A kinda basic question regarding which material stress-strain data to use in Non-linear analysis.
If I choose Plastic Option in the Material -> Non-linear tab and want to associate a function as shown below:
Does the function can be a:
The question applies to SOL 106 & 601 as well. The understanding I have is that for SOL 106, engineering stress-strain curve can be used but for SOL 601, a true stress vs plastic strain is needed?
• With NX NASTRAN Basic Nonlinear (SOL106) the first type of nonlinear isotropic material is the NonLinear Elastic material (MATS1, TYPE=NLELAST). This material does not exhibit strain hardening or as the load is released on the material, the material simply releases it’s strain based on the strain vs. stress curve selected in the Function Dependence property. The function for nonlinear elastic materials should be defined in the first and third quadrants to accommodate different uniaxial tension and compression properties. Nonlinear elastic properties can only be defined for isotropic materials. It is important to note that the Femap function must be of the type "4..vs. Stress" as opposed to the more familiar Stress vs. Strain curve.
• The second nonlinear model of NX NASTRAN (SOL106) is the bi-linear Elasto-plastic curve: this material do exhibit strain hardening, it can also include mixed Isotropic+Kinematic hardening definitions. The Elasto-plastics material model can be used with any combination of small or large displacements and small or large strains. Elasto-plastic materials use the linear constants EX coupled with the plasticity modulus, H to define a bi-linear stress-strain curve with the work hardening slope, and is related to the tangential modulus, ET (the slope of stress vs. plastic strain).
The Yield Criterion option contains information on the yield types to be used. This box is only relevant for elasto-plastic and plastic nonlinearity types. Four yield criterion are available (von Mises, Tresca, Mohr-Coulomb, and Drucker-Prager). Von Mises and Tresca require input of the initial yield stress, while Mohr-Coulomb and Drucker-Prager require input of 2*cohesion and angle of internal friction.
• The final type of nonlinear isotropic model is the Multilinear Plastic material (MATS1, TYPE=PLASTIC). To specify this type of material, you specify an Initial Yield Stress, the Yield Criterion, and under FUNCTION DEPENDENCE the "4..vs. Stress" function which defines the strain vs. stress curve by multiple points. When TYPE = “PLASTIC”, the software interprets the stress-strain table as engineering stress and strain.
Thank you for the clarification.
So, I gather that for SOL 601, if I want to capture Plasticity effects accurately, I can create an engineering stress-strain function and ask the solver to convert it in to true stess-strain function using the CSVSSVAL parameter.
From your experience, is it recommended to use true stress-strain values for most engineering applications or just use engineering stress-strain values?
Again, per my understanding, true values are recommended if the intent is to capture response up to failure (like modeling the response of a test specimen etc) and engineering values are sufficient to find out response of the structure beyond elastic domain (not necessarily that the stress values may reach Ftu in the component).
Does the above makes sense?