Using ANSYS for Creep Analysis

by Carlos Shultz of PADT

Creep is a rate dependent material nonlinearity in which the material continues to deform under a constant load. The three stages of creep are shown in the figure below. ANSYS has the capability of modeling the first two stages (primary and secondary). The tertiary stage is usually not analyzed since it implies impending failure (gross element distortion).


Creep strain due to constant applied stress

ANSYS analyzes creep using two time integration methods. Both are applicable to static or transient analyses.

Implicit Creep

Implicit creep refers to the use of backward Euler integration for creep strains. This method is numerically unconditionally stable, which means that it does not require as small a time-step as the explicit creep method, so it is much faster overall.

For implicit creep plus rate-independent plasticity, the plasticity correction and creep correction are done at the same time, not independently. Consequently, implicit creep is generally more accurate than explicit creep, but it is still dependent on the time-step size. A small enough time-step must be used to capture the path-dependent behavior accurately.

The following example input shows the use of the implicit creep method. TBOPT=2 specifies that the primary creep equation for model 2 will be used. Temperature dependency is specified using the TBTEMP command, and the four constants associated with this equation are specified as arguments with the TBDATA command.

TB,CREEP,1,1,4,2
TBTEMP,T1
TBDATA,1,C1,C2,C3,C4

You can simultaneously model implicit creep and BISO, MISO, NLISO, BKIN, and HILL plasticity.

RATE command can be used to turn implicit creep on and off. Useful for setting up initial conditions prior to a creep analysis (plasticity is often active during the ramp up phase of a creep analysis).

/SOLU
RATE,OFF     !Creep calculations turned off
TIME,1.0E-8  !Time period set to a very small value
SOLVE        !First load step
RATE,ON      !Creep analysis turned on
TIME,T1      !Time period set to desired value
SOLVE        !Second load step

Enforce a creep limit ratio using the creep ratio control option in commands CRPLIM or CUTCONTROL, CRPLIMIT. A recommended value for a creep limit ratio ranges from 1 to 10.

Explicit Creep

Explicit creep means that the forward Euler method is used for the calculation of creep strain evolution. The creep strain rate used at each time step corresponds to the rate at the beginning of the time step and is assumed to be constant throughout that time step, Δt. Because of this, very small time steps are required to minimize error.

For explicit creep with plasticity, plasticity correction is performed first followed by creep correction. These two corrections occur at different stress values; therefore, it may be less accurate.

Explicit creep is no longer recommended for creep analysis. If you are learning to use creep in ANSYS, learn to use the implicit creep method.

Life Calculations for Creeping Components

Currently there is not a standard criterion for estimating the life of components subjected to various amounts of stress and temperature. Several different methods have been proposed; here are a few of them:

  1. Time-hardening rule, total accumulated creep strain is the sum of creep strains at each level of exposure, the “state” of the component moves along constant time from curve to curve, failure occurs when the part reaches the end of a curve
  2. Strain-hardening rule, differs from time-hardening in that the “state” moves along constant strain from curve to curve, failure occurs when the part reaches the end of a curve
  3. Life-fraction rule, differs from time-hardening in that the “state” moves from curve to curve by determining the ratio of exposure time to total life which has been used up to that time and then moving to the next curve at that same ratio, failure occurs when the part reaches the end of a curve

The life-fraction rule is considered intermediate to the time- and strain-hardening rules; these bound real life behavior. These rules are sometimes implied by the choice of creep law. If you use a time-hardening creep equation, you are assuming that the component follows a time-hardening rule. More complex relationships can be implemented through the use of user defined creep routines (please contact us for additional information regarding user creep routines).

General Recommendations

  1. Prevent fictitious stresses from causing convergence issues
    1. Use broad boundary conditions to hold components, fictitious stresses often occur when fixed displacements are applied
    2. Use pressures and accelerations to load components, fictitious stresses often occur when fixed forces are applied
    3. If fictitious stresses are unavoidable, create a layer of linear elements (without the creep material model active) between the high stresses and the rest of the model
  2. Test your creep model on a simple test case
    1. 3D bars with constant stress applied is my preferred test case
    2. Correlate by checking deflections vs time to verify that your model is correct
    3. Be aware that creep data is often constant load data that is presented as constant stress data, adjusting for this is not a simply task
  3. Solution Controls, turn SOLCON,on and use NSUBST,4,1e6,4
    1. Keep it simple, only adjust solution parameters if the defaults fail you
  4. Deflection limited analyses much easier than analysis of rupture
    1. Element distortion will cause convergence issues when trying to model failure
    2. Biasing the mesh, by making the elements thinner in the anticipated primary direction of stress, can delay mesh distortion since the loading will be deforming the elements into a better shape