Element Type Definition

  FEMGEN will generate a finite element mesh of nodes and geometric element types. These geometric element types are related to the ANSYS element names via an element variant number. The element variant mappings for ANSYS may be displayed by using the FEMGEN command 'UTILITY TABULATE FE ANSYS', and these mappings are shown in tables 2.1 to 2.4. In addition, the user can now set their own default ANSYS element variants by defining them in a FEMGV resource file (see Chapter 1).

Element variants are assigned using the command 'MESHING TYPES part ELTYPE variantno'. The variant number is optional and the default is 1. It is also possible to specify an element variant by using its name directly, i.e. 'MESHING TYPES part PLANE82'.

Element types are defined in the input file with ANSYS 'ET' commands. The element type number is assigned by the interface program. The same element type can be defined twice with two different numbers if its material or/and physical properties are different from one to the other. The element type number is used in the ANSYS 'TYPE' command issued with the elements definition. The 'ET' command also includes element option keys (KEYOPT(n)), which are all set to their default values (usually 0) unless their value can be determined by the information input within FEMGEN. The element option keys defined by the interface program are:

• KEYOPT values for the analysis type, e.g. plane stress, plane strain, axisymmetric
• KEYOPT values determined from the physical properties entered
• KEYOPT values for optional mid-side nodes (e.g. SURF19 and SURF22)
• KEYOPT values determined from the type of thermal load (Heatflux or Convection)
• KEYOPT values determined from the material properties entered
• KEYOPT values for some optional degrees of freedom sets (structural degrees of freedom, or thermal, or coupled structural-thermal)

Eltype ANSYS Beam Type Element Variants

BE2 1 = BEAM3 2 = BEAM4 3 = BEAM23 4 = BEAM24

5 = BEAM44 6 = BEAM54 7 = PIPE16 8 = PIPE18

9 = PIPE20 10 = PIPE59 11 = PIPE60 12 = LINK1

13 = LINK8 14 = LINK10 15 = LINK11 16 = LINK31

17 = LINK32 18 = LINK33 19 = LINK34 20 = LINK68

21 = SHELL51 22 = SHELL61 23 = FLUID38 24 = FLUID66

25 = CONTAC12 26 = CONTAC52 27 = COMBIN14 28 = COMBIN39

29 = COMBIN40 30 = SURF19

BE3 1 = SURF19

 

Eltype ANSYS Plate/Shell Type Element Variants

TR3 1 = PLANE42 2 = PLANE13 3 = PLANE25 4 = PLANE55

5 = PLANE67 6 = PLANE75 7 = SHELL63 8 = SHELL41

9 = SHELL43 10 = SHELL57 11 = FLUID29 12 = HYPER56 13 = VISCO106

QU4 1 = PLANE42 2 = PLANE13 3 = PLANE25 4 = PLANE55

5 = PLANE67 6 = PLANE75 7 = SHELL63 8 = SHELL28

9 = SHELL41 10 = SHELL43 11 = SHELL57 12 = FLUID29

13 = FLUID79 14 = FLUID81 15 = HYPER56 16 = VISCO106

17 = SURF22 18 = FLUID15

TR6 1 = PLANE2 2 = PLANE35 3 = PLANE82 4 = PLANE53

5 = PLANE77 6 = PLANE78 7 = PLANE83 8 = SHELL93

9 = SHELL91 10 = SHELL99 11 = HYPER74 12 = HYPER84

13 = VISCO88 14 = VISCO108

QU8 1 = PLANE82 2 = PLANE53 3 = PLANE77 4 = PLANE78

5 = PLANE83 6 = SHELL93 7 = SHELL91 8 = SHELL99

9 = HYPER74 10 = HYPER84 11 = VISCO88 12 = VISCO108 13 = SURF22

 

Eltype ANSYS Brick Type Element Variants

PE6 1 = SOLID45 2 = SOLID5 3 = SOLID46 4 = SOLID64

5 = SOLID65 6 = SOLID69 7 = SOLID70 8 = SOLID73

9 = SOLID96 10 = FLUID30 11 = HYPER58 12 = HYPER86 13 = VISCO107

HE8 1 = SOLID45 2 = SOLID5 3 = SOLID46 4 = SOLID64

5 = SOLID65 6 = SOLID69 7 = SOLID70 8 = SOLID73

9 = SOLID96 10 = FLUID30 11 = FLUID80 12 = HYPER58

13 = HYPER86 14 = VISCO107

PE15 1 = SOLID95 2 = SOLID90

HE20 1 = SOLID95 2 = SOLID90

 

Eltype ANSYS Point Type Element Variants

P-EL 1 = MASS21 2 = MASS71

 

Note that some element types appear twice in the above tables as Ansys can allow various element shapes for one element type. For example, some plate/shell type elements can be defined either as quadrilateral (QU4, QU8) or triangular (TR3, TR6), and some brick type elements can be defined either as six-face solid (HE8, HE20) or wedge (PE6, PE15). Also element types such as SURF19 and SURF22 can be defined with or without mid-side nodes.