The following options are available under the Stress Analysis tab in the Project Settings dialog. These options can be used to customize the parameters which control the finite element stress analysis in Phase2.
Maximum Number of Iterations
The Maximum Number of Iterations controls the maximum number of iterations allowed in each Load Step. The default value is 500.
Tolerance
The Tolerance value defines the point at which the finite element solution is considered to have converged. The Tolerance for the stress analysis is a dimensionless parameter which represents the allowable unbalanced energy in the system, and corresponds to the Convergence Criterion (Absolute Energy or Square Root Energy). For a given Load Step:
If the energy imbalance of a current state (iteration) is less than the Tolerance value, then the solution is considered to have converged, and the iterations are stopped.
If the Tolerance value is not achieved within the specified Maximum Number of Iterations (i.e. energy imbalance remains greater than the Tolerance value), then the solution process is deemed not to have converged, for the specified convergence parameters.
For more information about Tolerance and convergence, see the Convergence Criteria document in the Phase2 theory section.
The default Tolerance is .001. The suggested range of values is .01 to .001. If your model is experiencing convergence problems, you can try increasing the Tolerance value in order to achieve convergence. However you must be aware that there can be many reasons why a model is not converging (often related to incorrect modeling procedures or input parameters), and increasing the Tolerance will not necessarily give you a correct answer, if your model is incorrect. Larger Tolerance values (e.g. .01) will speed up the solution time, but may give a less accurate solution. Smaller values (e.g. .0001) may give a more accurate solution, however, this will vary depending on the problem, and will increase computation time.
NOTE: for an elastic analysis (i.e. all materials are elastic), the Tolerance is not used since the solution is "exact". The Tolerance is only used for plasticity analysis (i.e. at least one material is defined as having plastic material properties).
Load Steps
By default, the Number of Load Steps used by COMPUTE at each stage is automatically determined by Phase2 (Number of Load Steps = Auto). The user can force COMPUTE to use a pre-determined Number of Load Steps, by entering a number from 1 to 30 in the Number of Load Steps option of Project Settings.
NOTE:
When Number of Load Steps = Auto, the number of Load Steps used at each stage will not necessarily be the same.
When a user-defined Number of Load Steps is entered, this number will be used AT EACH STAGE of calculation.
In general it is recommended that the user leave Number of Load Steps = Auto. Entering a user-defined Number of Load Steps is recommended for advanced users only.
Convergence Type
You may choose either Absolute Energy or Square Root Energy as the convergence criterion used for the finite element stress analysis. For details see the Convergence Criteria document in the Phase2 theory section.
Tensile Failure Reduces Shear Strength to Residual
There are two possible failure modes of a solid element in Phase2: tensile or shear. Either or both of these modes may occur in a given element.
If the Tensile failure reduces shear strength to residual checkbox is selected in Project Settings, then if tensile failure occurs at a point in a material (and shear failure has not already occurred), the shear strength of the material at that point will be automatically reduced to the residual shear strength parameters for that material. This is a realistic assumption to make, particularly for brittle materials.
It is important to note that this option is only applicable for materials where the material type = Plastic, and the residual strength parameters are less than the peak strength parameters.
This option will have NO effect for materials with the following parameters:
material type = Elastic, or
material type = Plastic, but the residual strength parameters are equal to the peak strength parameters (i.e. perfectly plastic material properties).
If the checkbox is NOT selected, then the shear strength parameters will NOT be reduced if tensile failure occurs in a material (i.e. the tensile and shear failure modes will be independent of each other).
NOTE: this feature was introduced as a user-configurable option in Phase2 version 5.047. In Phase2 versions 5.045 and 5.046, the option was automatically enabled in the Phase2 compute engine, but it could not be turned off by the user (i.e. the checkbox in Project Settings was not available). Prior to version 5.045, the option did not exist (i.e. equivalent to the checkbox being turned OFF). If you have files saved with previous versions of Phase2, you should run the analysis with this option turned OFF and then re-run the analysis with the option turned ON, to see if the analysis results are affected.
Joint Tension Reduces Joint Stiffness
The Joint Tension Reduces Joint Stiffness option allows you to specify a reduction factor for joint normal and shear stiffness, if a joint element is subjected to tensile stress normal to the joint. By default this option is ON with a default reduction factor of 0.01.
If this checkbox is turned OFF then tensile stress will NOT affect joint stiffness.