Connection element dialog boxes

Name
Name	Sets the name of the connection element.
Modelization
Manual	Appears for seam weld and spot weld elements.Lets you manually select the nodes at the weld line and existing elements that define the connection.
Type	Specifies the elements that you can use for meshing the connection. The type of elements you can use depend on the type of the connection and the specified solver.Note: If you created User Defined, Universal, or Inplane kinematic connections for a SOL 402 kinematic analysis, you must select MPC+RBE2 spiders(s). Otherwise, an error message is issued and you cannot complete the analysis.
Connection
Select connections	Lets you select connections for meshing. You can select a single connection or multiple connections (of the same type) from the existing connections under the Universal Connections container in the Simulation Navigator.
Create new connection	Opens the corresponding connection dialog box, where you can define new connections.
Minimum Bar Element Length
Available for bar connections.
Minimum Bar Element Length	Sets the minimum distance between the connection's targets that is required for the software to create a 1D bar element, such as CBAR.Setting a minimum distance prevents the software from creating zero length elements. The software uses the minimum distance as follows based on how you define the connection's targets on the Targets page of the Bar Connection dialog box:If the distance between Target 1 and Target 2 is greater than or equal to Minimum Bar Element Length, then the software realizes (meshes) the bar connection using a 1D bar element.If the distance between Target 1 and Target 2 is less than Minimum Bar Element Length, and both Target 1 and Target 2 are set to Single Point, then the software does not realize (mesh) the bar connection.If the distance between Target 1 and Target 2 is less than Minimum Bar Element Length, and Target 1 and Target 2 are set to any other combination, then software realizes (meshes) the bar connection rigidly using a RBE2 element.
Maximum Distance To Closest Node
Appears for the following connections:For seam weld connections, appears when the Manual check box is cleared and Type is set to RBE2.For adhesive and sealing connections, appears when Type is set to CELAS+RBE2.For crimp connections, appears when Type is set to RBE2 or RBE2+RBE2.For rivet connections, appears when Type is set to RBE2 or CBAR+CBUSH+RBAR.For clinch connections, appears when Type is set to RBE2.
Max Dist To Node	Sets the maximum permissible distance between the following entities:Each definition point on the line definition and each projection point on each support.The nodes on the connecting flanges closest to these points.RBE2 elements are created by the software between the nodes that lie in this range.
Override Shank Diameter
Available for bolt connections when Type is set to CBAR+RBE2 spider(s) or CBEAM+RBE2 spider(s) elements.Note: Available only in the Nastran solver environment.
Override Shank Diameter	Lets you manually override and edit the diameter of the beam element associated with a bolted connection.The diameter is overridden for every bolt within the connection.You can use this to test the effect that various diameters have on the solution, such as the reduction in cross-section caused by bolt preload.
Shank Element Diameter	Available when the Override Shank Diameter check box is selected.Sets the diameter of the beam element. A larger diameter corresponds to a higher bolt stiffness.
Minimum Shank Element Length
Available for bolt connections when Type is set to CBAR+RBE2 spider(s), CBEAM+RBE2 spider(s), B31+CONNECTORS spider(s) or BEAM188+CERIG spider(s) elements.
Minimum Shank Element Length	Sets the minimum distance required to create a beam element between the selected flanges.When the distance between the selected flanges is greater than this value, a beam element is created.When the distance between the selected flanges is less than this value, a spider element is created.
Split Shank Element
Available for bolt connections when Type is set to CBAR+RBE2 spider(s), CBEAM+RBE2 spider(s), B31+CONNECTORS spider(s) or BEAM188+CERIG spider(s) elements.
Number of Elements	Sets the number of equal-length elements to split the shank element into.The default value is one, meaning that the shank element is not split.If your connection contains multiple bolts, the shank element for each bolt within the connection is split into the specified number of elements.
Split Shank Element
Available for bolt connections.
2 Rings Spider	Select this check box to extend the legs of spider-type elements, such as Nastran RBE2 or ANSYS CERIG elements, to connect to the second ring of nodes around the bolt, even if the diameter of the bolt's head does not include those nodes.For more information, see Extending the legs of spider elements in bolt connections.
Stiffness Parameters
Available for rivet connections when type is set CBUSH+RBE3.
Stiffness Parameters	Specifies the method for determining the stiffness of the CBUSH element.Huth FormulaLets you set the stiffness parameters to be used in the Huth formula.User Defined StiffnessLets you manually set the stiffness values in the respective degrees of freedom.
Huth Formula
Available for rivet connections when type is set to CBUSH+ RBE3 and Stiffness Parameters is set to Huth Formula. These options are input to the Huth formula as outlined in Reference 1 below.
Shear Type	Specifies the shear type as input to the Huth formula.Single Shear****Double Shear
Rivet Type	Specifies the rivet type as input to the Huth formula.Rivet MetallicBolted MetallicBolted Graphite/EPoxy
Stiffness
Available for the following:Rivet connections when Type is set to CBUSH+ RBE3 and Stiffness Parameters is set to User Defined Stiffness.Adhesive connections when Type is set to CELAS+RBE2.
X Translation Y TranslationZ TranslationX Rotation per RadianY Rotation per RadianZ Rotation per Radian	Sets the stiffness along the X-axis, Y-axis, and Z-axis of the defined coordinate system.
Axis Type
Available for adhesive connections when Type is set to CELAS+RBE2.
Axis Type	Specifies the type of axis for CELAS element.
Local	Appears when Axis Type is set to Cartesian, Cylindrical, or SphericalLets you define the coordinate system.Click CSYS Dialog to use the CSYS dialog box to create the coordinate system. Click to choose a coordinate system command to create the coordinate system.
Layers per Width
Available for adhesive connections.
Layers per Width	Controls the number or size of solid elements to create along the width of the adhesive connection. Creating layers of solid elements along the width of the connection allows you to more accurately model the longitudinal shearing behavior of the adhesive.Select Number of Layers to specify the number of rows of solid elements to create across the width of the adhesive. The software divides the Width value by the Number of Layers value to determine the size of each layer of elements.Select Layer Size to specify the size of the solid elements to create. The software divides the Layer Size value that you specify by the Width value to determine the number of layers of elements to create. If the result is a real number, the software uses the integer as the total number of layers to generate. The software adjusts the Layer Size value to accommodate the width of the connection and issues an information message that displays the adjusted value.For more information, see Controlling the number of layers across the width of adhesive connections.
Number of Layers	Available if Layers per Width is set to Number of Layers.Lets you specify the number of rows of solid elements to create.
Layer Size	Available if Layers per Width is set to Layer Size.Lets you specify the size of the solid elements to create.
Select Nodes
Appears for seam weld elements when the Manual check box is selected.
Method	Specifies how you want to select the nodes.Connection NodesSelects nodes along the weld line.SpecifyLets you select the nodes.
Group Reference	Appears when Method is set to Specify.Opens the Group Selection dialog box from which you select the groups that you want to be available on this dialog box.For more information, see Group Reference options.
Select Node	Lets you select the nodes from the graphics window.
Node Labels	Lets you add nodes to the selection.Use a space or comma to separate your entries.Use a colon or a dash to add a range of node labels.For example, enter 1:10 or 1-10 to add all the node labels from 1 to 10.Use colons to add an incremented range of node labels.For example, enter:1:9:2 to add node labels 1, 3, 5, 7, 9.1:10:2 to add node labels 1, 3, 5, 7, 9, 10.10:1:-2 to add node labels 10, 8, 6, 4, 2, 1.Press enter or click Select to add your entries.To edit your selection, click Edit Node Selection .
Select Elements
Appears for seam weld and spot weld elements when the Manual check box is selected.
Group Reference	Opens the Group Selection dialog box from which you select the groups that you want to be available on this dialog box.For more information, see Group Reference options.
Select Elements	Lets you select the elements from the graphics window.
Labels	Lets you type the label number of the element you want to include. After you type the label number, click to select it. The Select Elements count updates with the number of elements you add.To edit the list of elements, click Edit Element Selection .
Physical Property
Available for bearing connections when Type is set to CBEAR2 + FOU3 + RBE3 spider(s) or CBEAR2 + RBE2 spider(s).
Type	Specifies the type of physical property table, PBEAR2, to associate with the CBEAR2 element.
Rotor Bearing Property	Specifies existing PBEAR type physical property tables.To modify the selected physical property table, click Edit .To define a new physical property table, select None and then click Create Physical .To search for and filter by existing property tables, click More Options
Options group
Available for bearing connections when you click More Options .
Find	Sets the name of an existing physical property table to search for. Click Find to search. Physical property tables meeting the search criteria are displayed in the list.
Filter by Name****Filter by Label	Sets the name or labels of the objects that you want to filter by. This filter supports wildcards. The default wildcard of * displays all entries in the list.
Physical property table list	Lists physical property tables. Select a physical property table from the list to use for Rotor Bearing Property.
Bushing Type
Available for bushing connections when Type is set to CBUSH2+RBE2 spider(s).Sets the type of coordinate system, either rectangular or cylindrical, used to define the PBUSH2 physical property.Note: Bushing Type should be set to match the Physicals Definition method on the General page of the Bushing Connection dialog box.
Eccentricity
Available for bushing connections when Type is set to CBUSH2+RBE2 spider(s).For more information, see the PBUSH2 bulk entry.
Eccentricity Type	Specifies how the location of eccentricity is defined.N1-N2Sets the eccentricity location between two nodes.ExplicitSets the eccentricity location using the X, Y, and, Z distance relative to the first node.
Eccentricity (LOCA)	Available when Eccentricity Type is set to N1-N2.Sets the eccentricity location between two nodes. 0.0 corresponds to the first node, 1.0 corresponds to the second node, 0.5 corresponds to midway between the first and second nodes, and so on.
**X value (ECC1)****Y value (ECC2)**Z value (ECC3)	Available when Eccentricity Type is set to Explicit.Sets the eccentricity location using the X, Y, and, Z distance relative to the first node.
Enable CSYS for Offset Values (FRM2)	Available when Eccentricity Type is set to Explicit.Enables you to define the location of the eccentricities with respect to a coordinate system.
CSYS	Available when Enable CSYS for Offset Values (FRM2) is selected .Specifies the type of coordinate system used to define the location of the eccentricities.
Local	Available when CSYS is set to Cartesian or Cylindrical.Lets you define a local Cartesian or cylindrical coordinate system in which to define the location of the eccentricities.
Damping Forces
Available for bushing connections when Type is set to CBUSH2+RBE2 spider(s).For more information, see the PBUSH2 bulk entry.
Compute the Damping Forces (DAMP)	Specifies whether damping forces are computed or set to zero.AlwaysComputes damping forces.No Damping when the Elastic Force Is NullSets damping forces to zero when elastic forces are zero.
Rupture with Damage
Available for bushing connections when Type is set to CBUSH2+RBE2 spider(s).For more information, see the PBUSH2 bulk entry.
Damage Nonlinear Function	Specifies whether to use the ellipsoid criterion to analyze the bushing.
Parameter for Delay (ADEL)	Available when Damage Nonlinear Function is set to Damage.Sets the time constant (ADEL).
Time Parameter for Delay (TAU)	Available when Damage Nonlinear Function is set to Damage.Sets the scaling factor (TAU).
Maximum Damage Value (DDEN)	Available when Damage Nonlinear Function is set to Damage.Sets the critical value, CRIT, in the ellipsoid criterion at which rupture is predicted to initiate.
**Rupture Limit Force X (FRUX)****Rupture Limit Force Y (FRUY)****Rupture Limit Force X (FRUZ)****Rupture Limit Moment X (MRUX)****Rupture Limit Moment Y (MRUY)**Rupture Limit Moment Z (MRUZ)	Available when Bushing Type is set to Rectangular and Damage Nonlinear Function is set to Damage.Sets the strength values that are used in the ellipsoid criterion for axial bushings.
**Rupture Limit Radial Force (FRUR)****Rupture Limit Force -Z (FRUZ)****Rupture Limit Radical Moment (MRUR)**Rupture Limit Moment -Z (MRUZ)	Available when Bushing Type is set to Cylindrical and Damage Nonlinear Function is set to Damage.Sets the strength values that are used in the ellipsoid criterion for radial bushings.
Mass
Available for bushing connections when Type is set to CBUSH2+RBE2 spider(s).
Mass (MASS)	Sets the mass of the bushing.
Hysteretical Damping Constants
Available for bushing connections when Type is set to CBUSH2+RBE2 spider(s) and Bushing Type is set to Rectangular.For more information, see the PBUSH2 bulk entry.
**X Translational (HCTX)****Y Translational (HCTY)**Z Translational (HCTZ)	Sets the values for hysteretic damping in translation.
**X Rotation (HCRX)****Y Rotation (HCRY)**Z Rotation (HCRZ)	Sets the values for hysteretic damping in rotation.

References

[1] Huth, Heimo. "Influence of Fastener Flexibility on the Prediction of Load Transfer and Fatigue Life for Multiple-Row Joints," in Fatigue in Mechanically Fastened Composite and Metallic Joints: A symposium, ed. John M. Potter. (ASTM Special Technical Publication 927, March 1985), 221.

How do I

Create and edit universal connections

Learn more

Universal connections

Quick links

Command reference

Pre/Post video examples

Bulk Entry Descriptions

Simcenter 3D tutorials

Browse Simcenter 3D help by product area

Connection element dialog boxes, 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 } });