Scope of Work-

There has been a high number of queries regarding the calculation of PEEQ Output variable (Equivalent Plastic Strain) in Abaqus.  I had a customer query wanting to know as to how PEEQ is determined.  In view of the high number of queries in regards to PEEQ calculation, this article is written and will cover PEEQ calculations for different scenarios.

PEEQ Calculation on the basis of PE (Plastic Strain Components) for Monotonic loadings

It is possible to determine the magnitude of PEEQ on basis of Plastic strain components. The corresponding simple formulae is “PEEQ = SQRT (2/3*((PE11*PE11+PE22*PE22+PE33*PE33) +0.5*(PE12*PE12+PE13*PE13+PE23*PE23)))”. The corresponding results when this formula is used is shown in the graph below (Graph 1).  

For certain elements, there might exist a small discrepancy between Abaqus queried PEEQ and PEEQ values determined through the above formulae. This could be a direct result of the fact that Abaqus would truncate and display values corresponding to only single-precision limits (PE values used in the formulae) whereas internal Abaqus calculations are done in double precision.

Although using the above formulae based upon Plastic strains is quite satisfactory for cases of Monotonic loading, this formulae might result in a fair bit of deviation between Abaqus determined PEEQ values and the PEEQ values got from the formulae for Sinusoidal loading cases as shown in the graph below (Graph 2). Hence, it can be safely said that the above formula can be successfully used only for Monotonic loading cases.  

From the above graphs, it is shown that PEEQ determined in Abaqus​​​​​​​ is an accumulative quantity (never decreases). However, the formulae 1 when used for Sinusoidal loading cases not only gives a deviation in results but also fails to predict the correct accumulative nature of PEEQ.

PEEQ Calculation on the basis of PE (Plastic Strain Components) for Sinusoidal loadings

The behavior that PEEQ values determined through the above formulae (formulae 1) does not correlate well with Abaqus queried PEEQ values for Sinusoidal loading cases is an expected one. This is because while individual Plastic Strain components (PE) go up during the loading phase and go down during the unloading phase, Abaqus PEEQ is an accumulative quantity. As visible in the below graph (graph 3) which contains output quantities directly queried from Abaqus, the plot for PEEQ becomes horizontal in some places and increases elsewhere but never decreases.

The formulae for PEEQ should be able to predict this cumulative nature of PEEQ. Hence, a slightly modified form of the already discussed equation which would take into account the rate of change of individual plastic strains and accumulation of PEEQ is presented below.

This equation can be successfully applied to Sinusoidal loading cases and also for Monotonic loading cases.

PEEQ Calculation on the basis of PENER and MISES Stress

Even after the usage of the modified formulae, there might exist discrepancies in PEEQ values for certain elements. This is because the formulae provided earlier works best for small deformation, i.e. nlgeom=no and not for large deformations.

As PEEQ is the strain equivalent of Von Mises Stress, an alternative approach based on Von-Mises stress and PENER (The plastic energy dissipated per unit volume) is possible and was presented to the customer. The formulae for PEEQ on basis of MISES stress and PENER is –
Similar to Mises stress, PEEQ is a non-negative scalar quantity. This equation-based upon PENER would be applicable to any case irrespective of it being Monotonic or Sinusoidal loading or it is small or large deformations.  The corresponding PEEQ values calculated by this approach correlates extremely well with the Abaqus queried PEEQ values. The results from this approach are shown below in Graph 4. 

Please Note: The formulae provided above may not hold for Kinematic Hardening cases.

Documentation Links for the definition of PEEQ : 

1. For classical metal plasticity, Please refer  Abaqus > Materials > Inelastic Mechanical Properties > Metal plasticity > Classical metal plasticity > References  

2. For metals subjected to Cyclic Loading, Please refer see   Reference > Library > Abaqus > Materials > Inelastic Mechanical Properties > Metal plasticity > Models for metals subjected to cyclic loading > Output  

Thanks and Best Regards.