Week-6 Calculate the Stretch Ratio by comparing the ELFORM (-2,-1,1,2) with Ogden_Material Model.

Objective:

• To create a block of 10mmx10mmx10mm dimension with 10 elements for each direction and use the material card attached (Ogden_Material.k) that is representative of the material properties from the below figure.
• To use appropriate boundary conditions to simulate tensile behavior for the model and finally compare the results from the simulation to the plot above up to stretch ratio 5. Only the uniaxial plot has to be compared.
• To compare the results for the simulation using ELFORM = 1, 2, -1, -2.

Introduction:

• The 'Ogden' material model is a material card modeled for a hyperelastic material. The hyperelastic material is commonly used to model mechanical behaviors of unfilled/filled elastomers. In addition to elastomers, hyperelastic material models are also used to approximate the material behavior of biological tissues, polymeric foams, etc.
•  The model was developed by Raymond Ogden in 1972. The Ogden model, like other hyperelastic material models, assumes that the material behavior can be described by means of a strain energy density function, from which the stress–strain relationships can be derived.
• In LS-DYNA, the output of stress and strains from Post>FringeComp, Stress/Strain is given as true stress and strains. The stretch ratio is defined as the ratio between the final length L and the initial length L0 of a component i.e. it is equal to (1 + engineering strain)

Procedure:

• The material file, 'Ogden_material.k', which was provided in the challenge was opened in "LS DYNA". The file did not have any part, but only the material keyword specified with certain standard values for a hyperelastic material.
• As specified in the challenge, a block with dimensions 10mm x 10mm x 10mm was created using the 'shape mesher' option which is available in the 'mesh' tab on the right side. The default values of 100 were changed to 10 and a solid block was created as shown in the image below.
  
  
  
  
  
• After creating the solid block, the boundary conditions were applied to it. Since the stretch ratio had to be compared only for the uni-axial tension test, the box had to be elongated only in any one of the directions or axes. One side of the box was fully fixed (constrained), while the other side was elongated. Here the X-axis was chosen for the elongation. On one of the faces of the X-axis, SPC (single point constraint) entities were created, and on the opposite face, a 'prescribed motion set' entity was created.
• For the SPC, all the nodes of the face were constrained in 4 directions, except the translational Y and Z. The nodes on central vertical line were constrained in the horizontal axis i.e. the Y-axis, while the nodes on the central horizontal line were constrained in the vertical axis i.e. the Z- axis in this case. If all the nodes of the face were constrained in all the 6 degrees of freedom, the elongation would not have been even throughout the block, instead there would have been a curved elongation right after the constrains. The image below shows the SPC entity creation.
  
  
  
  
  
  
• After creating the SPC, a node set was created from the 'create entity>set data>*SET_NODE', in which all of the nodes from the opposite face were added in order to define the displacement.
  
  
• A *DEFINE_CURVE keyword was created in order to define the load (displacement) curve from the keyword manager. This LCID would be used in the next step in the prescribed motion set keyword.  The curve data was as follows:
  0          0
  10.0     50
  10.1     50
  In this case, the termination time was decided to be 10 ms. Hence the values were plotted in this fashion in order to get a linear curve. It is good practice to add the load beyond the termination time in order to avoid any numerical instability and to get the loading till the end of the simulation. The image below shows the curve and the keyword.
  
  
  
  
• From the 'keyword manager', the *BOUNDARY_PRESCRIBED_MOTION_SET keyword was created and the node-set ID and the LCID created above were defined in this keyword. The DOF value was set a 1 for 'x-translation DOF, and the VAD value was set as 2 for 'displacement' as seen in the image below.
  
  
    
• Later, a section keyword was created in order to specify the section of the block. A *SECTION_SOLID was created from the 'keyword manager' with an element formulation 'ELFORM 1'.
  
  
  
  
• The material keyword card which was pre-specified was assigned to the solid block created. The material keyword was as shown below.
  
  
  
  
• After creating the section and material keyword, they were both assigned in the *PART to the block. In this case, the material that has been used for analysis is the Ogden material model which is a hyperelastic material model. Hyperelastic materials always behave non-linearly under loading. Therefore the type of analysis here becomes a non-linear analysis. The behavior of the model is not dependent on time, and the nature of loading is defined as displacement, instead of force, velocity, or acceleration. Hence analysis is almost static or quasi-static. Also, since the material is hyperelastic in nature, the strain rates during the analysis are negligible. Considering all these factors, the type of analysis had been chosen as Implicit Analysis. 
• Therefore, it has to be specified in the software that the analysis has to be done in implicit form. This is done by creating *CONTROL_IMPLICIT cards. There are different types of implicit keywords that are used to specify the implicit nature of the simulation. From the 'keyword manager', a *CONTROL_IMPLICIT_GENERAL was created in which the 'IMLAG' value was set as 1 which specifies the implicit type of analysis. The initial timestep 'DT0' was specified as 0.05 ms, as shown in the image below. 
  
  
  
  
• Along with this, a *CONTROL_IMPLICIT_AUTO keyword was created. This keyword is used to modify the timestep based on the state of the convergence of the model. The 'ITEOPT' defines the target value of iterations that are carried out to achieve convergence. The 'ITEWIN' parameter defines the iteration window or the tolerance values which alters the iteration numbers to achieve the convergence. In this case, all the values of these parameters were kept constant. The dtmin value was set as 0.0005, which is usually DT0/100, and the dtmax value was set as 0.5, which is usually DT0*10 as shown in the image below.
  
  
  
  
• In this challenge, the stretch ratio has to be calculated for which the strain values are required. Therefore, a *DATABASE_EXTENT_BINARY keyword was created, and the STRFLG value was kept as 1 which writes the strain tensor data to d3plot. Along with this the *DATABASE_ASCII_OPTION keyword was loaded and the cards for th glstat, matsum, sleout, etc. were created. 
  
  
  
  
• Later, a *CONTROL_TERMINATION keyword was created to specify the termination time of the simulation. The ENDTIM was specified as 10ms.
  
  
  
  
• After creating all the case setup and output requests, a final keyword check was performed on the model from 'keyword manager>model check>keyword check'. All the keywords were specified properly and were free of any errors, as shown in the image below.
  
  
• The keyword file was saved and the model was simulated in "LS RUN". Since it was an implicit analysis, convergence was achieved at the end of each step. For this, a number of iterations were performed till the equilibrium was achieved for that particular step. In the end, the termination was normal.
  
  
  
  
• The d3plot was opened in "LSPP" and the visual checks were performed. The contour for the von Misses stress was loaded from the 'fringe components' and the maximum value of VM stress was observed as 5.02 MPa.
  
  
  
  
• From the 'ASCII options', the 'glstat' file was loaded and different energy values like internal energy, kinetic energy, total energy, sliding energy, and damping energy values were plotted, as shown in the image below. Since the analysis was implicit and quasi-static in nature, the kinetic energy (A) was 0 throughout the simulation as there were no inertial effects. The maximum values of total and internal energy were the same at 4.25E3 Nmm.
• 
  
  
  
  
• Later the element formulation of the block was changed from the *SECTION_SOLID. The ELFORM value was set to -1 which stands for "fully integrated S/R solid intended for elements with poor aspect ratio, efficient formulation", while all th other keywords and parameters were kept constant.
  
  
  
  
• After saving this keyword file, the simulation was carried out in LSRUN and was carried out just like the previous one with a number of iterations to achieve convergence. The d3plot was opened in the LSPP and the von Misses stress contour was loaded. The maximum value of VM stress was equal to the previous case i.e. 5.023MPa. The animation below shows the VM contour.
  
  
  
  
• Similarly, by changing the element formulation, simulation was carried out for ELFORM -2, and ELFORM 2 as shown below.
  
  ELFORM -2:
  
  
  
  
  
  ELFORM 2:
  
  
  
  
  
• For both the above cases, the value of VM Stress was 5.022 MPa. After the simulation of all the 4 element formulations, the stretch ratios had to be compared to the plot which was provided in the challenge.
  
  
  
  
• In order to calculate the stretch ratio, engineering stress is required. But in LSPP the stress and strain values we get are true values. Therefore they have to be converted to engineering values. Following formulae had been used to calculate the stretch ratio:
  `sigma_t= sigma_e(1+epsi_e)`
  `sigma_e=sigma_t/((1+epsi_e)`
  `epsi_t=ln (1+ epsi_e)`
  `epsi_e=e^(epsi_t)-1`
  Stretch ratio, `lambda=1+epsi_e`
  Using these formulae stretch ratios were calculated for all the element formulations and the graphs were plotted in EXCEL.
  
  ELFORM 1:
  
   
  
  ELFORM -1:
  
   
  
  ELFORM -2:
  
   
  
  ELFORM 2: 
  
   
  
• It is evident from the above plots that the stretch ratios for all the element formulations were almost equal and the graphs have similar curves. The value of stress at the stretch ratio 5 in the original plot given for reference was around 1.8MPa. Whereas in our plot for the Ogden material model, the value of stress at the stretch ratio of 5 was only around 0.8MPa. Therefore it can be said that very low stress was generated in our models as compared to the original curve. It can also be seen that the shape of the curve was similar to the original reference curve only until the stretch ratio of 2. That is the stress value of 0.8 MPa was achieved right after the stretch ratio of 2 compared to that of 5 in our curves.

Conclusion:

• In this challenge, four element formulations, ELFORM 1, -1, -2, 2 was modeled and simulated in LSPP. Along with this the stretch ratios of all 4 formulations were compared. the calculations and the graph were done in Excel and are represented above. 
• In LSDYNA, the values of stresses or strains are true values. Hence these values were converted into engineering values and further calculations were done.
• This challenge was non-linear, quasi-static in nature. Hence the type of analysis chosen was implicit analysis. For this purpose, the two implicit keywords were applied, *CONTROL_IMPLICIT_GENERAL and *CONTROL_IMPLICIT_AUTO.

ADDITIONAL GDRIVE LINK FOR MODEL AND FILES: OGDEN MATERIAL STRETCH RATIO