Element Properties

Marc > Building A Model > Element Properties

XXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXX''">XXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXX''">

Element Properties

The Element Properties application allows properties to be defined and assigned or associated to various groups of elements supported by the Marc Preference.

For more details on the Element Properties application, see Create Element Property Sets (p. 62) in the Patran Reference Manual.

The following table outlines the supported element types. For a list by Marc element number, see the next table.


Dimension	Type	Option 1	Option 2
• 0D (structural)(coupled)	• Mass
	• Spring/Damper
• 0D(thermal)	• Spring/Damper
• 1D (structural)(coupled)	• General Beam	• Straight	• Standard (Type varies) • General (Type varies)
		• Curved (Type varies)
	• Elastic Beam	• General Section	• Euler-Bernoulli (Type 52) • Euler-Bernoulli w/Shear (Type 98) • Straight Beam(Type 31)
		• Arbitrary Section	• Standard Formulation (Type 31) • Euler-Bernoulli w/Shear (Type 98)
		• Curved w/Arbitrary Section (Type 31) • Curved w/General Section (Type 31) • Curved w/Pipe Section (Type 31) • Pipe Section (Type 31)
	• Thin-Walled Beam	• Closed Section	• Standard Formulation (Type 14) • Linear Axial Strain (Type 25) • Shell Stiffener (Types 76, 78)
		• Open Section	• Standard Formulation (Type 13) • Shell Stiffener (Types 77, 79)
		• Pipe Section	• Standard Formulation (Type 14) • Linear Axial Strain (Type 25) • Shell Stiffener (Types 76, 78)
	• Planar Beam	• Homogeneous or Laminate	• Standard Formulation (Types 5, 45) • Parabolic Shear Strain (Type 45) • Curved Isoparametric (Type 16)
	• Spring/Damper	• Nonlinear (Type SPRING) • Linear (Type SPRING)
	• Axisym Shell	• Homogeneous or Laminate	• Standard Formulation (Types 1, 89) • Fourier (Types 90) • Isoparametric (Types 15)
• 1D (cont.)(structural)(coupled)	• Gap	• Fixed Direction (Type 12) • True Distance (Type 12) • Friction with Bending (Type 97)
	• Cable	• Initial Stress Input (Type 51) • Length Input (Type 51)
	• Truss (Types 9, 64) • Spring (Type SPRING) • Damper (Type SPRING)
	• Rebar	• Plane Strain (Types 165, 168) • Axisymmetric (Types 166, 169) • Axisymmetric w/Twist (Types 167, 170)
• 1D (thermal/ coupled)	• Axisym Shell	• Homogeneous or Laminate	• Linear Temp Distr (Types 87, 88) • Quadratic Temp Distr (Types 87, 88)

	• Link	• Magnetostatic (Type 183) • Conduction (Types 36, 65) • Convection/Radiation (Types 36, 65)
	• Spring/Damper (Type SPRING)
• 2D (structural)(coupled)	• Thin Shell	• Homogeneous or Laminate (Types 49, 72, 138, 139)
	• Thick Shell	• Homogeneous or Laminate	• Standard Formulation (Types 22, 75) • Reduced Integration (Type 140)
	• Membrane	• Homogeneous (Types 18, 30)
	• Shear Panel	• Homogeneous (Type 68)
	• 2D Rebar (Types 147, 148)
• 2D (cont.) (structural)(coupled)	• 2D Solid	• Axisymmetric	• Standard Formulation(Types 2, 10, 28, 126) • Hybrid(Herrmann) (Types 82,156,33,129) • Hybrid(Herrmann) / Reduced Integration (Types 59, 119, 156) • Hybrid(Herrmann) / Twist (Types 66, 83) • Reduced Integration (Types 55, 116) • Twist (Type 20, 67) • Laminated Composite (Types 152 / GASKET, 154) • Fourier (Type 62) • Hybrid(Herrmann) / Fourier (Type 63) • Reduced Integration / Fourier (Type 73) • Hybrid(Herrmann) / Reduced Integration / Fourier (Type 74) • Bending (Types 95, 96) • Semi-Infinite (Types 92, 94) • Electromagnetic (Type 112) • Piezoelectric (Type 162)
•	•	• Plane Stress	• Piezoelectric (Type 160)
•	•	• Plane Strain	• Standard Formulation (Types 6, 11, 27, 125) • Hybrid(Herrmann)(Types 32, 80, 128, 155) • Hybrid(Herrmann) / Reduced Integration (Types 58, 118, 155) • Reduced Integration (Types 54, 115) • Generalized (Types 19, 29) • Generalized / Reduced Integration (Type 56) • Generalized / Hybrid(Herrmann) (Types 34, 81) • Generalized / Hybrid(Herrmann) / Reduced Integration (Type 60) • Laminated Composite (Type 151 / GASKET, 153) • Semi-Infinite (Type 91 93) • Electromagnetic (Type 111) • Piezoelectric (Type 161)
•	•	• Plane Stress	• Standard Formulation(Types 3, 26, 124) • Reduced Integration (Types 53, 114)
• 2D (thermal	• Shell	• Homogeneous or Laminate	• Linear Temp Distr (Types 50 85, 86) • Quadratic Temp Distr (Types 50, 85, 86)

	• 2D Solid	• Axisymmetric	• Standard Formulation (Types 38, 40, 42, 132) • Reduced Integration (Types 70, 122) • Laminated Composite (Types 178, 180) • Semi-Infinite (Types 102, 104)
		• Planar	• Standard Formulation (Types 37, 39, 41, 131) • Reduced Integration (Types 69, 121) • Laminated Composite (Types 177, 179) • Semi-Infinite (Types 101, 103)
• 3D (structural)(coupled)	• Solid	• Standard Geometry	• Standard Formulation (Types 7, 21, 127, 134) • Hybrid(Herrmann) (Types 35, 84, 130, 157) • Hybrid(Herrmann) / Reduced Integration (Types 61, 120, 130, 157) • Reduced Integration (Types 57, 117, 127, 134) • Electromagnetic (Type 113) • Piezoelectric (Types 163 164) • Magnetstatic (Types 109 181 182)
		• Auto Shell Typing	• Standard Formulation (Types 7, 21) • Reduced Integration (Type 57)
		• Laminated Composite (Types 149 / GASKET, 150)
		• Semi-Infinite (Types 107, 108)
• 3D (thermal)	• Solid	• Standard Formulation (Types 43, 44, 133, 135) • Reduced Integration (Types 71, 123, 135) • Semi-Infinite (Types 105, 106) • Semi-Infiite - Magnetostatic (Type 110)
	• Laminated Composite (Types 175, 176)

Marc supported element types:


Element #	Description	Dimension	Topologies
• Element 1	Straight Axisymmetric Shell	1D	Bar/2
• Element 2	Axisymmetric Triangular Ring	2D	Tri/3
• Element 3	Plane Stress Quadrilateral	2D	Tri3/, Quad/4
• Element 4	Curved Quadrilateral, Thin Shell Element	2D	NOT SUPPORTED
• Element 5	Beam Column	1D	Bar/2
• Element 6	Two-Dimensional Plane Strain Triangle	2D	Tri/3
• Element 7	Three-Dimensional Arbitrary Distorted Brick	3D	Wedge/6, Hex/8
• Element 8	Curved Triangular Shell	2D	NOT SUPPORTED
• Element 9	Three-Dimensional Truss	1D	Bar/2
• Element 10	Arbitrary Quadrilateral Axisymmetric Ring	2D	Quad/4
• Element 11	Arbitrary Quadrilateral Plane-Strain	2D	Quad/4
• Element 12	Friction and Gap Link Element	1D	Bar/2
• Element 13	Open Section Thin-Walled Beam	1D	Bar/2
• Element 14	Thin Walled Beam in Three Dimensions without Warping	1D	Bar/2
• Element 15	Axisymmetric Shell, Isoparametric Formulation	1D	Bar/2
• Element 16	Curved Beam in Two-dimensions, Isoparametric Formulation	1D	Bar/2
• Element 17	Constant Bending, Three-node Elbow Element	1D	NOT SUPPORTED
• Element 18	Four-Node, Isoparametric Membrane	2D	Tri/3, Quad/4
• Element 19	Generalized Plane Strain Quadrilateral	2D	Tri/3, Quad/4
• Element 20	Axisymmetric Torsional Quadrilateral	2D	Tri/3, Quad/4
• Element 21	Three-Dimensional 20-Node Brick	3D	Wedge/15, Hex/20
• Element 22	Quadratic Thick-Shell Element	2D	Tri/6, Quad/8
• Element 23	Three-dimensional 20-node Rebar Element	3D	NOT SUPPORTED
• Element 24	Curved Quadrilateral Shell Element	2D	NOT SUPPORTED
• Element 25	Thin Walled Beam in Three Dimensions	1D	Bar/2
• Element 26	Plane Stress, Eight-Node Distorted Quadrilateral	2D	Quad/8
• Element 27	Plane Strain, Eight-Node Distorted Quadrilateral	2D	Quad/8
• Element 28	Axisymmetric, Eight-Node Distorted Quadrilateral	2D	Quad/8
• Element 29	Generalized Plane Strain, Distorted Quadrilateral	2D	Tri/6, Quad/8
• Element 30	Membrane, Eight-Node Distorted Quadrilateral	2D	Quad/8
• Element 31	Elastic Curved Pipe (Elbow) / Straight Beam	1D	Bar/2
• Element 32	Plane Strain Eight-Node Distorted Quadrilateral, Herrmann Formulation	2D	Quad/8
• Element 33	Axisymmetric, Eight-Node Distorted Quadrilateral, Herrmann Formulation	2D	Quad/8
• Element 34	Generalized Plane Strain Distorted Quadrilateral, Herrmann Formulation	2D	Tri/6, Quad/8
• Element 35	Three-Dimensional 20-Node Brick, Herrmann Formulation	3D	Wedge/15, Hex/20
• Element 36	Three-Dimensional Link (Heat Transfer Element)	1D	Bar/2
• Element 37	Arbitrary Planar Triangle (Heat Transfer Element)	2D	Tri/3
• Element 38	Arbitrary Axisymmetric Triangle (Heat Transfer Element)	2D	Tri/3
• Element 39	Planar Bilinear Quadrilateral (Heat Transfer Element)	2D	Quad/4
• Element 40	Axisymmetric Bilinear Quadrilateral Element (Heat Transfer Element)	2D	Quad/4
• Element 41	Eight-Node Planar Biquadratic Quadrilateral (Heat Transfer Element)	2D	Quad/8
• Element 42	Eight-Node Axisymmetric Biquadratic Quadrilateral (Heat Transfer Element)	2D	Quad/8
• Element 43	Three-Dimensional Eight-Node Brick (Heat Transfer Element)	3D	Wedge/6, Hex/8
• Element 44	Three-Dimensional 20-Node Brick (Heat Transfer Element)	3D	Wedge/15, Hex/20
• Element 45	Curved Timoshenko Beam in a Plane	1D	Bar/3
• Element 46	Eight-node Plane Strain Rebar Element	2D	NOT SUPPORTED
• Element 47	Generalized Plane Strain Rebar Element	2D	NOT SUPPORTED
• Element 48	Eight-node Axisymmetric Rebar Element	2D	NOT SUPPORTED
• Element 49	Finite Rotation Linear Thin Shell Element	2D	Tri/6
• Element 50	Three-Node Linear Heat Transfer Shell Element	2D	Tri/3
• Element 51	Cable Element	1D	Bar/2
• Element 52	Elastic Beam	1D	Bar/2
• Element 53	Plane Stress, Eight-Node Distorted Quadrilateral with Reduced Integration	2D	Tri/6, Quad/8
• Element 54	Plane Strain, Eight-Node Distorted Quadrilateral with Reduced Integration	2D	Tri/6, Quad/8
• Element 55	Axisymmetric, Eight-Node Distorted Quadrilateral with Reduced Integration	2D	Tri/6, Quad/8
• Element 56	Generalized Plane Strain, Distorted Quadrilateral with Reduced Integration	2D	Tri/6, Quad/8
• Element 57	Three-Dimensional 20-Node Brick with Reduced Integration	3D	Wedge/15, Hex/20
• Element 58	Plane Strain Eight-Node Distorted Quadrilateral with Reduced Integration Herrmann Formulation	2D	Tri/6, Quad/8
• Element 59	Axisymmetric, Eight-Node Distorted Quadrilateral with Reduced Integration, Herrmann Formulation	2D	Tri/6, Quad/8
• Element 60	Generalized Plane Strain Distorted Quadrilateral with Reduced Integration, Herrmann Formulation	2D	Tri/6, Quad/8
• Element 61	Three-Dimensional, 20-Node Brick with Reduced Integration - Herrmann Formulation	3D	Tet/10, Wedge/15, Hex/20
• Element 62	Axisymmetric, Eight-node Quadrilateral for Arbitrary Loading (Fourier)	2D	Tri/6, Quad/8
• Element 63	Axisymmetric, Eight-node Distorted Quadrilateral for Arbitrary Loading, Herrmann Formulation (Fourier)	2D	Tri/6, Quad/8
• Element 64	Isoparametric, Three-Node Truss	1D	Bar/3
• Element 65	Heat Transfer Element, Three-Node Link	1D	Bar/3
• Element 66	Eight-Node Axisymmetric Herrmann Quadrilateral with Twist	2D	Tri/6, Quad/8
• Element 67	Eight-Node Axisymmetric Quadrilateral with Twist	2D	Tri/6,Quad/8
• Element 68	Elastic, Four-Node Shear Panel	2D	Quad/4
• Element 69	Eight-Node Planar Biquadratic Quadrilateral w/ Reduced Integration (Heat Transfer Element)	2D	Tri/6, Quad/8
• Element 70	Eight-Node Axisymmetric Biquadrilateral with Reduced Integration (Heat Transfer Element)	2D	Tri/6, Quad/8
• Element 71	Three-Dimensional 20-Node Brick with Reduced Integration (Heat Transfer Element)	3D	Wedge/15, Hex/20
• Element 72	Bilinear Constrained Shell Element	2D	Quad/8
• Element 73	Axisymmetric, Eight-node Quadrilateral for Arbitrary Loading with Reduced Integration (Fourier)	2D	Tri/6, Quad/8
• Element 74	Axisymmetric, Eight-node Distorted Quadrilateral for Arbitrary Loading, Herrmann Formulation, with Reduced Integration (Fourier)	2D	Tri/6, Quad/8
• Element 75	Bilinear Thick-Shell Element	2D	Tri/3, Quad/4
• Element 76	Thin-Walled Beam in Three Dimensions without Warping	1D	Bar/3
• Element 77	Thin-Walled Beam in Three Dimensions including Warping	1D	Bar/3
• Element 78	Thin-Walled Beam in Three Dimensions without Warping	1D	Bar/2
• Element 79	Thin-Walled Beam in Three Dimensions including Warping	1D	Bar/2
• Element 80	Arbitrary Quadrilateral Plane Strain, Herrmann Formulation	2D	Quad/4/5
• Element 81	Generalized Plane Strain Quadrilateral, Herrmann Formulation	2D	Tri/3, Quad/4
• Element 82	Arbitrary Quadrilateral Axisymmetric Ring, Herrmann Formulation	2D	Quad/4/5
• Element 83	Axisymmetric Torsional Quadrilateral, Herrmann Formulation	2D	Tri/3, Quad/4/5
• Element 84	Three-Dimensional Arbitrary Distorted Brick, Herrmann Formulation	3D	Wedge/6/7, Hex/8/9
• Element 85	Four-Node Bilinear Shell (Heat Transfer Element)	2D	Quad/4
• Element 86	Eight-Node Curved Shell (Heat Transfer Element)	2D	Tri/6, Quad/8
• Element 87	Three-Node Axisymmetric Shell (Heat Transfer Element)	1D	Bar/3
• Element 88	Two-Node Axisymmetric Shell (Heat Transfer Element)	1D	Bar/2
• Element 89	Thick Curved Axisymmetric Shell	1D	Bar/3
• Element 90	Thick Curved Axisymmetric Shell--for Arbitrary Loading (Fourier)	1D	Bar/3
• Element 91	Linear Plane Strain Semi-infinite Element	2D	Quad/4
• Element 92	Linear Axisymmetric Semi-infinite Element	2D	Quad/4
• Element 93	Quadratic Plane Strain Semi-infinite Element	2D	Quad/8
• Element 94	Quadratic Axisymmetric Semi-infinite Element	2D	Quad/8
• Element 95	Axisymmetric Quadrilateral with Bending.	2D	Tri/3, Quad/4
• Element 96	Axisymmetric, Eight-node Distorted Quadrilateral with Bending	2D	Tri/6, Quad/8
• Element 97	Special Gap and Friction Link for Bending	1D	Bar/2
• Element 98	Elastic Beam with Transverse Shear	1D	Bar/2
• Element 99	Heat Transfer Link Element Compatible with Beam Elements	2D	NOT SUPPORTED
• Element 100	Heat Transfer Link Element Compatible with Beam Elements	2D	NOT SUPPORTED
• Element 101	Six-node Plane Semi-infinite Heat Transfer Element	2D	Quad/4
• Element 102	Six-node Axisymmetric Semi-infinite Heat Transfer Element	2D	Quad/4
• Element 103	Nine-node Planar Semi-infinite Heat Transfer Element	2D	Quad/8
• Element 104	Nine-node Axisymmetric Semi-infinite Heat Transfer Element	2D	Quad/8
• Element 105	Twelve-node 3-D Semi-infinite Heat Transfer Element	3D	Hex/8
• Element 106	Twenty-seven-node 3-D Semi-infinite Heat Transfer Element	3D	Hex/20
• Element 107	Twelve-node 3-D Semi-infinite Stress Element	3D	Hex/8
• Element 108	Twenty-seven-node 3-D Semi-infinite Stress Element	3D	Hex/20
• Element 109	Eight-node 3-D Magnetostatic Element	3D	Hex/8
• Element 110	Twelve-node 3-D Semi-infinite Magnetostatic Element	3D	Hex/12
• Element 111	Arbitrary Quadrilateral Planar Electromagnetic	2D	Quad/4
• Element 112	Arbitrary Quadrilateral Axisymmetric Electromagnetic Ring	2D	Quad/4
• Element 113	Three-dimensional Electromagnetic Arbitrarily	3D	Hex/8
• Element 114	Plane Stress Quadrilateral, Reduced Integration	2D	Tri/3, Quad/4
• Element 115	Arbitrary Quadrilateral Plane Strain, Reduced Integration	2D	Tri/3, Quad/4
• Element 116	Arbitrary Quadrilateral Axisymmetric Ring, Reduced Integration	2D	Tri/3 Quad/4
• Element 117	Three-Dimensional Arbitrary Distorted Brick, Reduced Integration	3D	Wedge/6, Hex/8
• Element 118	Arbitrary Quadrilateral Plane Strain, Incompressible Formulation with Reduced Integration	2D	Quad/4/5
• Element 119	Arbitrary Quadrilateral Axisymmetric Ring, Incompressible Formulation with Reduced Integration	2D	Quad/4/5
• Element 120	Three-Dimensional Arbitrarily Distorted Brick, Incompressible Reduced Integration	3D	Wedge/6/7, Hex/8/9
• Element 121	Planar Bilinear Quadrilateral, Reduced Integration (Heat Transfer Element)	2D	Tri/6, Quad/4
• Element 122	Axisymmetric Bilinear Quadrilateral, Reduced Integration (Heat Transfer Element)	2D	Tri/6, Quad/4
• Element 123	Three-Dimensional Eight-Node Brick, Reduced Integration (Heat Transfer Element)	3D	Wedge/6, Hex/8
• Element 124	Plane Stress, Six-Node Distorted Triangle	2D	Tri/6
• Element 125	Plane Strain, Six-Node Distorted Triangle	2D	Tri/6
• Element 126	Axisymmetric, Six-Node Distorted Triangle	2D	Tri/6
• Element 127	Three-Dimensional Ten-Node Tetrahedron	3D	Tet/10
• Element 128	Plane Strain, Six-Node Distorted Triangle, Herrmann Formulation	2D	Tri/6
• Element 129	Axisymmetric, Six-Node Distorted Triangle, Herrmann Formulation	2D	Tri/6
• Element 130	Three-Dimensional Ten-Node Tetrahedron, Herrmann Formulation	3D	Tet/10
• Element 131	Planar, Six-Node Distorted Triangle (Heat Transfer Element)	2D	Tri/6
• Element 132	Axisymmetric, Six-Node Distorted Triangle (Heat Transfer Element)	2D	Tri/6
• Element 133	Three-Dimensional Ten-Node Tetrahedron (Heat Transfer Element)	3D	Tet/10
• Element 134	Three-Dimensional Four-Node Tetrahedron	3D	Tet/4
• Element 135	Three-Dimensional Four-Node Tetrahedron (Heat Transfer Element)	3D	Tet/4
• Element 136	Six-node Wedge	3D	NOT SUPPORTED
• Element 137	Six-node Wedge Heat Transfer	3D	NOT SUPPORTED
• Element 138	Bilinear Thin-triangular Shell Element	2D	Tri/3
• Element 139	Bilinear Thin-shell Element	2D	Quad/4
• Element 140	Bilinear Thick-shell Element with Reduced Integration	2D	Tri/3, Quad/4
• Element 141	Heat Transfer Shell	2D	NOT SUPPORTED
• Element 142	Eight-node Axisymmetric Rebar Element with Twist	2D	NOT SUPPORTED
• Element 143	Four-node Plane Strain Rebar Element	2D	NOT SUPPORTED
• Element 144	Four-node Axisymmetric Rebar Element	2D	NOT SUPPORTED
• Element 145	Four-node Axisymmetric Rebar Element with Twist	2D	NOT SUPPORTED
• Element 146	Three-dimensional 8-node Rebar Element	3D	NOT SUPPORTED
• Element 147	Four-node Rebar Membrane	2D	Quad/4
• Element 148	Eight-node Rebar Membrane	2D	Quad/8
• Element 149	Three-dimensional, Eight-node Composite Brick Element	3D	Wed/6, Hex/8
• Element 150	Three-dimensional, Twenty-node Composite Brick Element	3D	Wed/15, Hex/20
• Element 151	Quadrilateral, Plane Strain, Four-node Composite Element	2D	Tri/3, Quad/4
• Element 152	Quadrilateral, Axisymmetric, Four-node Composite Element	2D	Tri/3, Quad/4
• Element 153	Quadrilateral, Plane Strain, Eight-node Composite Element	2D	Tri/6, Quad/8
• Element 154	Quadrilateral, Axisymmetric, Eight-node Composite Element	2D	Tri/6, Quad/8
• Element 155	Plane Strain, Low-order, Triangular Element, Herrmann Formulations	2D	Tri/3/4
• Element 156	Axisymmetric, Low-order, Triangular Element, Herrmann Formulations	2D	Tri/3/4
• Element 157	Three-dimensional, Low-order, Tetrahedron, Herrmann Formulations	3D	Tet/4/5
• Element 158	Three-node Triangular Membrane Element	2D	NOT SUPPORTED
• Element 159	Four-node Bilinear Thick Shell Element	2D	NOT SUPPORTED
• Element 160	4-node Piezo Electric Plane Stress Element	2D	Quad/4
• Element 161	4-node Piezo Electric Plane Strain Element	2D	Quad/4
• Element 162	4-node Piezo Electric Axisymmetric Element	2D	Quad/4
• Element 163	8-node Piezo Electric Brick Element	3D	Hex/8
• Element 164	4-node Piezo Electric Tetrahedron Element	3D	Tet/4
• Element 165	Two-node Plane Strain Rebar Membrane	1D	Bar/2
• Element 166	Two-node Axisymmetric Rebar Membrane	1D	Bar/2
• Element 167	Two-node Axisymmetric Rebar Membrane w/ Twist	1D	Bar/2
• Element 168	Three-node Plane Strain Rebar Membrane	1D	Bar/3
• Element 169	Three-node Axisymmetric Rebar Membrane	1D	Bar/3
• Element 170	Three-node Axisymmetric Rebar Membrane w/ Twist	1D	Bar/3
• Element 171	Two-node 2-D Cavity Surface Element	1D	NOT SUPPORTED
• Element 172	Two-node Axisymmetric Cavity Surface Element	1D	NOT SUPPORTED
• Element 173	Three-node 3-D Cavity Surface Element	2D	NOT SUPPORTED
• Element 174	Four-node 3-D Cavity Surface Element	2D	NOT SUPPORTED
• Element 175	Eight-node Composite Heat Transfer Brick Element	3D	Wed/6, Hex/8
• Element 176	Twenty-node Composite Heat Transfer Brick Element	3D	Wed/15, Hex/20
• Element 177	Four-node Plane Strain Composite Heat Transfer Element	2D	Tri/3, Quad/4
• Element 178	Four-node Axisymmetric Composite Heat Transfer Element	2D	Tri/3, Quad/4
• Element 179	Eight-node Plane Strain Composite Heat Transfer Element	2D	Tri/6, Quad/8
• Element 180	Eight-node Axisymmetric Composite Heat Transfer Element	2D	Tri/6, Quad/8
• Element 181	3D Magnetostatic Tetrahedron	3D	Tet/4
• Element 182	3D Magnetostatic Tetrahedron	3D	Tet/10
• Element 183	3D Magnetostatic Current Carrying Wire	3D	Bar/2

Element Input Properties

This is an example of one of many Input Properties forms that can appear when defining element properties.

For a list of supported Marc element types, see (p. 126). The input properties for each Marc element type are listed below. They are listed in order of dimension as follows:


0D Elements	2D Elements
1D Elements	2D Solid Elements
1D Shell/Membrane Elements	3D Elements

0D Elements

Mass

This input data creates the MASSES keyword option. These act in the analysis coordinate frame of the node.


Property Name	Description
Translational Inertia, X/Y/Z	Defines the concentrated mass values for translational degrees-of-freedom. These properties are optional and can be entered either as real constants or references to existing field definitions. They appear on the third card of the MASSES option.
Rotational Inertia XX/YY/ZZ	Defines the rotational inertia values for rotational degrees-of-freedom. These properties are optional and can be entered either as real constants or references to existing field definitions. They appear on the third card of the MASSES option.

Spring/Damper

See Spring/Damper under 1D Elements.

1D Elements

Beams, Bars, Pipes, Trusses

This input data creates the Marc element types 5, 9, 13, 14, 16, 25, 31, 45, 52, 64, 76, 77, 78, 79, or 98. The properties entered into the Input Properties form fill out the necessary information in the GEOMETRY and/or BEAM SECT and NODAL THICKNESS keyword options of the Marc input file. The properties presented to you in the form are dependent on the element type to be created.
Spatial fields can be defined and referenced in various properties to denote that a property value varies with element position or length such as thickness or cross sectional area. See Fields - Tables for
more information.

Note that the General Beam selection behaves differently than the other selections such as Elastic Beam, Planar Beam or Thin-Walled Beam. The General Beam attempts to be smart and determine which beam element is the most appropriate for your particular application, whereas the other beam selection types will give you the beam that you ask for. If you don’t know what Marc beam element to use, we suggest you simply use General Beam and let the application determine the best fit. The logic at the right is used to determine the appropriate element type:

A list of all properties for beam/bar/pipe/ truss elements are given below. Only those applicable to the particular type of element appears on the Input Properties form.


Property Name	Description
Section Name	Defines the section to be used from a list of sections created or stored in the Beam Library. A list of all sections (currently in the database) is displayed. Either select from the list or type in the name. This property is required and only appears for General Beam. For other methods of assigning beam properties, a button at the bottom of the form allows you to select an existing beam section, but the section name is not associated to the property itself as is the case for General Beam.
Material Name	Defines the material to be used. A list of all materials (currently in the database) is displayed. Either select from the list or type in the name, preceded by an “m:”. This property is required.
XZ Plane Definition	Defines the orientation of the beam elements. This vector determines the plane that contains the local x-axis and the beam axis. The components of the vector appear in the EGEOM4, 5, and 6 data fields of the GEOMETRY option. This property is required.
Center of Curvature	Defines the center of the bend radius by referencing the ID of an existing node. The coordinates of the node appear in the EGEOM3, 4, and 5 data fields of the GEOMETRY option. This property is required for curved beams.
Cross-Sectional Area	Defines the area of the beam or truss cross section. It can be entered as a real constant or a reference to an existing field definition. For a truss element, the value appears in the EGEOM1 data field of the GEOMETRY option or in the second data field on the third card of the BEAM SECT option for beams/bars/pipes, and is a required property.
Section Radius (ave)	Defines the radius measured from the pipe center to the middle of the pipe wall. It can be entered either as a real constant or a reference to an existing field definition. The value appears in the EGEOM2 data field of the GEOMETRY option, and is a required property for pipe elements.
Section Height	Defines the beam thickness either as element uniform or tapered based on the selected “Value Type.” Real Scalar: Each element will have a uniform thickness which can be entered as a real constant, or a reference to an existing field definition. The data appears in the EGEOM1 data field of the GEOMETRY option. Field at Nodes: Tapered elements will be created by referencing an existing field definition. The data appears on the third card of the NODAL THICKNESS option. This property is required.
Section Width	Defines the beam section area for Bar/2 elements or beam section width for Bar/3 elements. It can be entered either as a real constant or a reference to an existing field definition. The value appears in the EGEOM2 data field of the GEOMETRY option, and is a required property.
Pipe Thickness	Defines the pipe wall thickness for pipe elements. It can be entered either as a real constant or a reference to an existing field definition. The value appears in the EGEOM1 data field of the GEOMETRY option, and is a required property for pipe elements.
Shear Area-x Shear Area-y	Defines the effective transverse shear area in the local x and y directions. They can be entered as a real constants or references to existing field definitions. The values appear in the sixth and seventh data fields on the third card of the BEAM SECT option.
Ixx Iyy	Defines the moments of inertia about the local x and y axes. They can be entered either as real constants or references to existing field definitions. The values appear in the fourth and fifth data fields on the third card of the BEAM SECT option, and are required properties.
Izz (K factor)	Defines the torsional stiffness factor. It can be entered either as a real constant or a reference to an existing field definition. The value appears in the fifth data field on the third card of the BEAM SECT option, and is a required property.
# Divisions ea Branch	Defines the number of divisions for each branch of the beam cross section for stress recovery. This data is entered as a list of integer constants - one value for each branch. The values appear on the third card of the BEAM SECT option, and are required properties. Each branch is divided (by you) into segments. The stress points of the section, that is, the points used by numerical integration of section stiffness and also for output of stress, are the segment division points. The end points of any branch are always stress points, and there must always be an even number of divisions (nonzero) in any branch. A maximum of 31 stress points (30 divisions) can be used in a complete cross-section, not counting branches of zero thickness.
X @ Begin 1st Branch Y @ Begin 1st Branch	Defines the coordinates at the beginning of the first branch in the beam cross section. These real constants appear in the first and second data fields on the fourth card of the BEAM SECT option, and are required properties.
[dx/ds @ Branch Begin] [dy/ds @ Branch Begin]	Defines the direction cosines of the tangent at the beginning of each branch relative to the local x and y axes. These lists of real constants are optional. The default directs the branch in a straight path between its ends and only operates when neither list is provided. When values are entered, they must be greater than or equal to -1.0 and less than or equal to +1.0. This data appears on the fourth card of the BEAM SECT option.
Thkns @ Branch Begin	Defines the thickness at the beginning of each branch. These real constants must have values that are greater than or equal to zero (branches with zero thickness can be used to double back over existing branches). They are entered on the fifth card of the BEAM SECT option, and are required properties.
X @ Branch End Y @ Branch End	Defines the coordinates at the end of each branch in the beam cross section. These real constants appear in the fifth and sixth data fields on the fourth card of the BEAM SECT option, and are required properties. The end branch location is always the beginning branch location for the next branch. In some cases, to define a proper cross section, the branches must overlap back onto themselves. In this case, the overlapping branch is assigned a zero thickness.
[dx/ds @ Branch End] [dy/ds @ Branch End]	Defines the direction cosines of the tangent at the end of each branch relative to the local x and y axes. These lists of real constants are optional. The default directs the branch in a straight path between its ends and only operates when neither list is provided. When values are entered, they must be greater than or equal to -1.0 and less than or equal to +1.0. This data appears on the fourth card of the BEAM SECT option.
Thkns @ Branch End	Defines the thickness at the end of each branch. These real constants must have values that are greater than or equal to zero (branches with zero thickness can be used to double back over existing branches). They are entered on the fifth card of the BEAM SECT option, and are required properties. If the thickness at the beginning of the branch is nonzero and the end is defined as zero, the branch is assumed to be of constant thickness.
[Contact Beam Radius]	Defines the radius of the beam for beam-to-beam contact purposes. This value is unnecessary for MSC.Marc versions 2001 and earlier in which the contact distance between touching beams is calculated automatically. However this radius is required for Marc 2003 if beam-to-beam contact is involved. The radius is entered in the 7th filed of the GEOMETRY option.
[Branch Length]	Defines the length of each branch. These real constants are optional. The default value is equal to the straight distance between the ends of the branch. They are entered on the fifth card of the BEAM SECT option.
[Transverse Shear]	If this is set to Parabolic, then the TSHEAR parameter is written, which changes the transverse shear model from constant through the thickness to a parabolic representation for planar beam, element type 45.
[Rigidity]	In a Coupled analysis, if this is set to Rigid, the element exhibits only heat transfer capabilities and becomes structurally rigid.


Note:	For most beam elements, you can select existing section and property data from the Beam Library which is an application under the Tools pull down menu. When this is done, the appropriate data boxes are filled in with the section properties automatically. In some cases this is property data while others it is branch information. For the General Beam, all this information is filled out, however, only the data needed for the selected element type is written to the Marc input file. For arbitrary beam section types, the Beam Library allows entry in the form of branch (or centerline) data. It is highly recommended to use the Beam Library to define this data as it is much easier.

Spring/Damper

This input data creates the SPRINGS keyword option in the Marc input file. Properties that can vary spatially (or nonspatially) are defined by referencing a spatial (or nonspatial) field (table). See Fields - Tables for more information.

Currently there are three selection for creating the SPRINGS keyword: Spring/Damper, Spring, or Damper. The latter two are somewhat obsolete in that they only allow you to define a linear spring or a linear damper. The Spring/Damper allows you to define both a linear or nonlinear combination spring/damper and is thus much more versatile and the recommended method. Nonlinear springs which reference nonspatial fields of force vs deflection are only valid for Marc version 2003 and beyond. Spring/dampers used in Thermal analysis only act as rigid links with thermal conduction. Linear spring/dampers cannot accept spatially or nonspatially varying fields.


Property Name	Description
Dof at Node 1 Dof at Node 2	Defines the degree-of-freedom to use at each end of the spring element. They are entered in the second and fourth data fields on the second card of the SPRINGS option, and are required properties. For 0D Objects, the D0f at Node 2 is not available and thus not entered to flag a grounded spring/damper.
Stiffness	Defines the spring stiffness. It can be entered either as a real constant or a reference to an existing nonspatial field definition of Force vs Deflection or Stiffness vs. Deflection for nonlinear springs only, which can vary with time and/or temperature also. The scalar value or unity appears in the 5th field on the 2nd data block of the SPRINGS option with a reference to a TABLE entry. The old, 1d linear Spring definition can accept a spatially varying field in which case multiple SPRINGS options are written to describe the spatial variation of stiffness.
Damping Coefficient	Defines the damping coefficient. It can be entered either as a real constant or a reference to an existing nonspatial field definition of Force vs Velocity or Coefficient vs. Velocity for nonlinear dampers only, which can vary with time and/or temperature also. The scalar value or unity appears in the 6th field of the 2nd data block of the SPRINGS option with a reference to a TABLE entry. The old, 1d linear Damper definition can accept a spatially varying field in which case multiple SPRINGS options are written to describe the spatial variation of damping.
Initial Force	This is a real scalar value of initial force in the spring. This cannot vary via a field definition. The scalar value appears in the 7th field of the 2nd data block of the SPRINGS option
Thermal Conduction	Defines the thermal conductivity for Thermal or Coupled analyses. It can be entered either as a real constant or a reference to an existing nonspatial field definition of Flux vs Temperature or Conduction vs. Temperature for nonlinear links only, which can vary with time also. The scalar value or unity appears in the 8th field on the 2nd data block of the SPRINGS option with a reference to a TABLE entry.
Numerical Stabalizer	This is a flag that, if set, will cause the spring to act as a numerical stabalizer and the spring force will always be set to zero.

Gaps

This input data creates Marc element type 12 and 97 (Friction and Gap Link), and the associated GAP DATA keyword options. The 7th data field on the third card of the GAP DATA option is set to zero (0) to indicate fixed direction input or to one (1) to indicate true distance input. The two connectivity nodes become the first and fourth nodes of the element. The second and third nodes are created during translation. The 3rd node uses the defaults for its coordinates, which define the friction directions. Properties that can vary spatially are defined by referencing a spatial field (table). See Fields - Tables for more information.


Property Name	Description
Init Open or Closed	Indicates the condition of the gap for the first iteration of the analysis. This data is optional and will default to initially open if not defined. It is entered in the 8th data field on the third card of the GAP DATA option.
Limiting Distance Closure Distance	Indicates that the “Limiting Distance” restricts the minimum or maximum opening of the gap. This property is optional and defaults to the minimum limit type. For “Closure Distance,” this data is place in the 1st field of the GAP DATA option.
Min or Max Limit Type	Defines a minimum or maximum restriction on the gap distance based on the selection made for “Min or Max Limit Type.” It can be entered either as a real constant or a reference to an existing field definition. The value appears in the first data field on the third card of the GAP DATA option.
Friction Coefficient	Defines the sliding friction coefficient when the gap is closed. This property is optional and defaults to zero when not defined. It can be entered either as a real constant or a reference to an existing field definition. The value appears in the second data field on the third card of the GAP DATA option.
K Normal (closed) K Tangent (closed)	Defines the normal and tangential stiffness of the element when the gap is closed. They can be entered either as real constants or references to existing field definitions. The values appear in the third and fourth data fields on the third card of the GAP DATA option.
Closure Direction	This is a vector that defines the closure direction and used only for Fixed Direction gaps. Note that this element is actually a 4 node element although only Bar/2 topologies are allowed. The two internal nodes are generated automatically by the translation. The first and fourth nodes couple to the rest of the structure while node 2 is the gap node. It has one degree of freedom, Fn, the force being carried across the link. The coordinate data of this node is used to input the direction of the gap closure direction and determined from this vector. Node 3 is the frictional node, which is automatically supplied by the translator. This property is required.

Cable

This input data creates Marc element type 51 (Cable Element). The GEOMETRY option is used to define the cross-sectional area and the initial length. Properties that can vary spatially are defined by referencing a spatial field (table). See Fields - Tables for more information.


Property Name	Description
Material Name	Defines the material to be used. A list of all materials (currently in the database) is displayed. Either select from the list or type in the name, preceded by an “m:”. This property is required.
Cross-Sectional Area	Defines the area of the cable cross section. It can be entered either as a real constant or a reference to an existing field definition. The value appears in the EGEOM1 data field of the GEOMETRY option, and is a required property.
Initial Stress	Defines the initial stress in the cable elements.This property is optional and will default to zero when not defined. It can be entered either as a real constant or a reference to an existing field definition. The value appears in the EGEOM3 data field of the GEOMETRY option.
Element Length	Defines the initial length of the cable elements. This property is optional and will default to the straight distance between the ends of the cable element. It can be entered either as a real constant or a reference to an existing field definition. The value appears in the EGEOM2 data field of the GEOMETRY option.

Links

This input data creates Marc element types 36 or 65. The GEOMETRY option is used to define the cross-sectional area for Conduction Links and the area where the element acts and the convective/radiative properties of the boundary for Convect/Radiation Links. Only the necessary properties are presented depending on the link type requested. Properties that can vary spatially are defined by referencing a spatial field (table). See Fields - Tables for more information.


Property Name	Description
Material Name	Defines the material to be used. A list of all materials (currently in the database) is displayed. Either select from the list or type in the name, preceded by an “m:”. This property is required.
Cross-Sectional Area	Defines the area of the link cross section. It can be entered either as a real constant, or a reference to an existing field definition. The value appears in the EGEOM1 data field of the GEOMETRY option and is required.
Emissivity	Defines the emissivity between the two end nodes of this link. This is entered in the EGEOM2 data field of the GEOMETRY option. This value can be either a real constant or a reference to an existing field definition. This property is optional.
Stefan-Boltz Constant	Defines the Stefan-Boltzmann radiation constant. It can be entered either as a real constant or a reference to an existing field definition.The value is entered in the EGEOM3 data field of the GEOMETRY option. This property is optional.
Abs Temp Conversion	Defines the absolute temperature conversion factor for the radiative boundary conditions. It can be entered either as a real constant or a reference to an existing field definition. The value is entered in the EGEOM4 data field of the GEOMETRY option. This property is optional.
Film Coefficient	Defines the convective film coefficient for convective boundary conditions. It can be entered either as a real constant or a reference to an existing field definition. The value appears in the EGEOM5 data field of the GEOMETRY option. This property is optional.

1D Shell/Membrane Elements

Axisymmetric Shell

This input data creates Marc element types 1, 15, 89 and 90 for structural elements or 87 and 88 for heat transfer elements. The properties entered into the Input Properties form fill out the necessary information in the GEOMETRY and NODAL THICKNESS keyword options of the Marc input file. The properties presented to you in the form are dependent on the element type to be created. Properties that can vary spatially are defined by referencing a spatial field (table). See Fields - Tables for more information. A list of all properties for beam/bar/pipe/truss elements are given below:


Property Name	Description
Material Name	Defines the material to be used. A list of all materials (currently in the database) is displayed. Either select from the list or type in the name, preceded by an “m:”. This property is required.
Thickness	For non-laminated axisymmetric shells, defines the shell thickness either as an element uniform or tapered based on the selected Value Type: Real Scalar: Each element will have a uniform thickness which can be entered as a real constant or a reference to an existing field definition. The data appears in the EGEOM1 data field of the GEOMETRY option. Field at Nodes: Tapered elements will be created by referencing an existing field definition. The data appears on the third card of the NODAL THICKNESS option. This property is required.
[Rigidity]	In a Coupled analysis, if this is set to Rigid, the element exhibits only heat transfer capabilities and becomes structurally rigid.
[Temperature Distribution]	In a Coupled analysis, if this is set to Quadratic, shell element temperatures will have 3 degrees-of-freedom (top, bottom, middle) as opposed to only two (top, bottom). The HEAT parameter is written to indicate this.

1D Rebar Membrane

This input data creates Marc rebar membrane element types 165 to 170, which are either plane strain or axisymmetric type elements for use in inserting into 2D solid plane strain or axisymmetric elements to define rebar layers. The properties entered into the Input Properties form fill out the necessary information in the REBAR and INSERT keyword options of the Marc input file. Properties that can vary spatially are defined by referencing a spatial field (table). See Fields - Tables for more information. A list of all properties for rebar membrane elements are given below:


Property Name	Description
Material Name	Defines the material to be used. A list of all materials (currently in the database) is displayed. Either select from the list or type in the name, preceded by an “m:”. This property is required.
Area	Defines the cross sectional area of each rebar in the layer. A spatially varying field can be provided if this varies along the length of the layer. Entered in the 3rd field of the 4th data block of the REBAR option. A spatial field can be entered if the Area varies from one location to another. In this case the 5th data block is also written.
Spacing	Defines the spacing of the rebar cords in the layer. A spatially varying field can be provided if this varies along the length of the layer. Entered in the 4th field of the 4th data block of the REBAR option. A spatial field can be entered if the Spacing varies from one location to another. In this case the 5th data block is also written.
Orientation	Defines the orientation angle of the rebar cords in the layer relative to the Reference Axis. This is the angle between the rebar and the projection of the reference axis on the rebar layer plane. A spatially varying field can be provided if this varies along the length of the layer. Entered in the 5th field of the 4th data block of the REBAR option. A spatial field can be entered if the Orientation varies from one location to another. In this case the 5th data block is also written.
[Reference Axis]	This is used to define the orientation angle. The reference axis is defined as a vector which is then projected onto the rebar layer plane. The orinetation angle is measured from this projection. If blank, it defaults to <1,0,0>, the x-axis. Reference axis is placed in the 4th-6th fields of the 3rd data block of the REBAR option.
[Microbuckle Factor]	If a factor is entered, this activates the microbuckle behavior of rebar cords in compression. The factor reduc es the rebar compression stiffness. A good default value is 0.02. Entry is flagged in the 8th field of the 3rd datablock of the REBAR option. The factor is placed in the 9th field.
[Original Radius for Cylinder Expansion]	If entered, flags structure as an axisymmetric expansion of cylinders of bias plies with cords nearly inextensible relative to matrix material. Rebar properties are then calculated by Marc. The reference axis needs to be the symmetric axis of the orignal cylinder and needs to pass through the origin of the coordinates. Entry is flagged on the 3rd card of the 3rd data block and the radius is placed in the 6th field of th3 4th data block of the REBAR option.
[Create MFD File?]	If this is set to YES, then a MFD file is written with the geometric rebar information. This file can only be accessed and visualized by MSC.Marc Mentat currently.


Note:	You may either generate 1D rebar membrane elements manually through the Element Properties application by assigning properties directly to a generated 1D mesh. Or you may use the Rebar Definitions tool available from the Tools pull down menu, which will generate the mesh and assign the properties automatically for you. See Rebar Definition Tool at the end of this section. A list of elements into which these rebar membrane elements are to be inserted is automatically determined on translation based on geometric tolerance, which writes the INSERT option to the input file. Only one rebar layer may be defined by any one element property set. If more than one layer is necessary, create coincident elements and define another rebar property set to these elements.

2D Elements

Shells, Plates, Membranes, Shear Panels

This input data creates Marc element types 18, 22, 30, 49, 68, 72, 75, 138, 139, 140, 147, or 148 for structural elements and element types 50, 85, or 86 for heat transfer elements. The properties entered into the Input Properties form fill out the necessary information in the GEOMETRY and NODAL THICKNESS keyword options of the Marc input file. When a preferred element coordinate system is requested, the ORIENTATION option is generated. Properties that can vary spatially are defined by referencing a spatial field (table). See Fields - Tables for more information. A list of all properties for shell/ plate/ membrane/ shear panel elements are given below:


Property Name	Description
Material Name	Defines the material to be used. A list of all materials (currently in the database) is displayed. Either select from the list or type in the name, preceded by an “m:”. This property is required.
Thickness	Defines the shell thickness either as element uniform or tapered based on the selected “Value Type.” Real Scalar: Each element will have a constant uniform thickness which can be entered as a real constant or a reference to an existing field definition. The data appears in the EGEOM1 data field of the GEOMETRY option. Element Nodal: Tapered elements will be created by referencing an existing field definition. The data appears on the third card of the NODAL THICKNESS option. This property is required.
Orientation System	Selects the coordinate frame in which to define preferred material orientation. See Material Orientation for more explanation. Only CID (coordinate frame specification) is valid (or a flagging User Sub. ORIENT).
Orientation Angle	Defines the angle measured from the edge of the element or other reference line (vector) to the first preferred material direction of the element. It can be entered either as a real constant or a reference to an existing field definition. The value appears in the second data field on the third card of the ORIENTATION option. This property is optional. See Material Orientation for more explanation.
[Transverse Shear]	If this is set to Parabolic, then the TSHEAR parameter is written, which changes the transverse shear model from constant through the thickness to a parabolic representation for thich shells, element types 22, 75, and 140.
[Rigidity]	In a Coupled analysis, if this is set to Rigid, the element exhibits only heat transfer capabilities and becomes structurally rigid.
[Temperature Distribution]	In a Coupled analysis, if this is set to Quadratic, shell element temperatures will have 3 degrees-of-freedom (top, bottom, middle) as opposed to only two (top, bottom). The HEAT parameter is written to indicate this.

2D Rebar Membrane

This input data creates Marc rebar membrane element types 147 and 148 which are 4 and 8-noded quad type elements, respectively, for use in inserting into solid 3D elements (7, 21, 35, 57, 84, 117) to define rebar layers (or laying on top of 2D membrane elements (18,30). The properties entered into the Input Properties form fill out the necessary information in the REBAR and INSERT keyword options of the Marc input file. Properties that can vary spatially are defined by referencing a spatial field (table). See Fields - Tables for more information. A list of all properties for rebar membrane elements are given above in 1D Rebar Membrane.

2D Solid Elements

Axisymmetric, Plane Stress, Plane Strain

This input data creates Marc element types 2, 3, 6, 10, 11, 19, 20, 26, 27, 28, 29, 32, 33, 34, 53, 54, 55, 56, 58, 59, 60, 62, 63, 66, 67, 73, 74, 80, 81, 82, 83, 91, 92, 93, 94, 95, 96, 114, 115, 116, 118, 119, 124, 125, 126, 128, 129, 151, 152, 153, 154, 155, or 156 for structural problems and 37, 38, 39, 40, 41, 42, 69, 70, 101, 102, 103, 104, 121, 122, 131, 132, 177, 178, 179, or 180 for heat transfer problems. The properties entered into the Input Properties form fill out the necessary information in the GEOMETRY keyword options of the Marc input file for thickness. When a preferred element coordinate system is requested, the ORIENTATION option is generated. Properties that can vary spatially are defined by referencing a spatial field (table). See Fields - Tables for more information. A list of all properties for axisymmetric, plane stress, and plan strain elements are given below. Only those pertinent to the element type are presented.


Property Name	Description
Formulation Options	This is set to none by default. If you wish to use an Assumed Strain, Constant Volume or Both of these formulation options, you must set this with the pull down menu to the right of this input property widget. The appropriate flag is placed in the GEOMETRY option to turn these options on if selected. Note that under the Translation Parameter form, Assumed Strain and Constant Volume (or Dilatation) can be globally turned ON for all elements. If you wish these options to vary with element property definitions, you must turn them OFF globally in Job Parameters.
Material Name	Defines the material to be used. A list of all materials (currently in the database) is displayed. Either select from the list or type in the name, preceded by an “m:”. This property is required.
Thickness	Defines the shell thickness either as element uniform or tapered based on the selected “Value Type.” Real Scalar: Each element will have a uniform thickness which can be entered as a real constant or a reference to an existing field definition. The data appears in the EGEOM1 data field of the GEOMETRY option. Element Nodal: Tapered elements will be created by referencing an existing field definition. The data appears on the third card of the NODAL THICKNESS option. This property is required.
Orientation System	Selects the coordinate frame in which to define preferred material orientation. See Material Orientation for more explanation. Only CID (coordinate frame specification) is valid (or a flagging User Sub. ORIENT).
Orientation Angle	Same explanation as for 2D Elements above.
Thickness Change	Defines the thickness change at a position within the application region. The thickness change value is determined from the translational z component of the displacement boundary condition at the selected node.
Rel. Surface Rotation	Defines the rotation of the application region’s top surface relative to its bottom surface. The rotation values are determined from the rotational x and y components of the displacement boundary condition at the selected node.
[Rigidity]	In a Coupled analysis, if this is set to Rigid, the element exhibits only heat transfer capabilities and becomes structurally rigid.

For lower-order laminated composite elements 151, and 152 (and 149) the following additional properties can be entered to define GASKET option (referred to as a GASKET material in the input file). If none of these properties are supplied, no GASKET option will be written.


Property Name	Description
Loading Path	This data box that accepts a non-spatial field of Stress(pressure) vs. Closure Distance (a non-spatial displacement field). A table is written according to the TABLE option with gasket closure as the independent variable. The table ID is referenced in 2nd field of 3rd data block of the GASKET option.
Yield Pressure	Enter the yield pressure of the gasket material. This fills in the 1st field of 5th data block of GASKET option. Only a scalar value can be entered.
Tensile Modulus	Enter the tensile modulus of the gasket material. This fills in the 2nd field of 5th data block of GASKET option. Only a scalar value can be entered.
Transverse Shear Modulus	Enter the transverse shear modulus of the gasket material. This fills in the 3rd field of 5th data block of GASKET option. Only a scalar value can be entered.
Initial Gap	Enter the initial gap of the gasket material. This fills in the 4th field of 5th data block of GASKET option. Only a scalar value can be entered.
Unloading Path 1-10	These are 10 data boxes like Loading Path that can accept non-spatial fields or Stress vs. Closure, written to the TABLE option, and referenced in data block 4, fields 1-10, respectively. Multiple unloading paths are allowed to fully model the behavior of these gasket type materials where each load cycle can see a different unloading path.

3D Elements

Solid

This input data creates Marc element types 7, 21, 35, 57, 61, 84, 107, 108,117, 120, 127, 130, 134, 149, 150, or 157 for structural problems and 43, 44, 71, 105, 106, 123, 133, 135, 175, or 176 for heat transfer problems. Properties that can vary spatially are defined by referencing a spatial field (table). See Fields - Tables for more information. When a preferred element coordinate system is requested, the ORIENTATION option is generated.


Property Name	Description
Formulation Options	This is set to none by default. If you wish to use an Assumed Strain, Constant Volume or Both of these formulation options, you must set this with the pull down menu to the right of this input property widget. The appropriate flag is placed in the GEOMETRY option to turn these options on if selected. Note that under the Translation Parameter form, Assumed Strain and Constant Volume (or Dilatation) can be globally turned ON for all elements. If you wish these options to vary with element property definitions, you must turn them OFF globally in Job Parameters.
Material Name	Defines the material to be used. A list of all materials (currently in the database) is displayed. Either select from the list or type in the name, preceded by an “m:”. This property is required.
Orientation System	Selects the coordinate frame in which to define the preferred material orientation. See Material Orientation for more explanation. Only CID (coordinate frame specification) is valid (or a flagging User Sub. ORIENT).
Orientation Angle	Defines the angle through which the Orientation System is rotated to define the preferred orientation. This property is optional. See Material Orientation for more explanation.
[Rigidity]	In a Coupled analysis, if this is set to Rigid, the element exhibits only heat transfer capabilities and becomes structurally rigid.


Note:	For solid laminated composite element 149, a GASKET option (material) can also be defined as explained in 2D Solid Elements.

Solid with Auto Tie

This input data creates Marc element types 7, 21, or 57 to tie shells to solid elements. Properties that can vary spatially are defined by referencing a spatial field (table). See Fields - Tables for more information. When a preferred element coordinate system is requested, the ORIENTATION option is generated. The thickness of the attached shell is placed in the GEOMETRY keyword option.


Property Name	Description
Formulation Options	Same explanation as for 3D Elements Solid elements.
Material Name	Defines the material to be used. A list of all materials (currently in the database) is displayed. Either select from the list or type in the name, preceded by an “m:”. This property is required.
Orientation System	Selects the coordinate frame in which to define material orientation angle. See Material Orientation for more explanation. Only CID (coordinate frame specification) is valid (or a flagging User Sub. ORIENT).
Orientation Angle	Same explanation as for Solid elements above.
Tied Shell Thickness	Defines the transition thickness where the solid element attaches to the adjacent shell elements. It can be entered either as a real constant or a reference to an existing field definition. The value is entered in the EGEOM1 data field of the GEOMETRY option and is required.

Material Orientation

Most 2D and 3D elements can have a preferred material orientation for orthotropic and anisotropic materials. This can be specified in a number of ways. The actual preferred orientation is measured from the given preferred directions based on the orientation angle given. The various scenarios that exist are:

• No Orientation Angle or Orientation System - no ORIENTATION option written. In this case, Marc will use its default preferred directions for 2D and 3D elements, which in most cases are defined by the element coordinate system.

• Orientation Angle given with no Orientation System specified. For 2D elements the EDGE 1-2 option is used in the ORIENTATION option. Only the EDGE 1-2 and the Orientation Angle are written to the ORIENTATION option. Marc determines the preferred directions from this data. The angle is measured from this element edge (projected onto the elements tangent plane and rotated about the tangent plane normal) and defines the 1st preferred direction. The 3rd preferred direction is the tangent plane normal and the 2nd preferred direction is the cross product of the 3rd and 1st preferred directions. This option is not practical because generally the material orientation does not change, but the element edges and their orientations relative to the actual material orientation do, thereby making this option useless unless the element 1-2 edge points the same direction for every element.

For 3D elements the 3D ANISO option is used in the ORIENTATION option. If no orientation system is specified, then the global system is assumed. The 1st, 2nd, and 3rd preferred direction are the x, y, and z-axes, respectfully rotated about the z-axis by the amount of the Orientation Angle specified. The rotated x and y-axis vectors are written to the ORIENTATION option.

• Orientation System given with or without the Orientation Angle. A coordinate system must be selected. For 2D elements, the UU PLANE option is written to the ORIENTATION option. The two vectors written to the ORIENTATION option are the x and z-axes of the Orientation System for rectangular systems. Again, Marc determines the preferred directions from this information. The 1st preferred direction is determined by the intersection of this x-z plane with the element tangent plane, rotated through the Orientation Angle about the element tangent plane’s normal vector. The 3rd preferred direction is the element tangent plane’s normal vector. And the 2nd preferred direction is the cross product of the 3rd and 1st preferred directions. Display of the 1st preferred material direction is a single vector at the centroid of the element in the element tangent plane. A warning message is issued if the plane defined and the element tangent plane are coplanar. In this case, this could pose problems to the Marc solver and should be corrected.

For cylindrical systems, the plane used to intersect the element tangent plane is the r-z plane. Thus there are an infinite number of possible planes in the theta direction. The plane used for a particular element is determined by the radial vector emanating from the coordinate system’s z-axis to the centroid of the element and the z-axis. Display of the 1st preferred material direction is a single vector at the centroid of the element. A warning message is issued if the plane defined and the element tangent plane are coplanar. In this case, this could pose problems to the Marc solver and should be corrected.

For 3D elements, the 3D ANISO option is used and the x and y axes of the selected coordinate system are written as the vectors in the ORIENTATION option with respect to the global system. The x, y, and z-axes define the 1st, 2nd, and 3rd preferred material directions. If an Orientation Angle is supplied, these vectors are rotated by this amount about the z-axis and written as such to the ORIENTATION option. For cylindrical systems the r, theta, z-axes are the 1st, 2nd, and 3rd preferred directions and again are rotated about z-axis if an Orientation Angle is supplied and written as such to the ORIENTATION option in the global system for each element. Display of the three preferred material directions is a triad at the centroid of the element with color coding and labels of the respective directions.

Use the Element Properties application Show | Orientation Angle/System to visualize the preferred directions in Patran. For 2D elements, the 1st preferred direction is displayed at the centroid of the element or at the corners of the associated geometry. The 2nd preferred direction is in the plane of the element at 90 degrees to the 1st preferred direction but is not plotted. The 3rd preferred direction is normal to the element tangent plane and also is not plotted. For 3D elements the complete triad is plotted. The 1st, 2nd, and 3rd preferred directions are plotted as magenta, cyan, red, respectfully.

See Volume C of the Marc documentation for more detailed information on the ORIENTATION option.

Elements in Coupled Analysis

Specifying element property data for Coupled analysis is identical to Structural analysis. In fact, coupled elements are structural elements in Marc but internally use the corresponding thermal element for the heat transfer portion of the analysis. There is only one exception to this and that is when you want elements to only display thermal properties and act structurally rigid. All coupled elements have a property word to force them to be structurally rigid. If this property word is left blank, structural element will be used. If set to “rigid,” the thermal element will be used and will act structurally rigid.

The table below indicates the Marc structural element (jsolid) and its corresponding thermal equivalent (jheat). A minus one (-1) indicates that the element is already a thermal element. A zero (0) indicates that the element does not have an equivalent thermal element and the coupled analysis will stop if used in a Coupled analysis.


jsolid/jheat	jsolid/jheat	jsolid/jheat	jsolid/jheat	jsolid/jheat	jsolid/jheat	jsolid/jheat
1 88	27 41	53 69	79 100	105 -1	131 -1	157 135
2 38	28 42	54 69	80 39	106 -1	132 -1	158 37
3 39	29 41	55 70	81 39	107 105	133 -1	159 85
4 0	30 44	56 69	82 40	108 106	134 135	160 39
5 99	31 0	57 71	83 40	109 -1	135 -1	161 39
6 37	32 41	58 69	84 43	110 -1	136 137	162 40
7 43	33 38	59 70	85 -1	111 -1	137 -1	163 43
8 0	34 41	60 69	86 -1	112 -1	138 50	164 135
9 36	35 44	61 71	87 -1	113 -1	139 85	165 0
10 40	36 -1	62 0	88 -1	114 121	140 85	166 0
11 39	37 -1	63 0	89 87	115 121	141 -1	167 0
12 -1	38 -1	64 65	90 0	116 122	142 0	168 0
13 99	39 -1	65 -1	91 101	117 123	143 0	169 0
14 99	40 -1	66 42	92 102	118 121	144 0	170 0
15 88	41 -1	67 42	93 103	119 122	145 0	171 0
16 99	42 -1	68 0	94 104	120 123	146 0	172 0
17 0	43 -1	69 -1	95 0	121 -1	147 0	173 0
18 39	44 -1	70 -1	96 0	122 -1	148 0	174 0
19 39	45 65	71 -1	97 0	123 -1	149 175	175 149
20 40	46 0	72 85	98 36	124 131	150 176	176 150
21 44	47 0	73 0	99 -1	125 131	151 177	177 151
22 85	48 0	74 0	100 -1	126 132	152 178	178 152
23 0	49 50	75 85	101 -1	127 133	153 179	179 153
24 0	50 -1	76 100	102 -1	128 131	154 180	180 154
25 99	51 0	77 100	103 -1	129 132	155 37
26 41	52 99	78 100	104 -1	130 133	156 38

Rebar Definition Tool

For the Marc Preference, a special application for creation of 2D layered rebar is available under the Rebar Definition tool in the Tools pulldown menu. Discrete rebar models and general 3d layered rebar models are not supported. Rebar is actually an element property definition for the Marc Preference, however this tool is used to automate the creation of rebar layers and embed them into existing element meshes. This tool allows you to:

• Create, modify, delete and visualize Rebar data definitions.

• Support multiple rebar definitions, both isoparametric and skew type geometry. See Figure 2‑1.

• Support rebar membrane elements in 2D solid (plane strain and axisymmetric) elements.

• Create a customized mesh and automatically assign rebar properties to these elements.


Note:	The Rebar Definition tool supports automatic generation of rebar elements and properties for 2D solid elements only. For rebar embedded into 3D solid elements, you must manually create the elements (mesh) and assign properties in the Element Properties application using 2D Rebar Membrane definition. You can also manually create 1D Rebar Membrane elements without using this tool but this is less convenient.

The most common use of this tool is in tire analysis, specifically where an axisymmetric model of a tire is created with multiple rebar layers. The axisymmetric rebar membrane elements are created across the existing mesh of the tire model using this tool. The axisymmetric analysis is run and then full 3D analysis performed by using Marc’s AXITO3D capability. The axisymmetric model is swept into full 3D including the rebar elements, which are then assigned 2D rebar membrane element properties for a full 3D analysis. This procedure is explained in Pre State Options.

Figure 2‑1 Rebar layer definitions for 2D solid elements with
a) SKEW and b) ISOMPARAMETIC type geometry.

The tool is quite simple to use as explained here. There are four basic commands: Create, Modify, Delete, and Show.

When a rebar layer is created it does a number of things:

1. First elements are created along the length of the curve. These elements are created such that nodes are placed at locations where the curve intersects element edges of the existing 2D mesh. You can think of the Rebar Definition tool as a specialized mesher.

2. A group with these nodes and elements by the same name as the rebar layer is created.

3. The elements for the rebar layer are assigned 1D rebar membrane properties. The Type and Option in the Element Properties application are determined by the continuum element types through which the rebar passes. This requires that the continuum element have properties assigned them before the rebar evaluation otherwise an error is issued. The list of continuum elements through with the layer passes plus the associated properties become part of the property set.

The best way to illustrate this is through an example. Below is a 3x3 mesh with two rebar layers passing through it.

The rebar layers must be evaluated and nodes created at all the intersecting element edge locations shown by dots. Elements must then be created by connecting the dots. These elements must then have properties assigned to them and stored as new element properties by the same name as the rebar layer(s). You can think of the evaluation as a mesher and property assignment all in the same operation.


Caution:	If you delete a rebar definition, the elements, property, and group that were created are still maintained (you can delete them manually if necessary). You can delete the elements and properties, but leave the rebar definition. If you try to recreate or modify an existing rebar definition it will recreate or modify the existing elements, property, and group.

The Rebar Definition tool is used to create layered rebar by defining a data set for a Curve list, material, cross-sectional area and other properties. After creation of the rebar definitions, you may proceed to the Analysis application and under Job Parameters you select the associated rebar for translation. See Job Parameters. When a user submits a job for analysis, only the rebar layers that are selected are translated


Note:	That is, if a rebar layer exists but is not selected, it will not be translated. However if a rebar property is defined but has no corresponding rebar layer as defined in the Rebar Definition tool, it will still be translated.

The preferred method in Marc is to use rebar membrane elements 147, 148, 165-170. These elements do not occupy the same space as the continuum elements as is necessary with other types of Marc rebar elements, but must be inserted into the element using the INSERT option. They support the skew type of definition because they are elements with one dimension less than their continuum counterparts. This means that a bar represents a layer across a 2D solid continuum element and a quad represents a plane across a 3D element, thus they can cross adjacent edges. A list of “membrane” rebar elements is listed here with their corresponding continuum element types


Element	Description	Corresponding Elements
147	4-Node 3D Rebar Membrane	18 or 7, 84, 117
148	8-Node 3D Rebar Membrane	30 or 21, 35, 57
165	2-Node Plane Strain Rebar Membrane	11, 80, 115, 118
166	2-Node Axisymm Rebar Membrane	10, 82, 95, 116, 119
167	2-Node Axisymm Rebar Membr w/ twist	20, 83
168	3-Node Plane Strain Rebar Membrane	27, 29, 32, 34, 54, 56, 58, 60
169	3-Node Axisymm Rebar Membrane	28, 33, 55, 59, 96
170	3-Node Axisymm Rebar Membr w/ twist	66, 67


Note:	These are the only rebar elements supported in the Marc Preference.

For 3D applications where rebar membrane elements are inserted into Hex elements (or possibly where rebar membrane elements are overlaid on top of standard membrane elements, the Rebar Definition tool is not used. The user must manually create the elements or sweep them such as in a AXITO3D application and then assign rebar element properties to them. As part of the rebar element property definition, the host elements are specified.

In actuality, the plane strain and axisymmetric cases can also be manually defined, but this is more difficult to mesh and visualize the rebar layers as the Rebar Definition tool does this for you.

For a general 3D problem, the rebar membrane properties can vary on all four edges of the Hex elements in which they pass. For a AXITO3D problem, the property definitions will remain exactly the same as for the axisymmetric case. They may vary on two of the edges but will not on the other two. In this case the c1 direction varies only. For a general case, a parametrically varying spatial field where c1 and c2 vary could be supplied.