- Mapdl.rsys(kcn='', **kwargs)#
Activates a coordinate system for printout or display of element and
APDL Command: RSYS nodal results.
The coordinate system to use for results output:
0 - Global Cartesian coordinate system (default, except for spectrum analyses).
1 - Global cylindrical coordinate system.
2 - Global spherical coordinate system.
> 10 - Any existing local coordinate system.
- SOLU - Solution coordinate systems. For element quantities, these are the element
coordinate system for each element. For nodal quantities, these are the nodal coordinate systems. If an element or nodal coordinate system is not defined, ANSYS uses the global Cartesian coordinate system. If you issue a LAYER,N command (where N refers to a layer number), the results appear in the layer coordinate system. (SOLU is the default for spectrum analyses.)
- LSYS - Layer coordinate system. For layered shell and solid elements, the results
appear in their respective layer coordinate systems. For a specific layer of interest, issue a LAYER,N command (where N refers to a layer number). If a model has both nonlayered and layered elements, you can use RSYS,SOLU and RSYS,LSYS simultaneously (with RSYS,SOLU applicable to nonlayered elements and RSYS,LSYS applicable to layered elements). To reverse effects of the LSYS option, issue an RSYS,0 command. LSYS is the default for spectrum analysis.
The RSYS command activates a coordinate system for printing or displaying element results data such as stresses and heat fluxes, and nodal results data such as degrees of freedom and reactions. ANSYS rotates the results data to the specified coordinate system during printout, display, or element table operations (such as PRNSOL, PRESOL, PLNSOL, and ETABLE). You can define coordinate systems with various ANSYS commands such as LOCAL, CS, CLOCAL, and CSKP.
If you issue RSYS with KCN > 10 (indicating a local coordinate system), and the specified system is subsequently redefined, you must reissue RSYS for results to be rotated into the redefined system.
Note:: : The default coordinate system for certain elements, notably shells, is not global Cartesian and is frequently not aligned at adjacent elements.
The use of RSYS,SOLU with these elements can make nodal averaging of component element results, such as SX, SY, SZ, SXY, SYZ, and SXZ, invalid and is not recommended.
The RSYS command has no effect on beam or pipe stresses, which ANSYS displays (via /ESHAPE,1 and PowerGraphics) in the element coordinate system.
Element results such as stresses and heat fluxes are in the element coordinate systems when KCN = SOLU. Nodal requests for element results (for example, PRNSOL,S,COMP) average the element values at the common node; that is, the orientation of the node is not a factor in the output of element quantities. For nearly all solid elements, the default element coordinate systems are parallel to the global Cartesian coordinate system. For shell elements and the remaining solid elements, the default element coordinate system can differ from element to element. For layered shell and layered solid elements, ANSYS initially selects the element coordinate system when KCN = SOLU; you can then select the layer coordinate system via the LAYER command.
Nodal results such as degrees of freedom and reactions can be properly rotated only if the resulting component set is consistent with the degree-of-freedom set at the node. (The degree-of-freedom set at a node is determined by the elements attached to the node.) For example, if a node does not have a UZ degree of freedom during solution, then any Z component resulting from a rotation does not print or display in POST1. Therefore, results at nodes with a single degree-of-freedom (UY only, for example) should not be rotated; that is, they should be viewed only in the nodal coordinate system or a system parallel to the nodal system. (The global Cartesian system–the RSYS command default–may not be parallel to the nodal system.) Results at nodes with a 2-D degree- of-freedom set (UX and UY, for example) should not be rotated out of the 2-D plane.
For PowerGraphics, ANSYS plots PLVECT vector arrow displays (such temperature, velocity, and force) in the global Cartesian coordinate system (RSYS = 0). Subsequent operations revert to your original coordinate system.
When you generate a .PGR file in SOLUTION, you can use the Results Viewer to display your stresses only in the coordinate system in which you write your .PGR file. To view stresses in other coordinate systems, load your results file into the Results Viewer and regenerate the data.
If large deflection is active (NLGEOM,ON), ANSYS rotates the element component result directions by the amount of rigid body rotation.
ANSYS displays the element component results in the initial global coordinate system for the following elements: SHELL181, SHELL281, ELBOW290, PLANE182, PLANE183, SOLID185, SOLID186, SOLID187, SOLID272, SOLID273, SOLID285, SOLSH190, SHELL208, and SHELL209. All other element result transformations are, therefore, also relative to the initial global system. Nodal degree-of-freedom results are based on the initial (and not the updated) geometry. For all other element types, component results displayed in the co-rotated coordinate system include the element rigid body rotation from the initial global coordinate system, and all other element result transformations are relative to the rotated global system.
You can use the RSYS command to rotate stress data for all explicit (ANSYS LS-DYNA) elements except BEAM161, COMBI165, and composite SHELL163 (KEYOPT(3) = 1). In models that contain these element types combined with other explicit elements, you must unselect the unsupported elements before issuing the RSYS command. The command does not support strain data for any explicit element types. If you request strain results for explicit elements when RSYS is not set to the global Cartesian coordinate system (KCN = 0), ANSYS ignores the printing or plotting command. (ANSYS always rotates displacements into the results coordinate system, independent of the explicit element type.)