End releases for 1D elements

When using Nastran, ANSYS, LS-DYNA, or Simcenter Samcef as your solver, you can define end releases on beam and bar elements to model hinged or pinned beam ends (rather than welded, continuous ends). End releases are referred to as pin flags in Nastran.

End releases remove connections between a node and selected degrees of freedom. The degrees of freedom are defined in the element coordinate system.

In the following beam example, a force is defined on the horizontal span. Because end releases are defined at the ends of the bracing beams, the solver does not transfer the moment load from the horizontal beam to the bracing beams. The moments are transferred across the other elements in the horizontal span.

Bridge model. (1) and (2) represent the end releases

Note:

For information about displaying the end release icons on the model, see Displaying beam cross sections.

Bridge model; deflected shape with end releases

Bridge model; deflected shape without end releases

You can define end releases in the Mesh Associated Data or Element Associated Data dialog box.

Nastran

You can set DOF1 – DOF6 to On to disconnect the following forces for end A and/or end B of the element:

• DOF1 — axial force in Plane 1

• DOF2 — shearing force in Plane 1

• DOF3 — shearing force in Plane 2

• DOF4 — axial torque in Plane 2

• DOF5 — moment in Plane 2

• DOF6 — moment in Plane 1

As shown in the picture below, Plane 1 is the XY plane formed by the X and Y axes in the element coordinate system. Plane 2 is the XZ plane formed by the X and Z axes.

CBEAM element planes

In the bridge example, DOF6 is set to On at the ends of the bracing beams (the model is shown in the XY plane).

Ansys

You can set the degrees of freedom to On to disconnect the following forces for end I and/or end J of the element:

• UX — Displacements in the X direction.

• UY — Displacements in the Y direction.

• UZ — Displacements in the Z direction.

• ROTX — Rotations in the X direction.

• ROTY — Rotations in the Y direction.

• ROTZ — Rotations in the Z direction.

LS-DYNA

You can set the degrees of freedom to On to disconnect the following forces for end A (N1) and/or end B (N2) of the element:

LS-DYNA variable (*ELEMENT_BEAM keyword)	DOF1	DOF2	DOF3	DOF4	DOF5	DOF6
RT1,RT2 EQ.0	Off	Off	Off	—	—	—
RT1,RT2 EQ.1	On	Off	Off	—	—	—
RT1,RT2 EQ.2	Off	On	Off	—	—	—
RT1,RT2 EQ.3	Off	Off	On	—	—	—
RT1,RT2 EQ.4	On	On	Off	—	—	—
RT1,RT2 EQ.5	Off	On	On	—	—	—
RT1,RT2 EQ.6	On	Off	On	—	—	—
RT1,RT2 EQ.7	On	On	On	—	—	—
RR1,RR2 EQ.0	—	—	—	Off	Off	Off
RR1,RR2 EQ.1	—	—	—	On	Off	Off
RR1,RR2 EQ.2	—	—	—	Off	On	Off
RR1,RR2 EQ.3	—	—	—	Off	Off	On
RR1,RR2 EQ.4	—	—	—	On	On	Off
RR1,RR2 EQ.5	—	—	—	Off	On	On
RR1,RR2 EQ.6	—	—	—	On	Off	On
RR1,RR2 EQ.7	—	—	—	On	On	On

Simcenter Samcef

You can set DOF1 – DOF6 to On to disconnect the following DOFs of the element:

• DOF1 — Displacements in the xelem direction.

• DOF2 — Displacements in the yelem direction.

• DOF3 — Displacements in the zelem direction.

• DOF4 — Rotations in the xelem direction.

• DOF5 — Rotations in the yelem direction.

• DOF6 — Rotations in the zelem direction.

Beam element axes

Note:

Releasing ends of beams is only available in the Simcenter Samcef Linear solutions. For more details, see the beam element in the Simcenter Samcef structure element library.

How do I

Create a 1D mesh

Beam cross section workflow

Create a standard cross section

Create a cross section from the face of a solid

Create a cross section from a sketch

Create a cross section by entering properties

Assign a cross section to a beam mesh

Define cross section orientation

Offset a cross section

Improving performance for narrow beam cross sections

Learn more

1D meshing

1D element coating meshes

Ensuring consistent 1D element orientation during mesh creation

Creating beam cross sections

Displaying beam cross sections

Reusable beam cross sections

Quick links

Command reference

Pre/Post video examples

Bulk Entry Descriptions

Simcenter 3D tutorials

Browse Simcenter 3D help by product area

End releases for 1D elements, Simcenter 3D 2021.1 Series

© 2020 Siemens

window.mainLanguage="en_US"

window.delivId=""

window.projectId=""

MathJax.Hub.Config({ TeX: { extensions: ["autoload-all.js"] }, tex2jax: { displayMath: [ ] }, "SVG": { scale: 125 } });