXFEM flag is active.
3. IXFEM is the linear elastic failure mechanism.If active XFEM formulation takes place.

• Case 3:- Simulate case 2 by removing the failure johnson card.

1. Import the solverdeck into hypermesh.
2. In the model browser select the failure johnson card and delete it.
3. Rename & save the model as Law2_Epspmax_Nofail.
4. Repeat the steps 4-6 of case 1.

• Case 4:-Simulate case 3 by removing Eps_P_max card.

1. Import the solver deck into hypermesh.
2. Go to material properties of the model and delete the existing value of Eps_P_max parameter.
3. Rename & save the model as Law2_Epspmax_Nofail.
4. Repeat the steps 4-6 of case 1.

• Case 5:- Simulate case 4 by changing the material card to Law 1 keeping the same (Rho,Nu & E values).

1. Import the solverdeck into hypermesh.
2. Go to material properties of the model and change the material law to Law 1 (Linear Elastic Material) -{M1_ELAST}.Keeping the same Rho,Nu and E values.
3. Rename & save the model as Law1.
4. Repeat the steps 4-6 of case 1.

• Case 6:- Simulate the model with Material Law 27.

1. Import the Law27_0000.rad file into hypermesh.
2. Check the material properties and notice the unique parameters present.(Eps_m1,Eps_t1,Eps_f1).
3. Repeat the steps 4-6 of case 1.

What is Eps_m1,Eps_t1,Eps_f1 ?

1. Eps_m1 is Maximum tensile failure strain in principal strain direction 1 at which the stress in the element is set to a value dependent on dmax1.
2. Eps_t1 is a Tensile failure strain at which stress starts to reduce in the principal strain direction 1.
3. Eps_f1 is Maximum tensile strain for element deletion in principal strain direction 1.

• Case 7:- Simulate the model using Material Law 36.

1. Import the solver deck into hyperworks.
2. Go to material properties and change the material law to Law 36 (Tabulated Piecewise Linear and Quadratic Elasto-plastic Law) -{M36_PLAS_TAB).

1. Change the following values (N_funct = 1,Fscale=1,Eps_dot=1,fct_ID=test_curve,Fsmooth=0).
2. In the model browser right click on curves can create a curve named test_cuve with following coordinates.

X	Y
0	300
0.000484405	360.13
0.00111878	390.56
0.0032105	442.82
0.00478134	465.98

1. Repeat steps 4-6 of case 1 for post processing.

Results:-

• Energy Error and Mass Errors.

1. For case 1 the solver took 68.80 seconds & 49379 iterations to complete the solving process.The energy error was found out to be 0.8% and mass error was 0%.
2. For case 2 the solver took 106.27 seconds & 49216 iterations to complete the solving process.The energy error was found out to be 4.1% and mass error was 0%.
3. For case 3 the solver took 228.45 seconds & 49407 iterations to complete the solving process.The energy error was found out to be 0.8% and mass error was 0%.

• For case 4 the solver took 220.97 seconds & 48736 iterations to complete the solving process.The energy error was found out to be 3.0% and mass error was 0%.

• For case 5 the solver took 59.78 seconds & 47968 iterations to complete the solving process.The energy error was found out to be 4.1% and mass error was 0%.

• For case 6 the solver took 95.54 seconds & 49355 iterations to complete the solving process.The energy error was found out to be 1.1% and mass error was 0%.

• For case 7 the solver took 196.06 seconds & 41837 iterations to complete the solving process.The energy error was found out to be -1.8% and mass error was 0%.

• Element Failure Method.

1. For case 1,EPS_P_Max and failure johnson card(ductile failure model) are present.Since IXFEM=0,element failure takes place by element deletion method.
2. For case 2,IXFEM=1 & Dadv=1 therefore element failure takes place by crack formation.
3. For case 3, the failure card is deleted,so the element failure is governed by EPS_P_Max value.The EPS_P_Max value is 0.151,therefore the failure occurs at 15.1% of plastic strain.Failure takes place by element deletion.
4. For case 4,EPS_P_Max card is deleted.So there is no governing parameter for failure.The plate will handle infinite strain without any failure.
5. For case 5,the material law is changed to law 1.The element goes under elastic deformation throughout,so there will be no failure.
6. For case 6,the material law is law 27.Brittle failure model is present,element failure takes place by deletion.
7. For case 7,material consists of user defined work hardening curve.Element failure takes place by deletion.

• Energy Behaviour bases on energy plots.

1. Except case 5,all cases show almost linear increase in energies.Case 5 shows exponential increase due to elastic deformation.

Conclusion:-

1. Different material laws were studied and all the 7 cases were performed.
2. Results were observed by plotting curves in Hypergraph and animation in Hyperview.
3. By altering various parameters ,failure models and material cards respective changes were observed in the results.