- Mapdl.esurf(xnode='', tlab='', shape='', **kwargs)¶
Generates elements overlaid on the free faces of selected nodes.
APDL Command: ESURF
int]) – Node number that is used only in the following two cases:
Generates target, contact, and hydrostatic fluid elements with correct direction of normals.
- TOP - Generates target and contact elements over beam and
shell elements, or hydrostatic fluid elements over shell elements, with the normals the same as the underlying beam and shell elements (default).
- BOTTOM - Generates target and contact elements over beam
and shell elements, or hydrostatic fluid elements over shell elements, with the normals opposite to the underlying beam and shell elements.
If target or contact elements and hydrostatic fluid elements are defined on the same underlying shell elements, you only need to use this option once to orient the normals opposite to the underlying shell elements.
- REVERSE - Reverses the direction of the normals on
existing selected target elements, contact elements, and hydrostatic fluid elements. - If target or contact elements and hydrostatic fluid elements are defined on the same underlying shell elements, you only need to use this option once to reverse the normals for all selected elements.
Used to specify the element shape for target element TARGE170 (Shape = LINE or POINT) or TARGE169 elements (Shape = POINT).
- (blank) - The target element takes the same shape as the
external surface of the underlying element (default).
- LINE - Generates LINE or PARA (parabolic) segments on
exterior of selected 3-D elements.
POINT - Generates POINT segments on selected nodes.
The ESURF command generates elements of the currently active element type overlaid on the free faces of existing elements. For example, surface elements (such as SURF151, SURF152, SURF153, SURF154, or SURF159) can be generated over solid elements (such as PLANE55, SOLID70, PLANE182, SOLID185, or SOLID272, respectively).
Element faces are determined from the selected node set (NSEL) and the load faces for that element type. The operation is similar to that used for generating element loads from selected nodes via the SF,ALL command, except that elements (instead of loads) are generated. All nodes on the face must be selected for the face to be used. For shell elements, only face one of the element is available. If nodes are shared by adjacent selected element faces, the faces are not free and no element is generated.
Elements created by ESURF are oriented such that their surface load directions are consistent with those of the underlying elements. Carefully check generated elements and their orientations.
Generated elements use the existing nodes and the active MAT, TYPE, REAL, and ESYS attributes. The exception is when Tlab = REVERSE. The reversed target and contact elements have the same attributes as the original elements. If the underlying elements are solid elements, Tlab = TOP or BOTTOM has no effect.
When the command generates a target element, the shape is by default the same as that of the underlying element. Issue ESURF,,, LINE or ESURF,,,POINT to generate LINE, PARA, and POINT segments.
The ESURF command can also generate the 2-D or 3-D node-to-surface element CONTA175, based on the selected node components of the underlying solid elements. When used to generate CONTA175 elements, all ESURF arguments are ignored. (If CONTA175 is the active element type, the path Main Menu> Preprocessor> Modeling> Create> Elements> Node-to-Surf uses ESURF to generate elements.)
To generate SURF151 or SURF152 elements that have two extra nodes from FLUID116 elements, KEYOPT(5) for SURF151 or SURF152 is first set to 0 and ESURF is issued. Then KEYOPT(5) for SURF151 or SURF152 is set to 2 and MSTOLE is issued. For more information, see Using the Surface Effect Elements in the Thermal Analysis Guide.
For hydrostatic fluid elements HSFLD241 and HSFLD242, the ESURF command generates triangular (2-D) or pyramid-shaped (3-D) elements with bases that are overlaid on the faces of selected 2-D or 3-D solid or shell elements. The single vertex for all generated elements is at the pressure node specified as XNODE. The generated elements fill the volume enclosed by the solid or shell elements. The nodes on the overlaid faces have translational degrees of freedom, while the pressure node shared by all generated elements has a single hydrostatic pressure degree of freedom, HDSP (see HSFLD241 and HSFLD242 for more information about the pressure node).
- Return type