Results from a contact analysis consist mainly of displacements, stresses, strains, reaction forces, and the contact information (contact pressure, sliding, and so on). You can review these results in POST1, the general postprocessor, or in POST26, the time-history postprocessor.
If you issued NLDIAG,CONT before solving the analysis, you can also view contact pair results which are saved to a text file named Jobname.cnd.
For contact-related results, you can select CONT as a plotting or list item. While in POST1, you can also review the results from within the Contact Manager (via the Contact Manager icon in the Standard Toolbar). See the "Output Data" section of the element descriptions (in the Element Reference) for the available output components.
In POST1, only one substep can be read in at a time. The results for the specified substep should have been written to Jobname.rst (or Jobname.rcn which contains the initial contact configuration calculated by CNCHECK,POST or the initial adjustments calculated by CNCHECK,ADJUST). The load step option command (OUTRES) controls which substep results are stored on Jobname.rst.
The following topics are available for reviewing contact results:
Following are important guidelines for postprocessing contact analysis results:
When postprocessing results obtained from a contact analysis, the database must be saved after the first solution is finished because the nodal connectivity of contact elements is updated and internal nodes are added during the solution.
To make sure you are viewing contact results for the correct substep, you should always postprocess results from the results file (Jobname.rst) and not from the database. Use the SET command in POST1 to read results from the results file.
In order to reduce the size of the results file, contact element results (such as temperature, ETABLE quantities, contact pressure, sliding, and so on) are not stored in the results file if the contact status is far-field. In this case, to correctly plot or list nodal temperatures at contact surfaces, you must select only the underlying elements before the plot or list operation.
When contact elements are included in a linear analysis (for example, a modal analysis), the contact is treated as linear (see Contact Behavior in Linear Analyses). The contact elements' stiffnesses are calculated based on their initial status and never change during the solution. Thus, the total forces contributed from contact elements (for example, FSUM,,CONT) in a linear analysis do not represent the actual physical values.
In a linear perturbation analysis, the program assumes that the initial status of the contact elements is the status at the completion of the static prestress analysis.
See also Hints and Tips in the Structural Analysis Guide.
The steps for reviewing results in POST1 are the same as those for a typical nonlinear analysis (see Reviewing Results in POST1 in the Structural Analysis Guide).
The following table shows the various contact (CONT) result items available via the PLNSOL and PLESOL commands.
| CONT | STAT | Contact status[1]:
| ||||
| " | PENE | Contact penetration | ||||
| " | PRES[2] | Contact pressure | ||||
| " | SFRIC[2] | Contact friction stress | ||||
| " | STOT[2] | Contact total stress (pressure plus friction) | ||||
| " | SLIDE | Contact sliding distance | ||||
| " | GAP | Contact gap distance | ||||
| " | FLUX | Heat flux at contact surface | ||||
| " | CNOS | Total number of contact status changes during substep | ||||
| " | FPRS | Fluid penetration pressure (surface-to-surface contact only) |
For MPC-based contact definitions, the value of STAT can be negative. This indicates that one or more contact constraints were intentionally removed to prevent over-constraint. STAT = -3 is used for MPC bonded contact. STAT = -2 is used for MPC no-separation contact. Negative values are valid for CONTA172, CONTA174, CONTA175, and CONTA177.
For the contact force-based model (used for CONTA175 with KEYOPT(3) = 0 and CONTA177 with KEYOPT(3) = 0 or 4), PRES, SFRIC, and STOT are the contact normal force, contact friction force, and total contact force, respectively.
For rigid-to-flexible contact or asymmetric flexible-to-flexible contact, the contact element provides the true pressure and friction stress. However, for symmetric flexible-to-flexible contact, the true pressure and friction stress is the average of the pressures and friction stresses from both sides of the contact elements.
Note: The contact results are only reported at the corner nodes of contact elements. PRNSOL, PRESOL, PLNSOL, and PLESOL only list/plot corner node results. Therefore, for higher order contact elements, mid-side node contact can occur without pressure being reported.
In this case, the element's contact status and contact pressure reported via ETABLE may give more precise information. In addition, contact pair-based summaries reported by CNCHECK,DETAIL, CNCHECK,POST, NLDIAG, and NLHIST include both corner and midside node information.
Also be aware that when the unified contact detection approach (KEYOPT(4) = 5) is used, only contact results of the standard surface projection method are reported at the corner nodes by PRNSOL, etc. However, the contact pair based summaries mentioned above include contact results at the integration points for all three of the detection methods employed by the unified contact detection approach.
Note that the contact-specific information (CONT) plots as follows. For 2D contact analyses, the model will plot in gray and the requested item will be contoured as an area (trapezoid) along the edge of the model where the contact elements are located. Use the FACT item to scale 2D contour size. For 3D contact analyses, the model will plot in gray and the requested item will be contoured as a 2D surface where the contact elements overlay the model.
For tabular listings, you may also list contact-specific information by using the CONT label and its arguments with the PRNSOL or PRESOL commands or their related menu items.
You should not use the PLESOL or PRESOL command to obtain contact forces for contact elements. The force values reported by these commands may not be accurate for these elements. Instead, use the ETABLE command to obtain contact force values.
Various sliding/slip quantities are reported through the ETABLE command. The table below described these quantities for the 3D case.
| TASS/TASR | Algebraic sum of sliding components in S and R directions when the contact status is sliding or sticking (STAT = 2, 3). |
| AASS/AASR | Absolute sum of sliding components in S and R directions when the contact status is sliding or sticking F(STAT = 2, 3). |
| SLIDE | Amplitude of total accumulated sliding [SQRT*(TASS**2 + TASR**2)] when the contact status is sliding or sticking (STAT = 2, 3). |
| GSLID | Amplitude of total accumulated sliding when the contact status is near-field, sliding, or sticking (STAT = 1, 2, 3). |
| ELSI | Total equivalent elastic slip. This represents the reversible tangential motion from the point of zero tangential stresses. |
| PLSI | Total equivalent tangential plastic slip. This represents the accumulated irreversible frictional sliding when the contact status is sliding (STAT = 2). |
| VREL | Equivalent sliding velocity (slip rate). |
The energies output for contact elements are not reported separately but are included in the element energies (for example, PLESOL,SEND) as follows:
Contact element strain energy (energy from enforcing contact non-penetration and sticking conditions) is included in the element strain energy (SEND,ELASTIC).
Friction dissipation is included in the element plastic energy (SEND,PLASTIC).
Damping energy is included in the element dissipation energy (SEND,VDAM).
You can animate contact results over time by using the ANTIME command (choose in the user interface).
A Jobname.rcn file is created if you issued CNCHECK,POST or CNCHECK,ADJUST during the analysis. You can use this file to view contact result items for the initial contact configuration (CNCHECK,POST) or initial adjustment values reported as structural displacement values (CNCHECK,ADJUST). To do so, you must explicitly read the results of the first load step from Jobname.rcn by issuing the FILE and SET,FIRST commands before postprocessing. Otherwise, the result file may be read improperly.
The steps for reviewing results in POST26 are the same as those for a typical nonlinear analysis See Reviewing Results in POST26 in the Structural Analysis Guide.
You can issue NLDIAG,CONT to monitor contact pair-based results during the solution according to a specified writing frequency (each iteration, substep, or load step). The resulting output is stored in a text file named Jobname.cnd. The following is a subset of information contained in this file that may be of interest:
| CFNX | Total force due to contact pressure - X component |
| CFNY | Total force due to contact pressure - Y component |
| CFNZ [2] | Total force due to contact pressure - Z component |
| CFSX | Total force due to tangential stress - X component |
| CFSY | Total force due to tangential stress - Y component |
| CFSZ [2] | Total force due to tangential stress - Z component |
| CTRQ [1] | Maximum torque in an axisymmetric analysis with MU = 1.0 |
For the 2D axisymmetric case, the maximum torque M (CTRQ) is defined as:
where p is the contact pressure, x is the x coordinate of the contact point on the interface, and s is the length domain of the contact interface. This definition of torque is associated with a friction coefficient of unity. It can be evaluated by scaling the friction coefficient for a particular contact pair. The reported torque M is useful in modeling threaded connectors.
For the case of 2D axisymmetric with torsion (KEYOPT(3) = 4), CFNZ and CFSZ represent moments along the Y direction.
See the NLDIAG command for a complete list of contact results written to Jobname.cnd.