prnsol

Mapdl.prnsol(item='', comp='', **kwargs)

Prints nodal solution results.

APDL Command: PRNSOL

Parameters:

item

Label identifying the item. Valid item labels are shown in Table 225: PRNSOL - Valid Item and Component Labels below. Some items also require a component label.

comp

Component of the item (if required). Valid component labels are shown in Table 225: PRNSOL - Valid Item and Component Labels below. Defaults to COMP.

Returns:

str

Str object with the command console output. This object also has the extra methods: to_list(), to_array() (only on listing commands) and to_dataframe() (only if Pandas is installed).
NOTE: If you use these methods, you might obtain a lower precision than using Mesh methods.
For more information visit Postprocessing.

Notes

Prints the nodal solution results for the selected nodes in the sorted sequence. For example, PRNSOL,U,X prints the X component of displacement vector U (that is, the UX degree of freedom). Component results are in the global Cartesian coordinate directions unless transformed (RSYS). Various element results also depend upon the recalculation method and the selected results location (AVPRIN, RSYS, LAYER, SHELL, and NSEL). If the LAYER command is issued, then the resulting output is listed in full graphics mode (/GRAPHICS,FULL). You can use the FORCE command to define which component of the nodal load (static, damping, inertia, or total) should be used.

PowerGraphics can affect your nodal solution listings. For PowerGraphics (/GRAPHICS,POWER), results are listed only for the model exterior surfaces.

When shell element types are present, results are output on a surface- by-surface basis. For shell elements, such as SHELL181 or SHELL281, and for ELBOW290, printed output is for both the top and bottom surfaces. For solid elements such as SOLID185, the output is averaged for each surface and printed as follows:

For a node at a vertex, three lines are output (one printed line for each surface).

For a node on an edge, two lines are output (one printed line for each surface).

For nodes on a face, one value is output.

For nodes interior to the volume, no printed values are output.

If a node is common to more than one element, or if a geometric discontinuity exists, several conflicting listings may result. For example, a corner node incorporating results from solid elements and shell elements could yield as many as nine different results; the printed output would be averages at the top and bottom for the three shell surfaces plus averages at the three surfaces for the solid, for a total of nine lines of output. ANSYS does not average result listings across geometric discontinuities when shell element types are present. It is important to analyze the listings at discontinuities to ascertain the significance of each set of data.

The printed output for full graphics (/GRAPHICS,FULL) follows the standard ANSYS convention of averaging results at the node. For shell elements, the default for display is TOP so that the results for the top of the shell are averaged with the other elements attached to that node.

If an NSORT, ESORT or /ESHAPE command is issued with PowerGraphics activated, then the PRNSOL listings will be the same as in full graphics mode (/GRAPHICS,FULL). The items marked with [2] are not supported by PowerGraphics. To print midside nodes, you must first issue an /EFACET,2 command.

Table: 225:: : PRNSOL - Valid Item and Component Labels

Failure criteria [2][4].

Default components: Maximum of all failure criteria defined at current location (MAX), maximum strain (EMAX), maximum stress (SMAX), Tsai-Wu Strength Index (TWSI), inverse of Tsai-Wu Strength Ratio Index (TWSR).