Force dialog box

Type
Type	Specifies how the force load is defined.Magnitude and DirectionDefines a force load with a magnitude and a single direction.NormalDefines a force load with a magnitude and a +/– direction normal to the selected geometry or element faces. ComponentsDefines a force load in terms of a global or local coordinate system. For example, if you choose a local Cartesian coordinate system, you can enter force magnitude for each of the X, Y, and Z components.To apply the force load to models in both the Simcenter Nastran Axisymmetric Structural and Structural environments or in the Samcef Axisymmetric and Other 2D Structural environment, select Component Force ZX or Component Force XY.Spatial TableDefines a force load using a set of nodes located near the spatial locations in the magnitude field. For each node in the target set, the load magnitude defined in the field is multiplied by the scale factor.Node ID TableDefines a force load using a node ID table, which contains a list of node IDs and corresponding scale factors for each nodal component (X,Y,Z). For each node in the node ID table, the load magnitude at the component is multiplied by the scale factor.Edge-FaceDefines a force load on an edge using the face for the orientation. The face defines the in-plane and out-of-plane directions. To apply the force load to models in both the Simcenter Nastran Axisymmetric Structural and Structural environments or in the Samcef Axisymmetric and Other 2D Structural environment, select Edge-Face ZX or Edge-Face XY.
Name
Name	Sets the name of the force node.
Description	Sets the description for the force node.
Destination Folder
Load Container	Specifies the folder in the Simulation Navigator in which the boundary condition will be stored. The list includes the root container and existing folders that you created using the New Folder command. Examples of a root container include Load Container, Constraint Container, and Simulation Object Container.To view a hierarchical list of existing folders, click Folder Manager . To create a new folder, right-click any level of the hierarchy and choose New Folder.
Model Objects
Appears when Type is set in Force dialog box to Magnitude and Direction, Normal, Components, or Edge-Face.
Group Reference	Lets you apply the force to a group.For more information, see Group Reference options.
Select Object Note: The graphic varies by Type.	Lets you select the geometry or FE entities on which the load will be applied.
Stacked Smart Selector Methods	Opens the Smart Selector Methods dialog box where you can specify a progression of smart selection filters.For more information, see Smart Selector Methods dialog box.
Excluded	Lets you remove individual entities from within the selected object.
Magnitude
Appears when Type is set to Magnitude and Direction, Normal, or Node ID Table.
Force	Sets the magnitude of the force load. For more information, see Additional magnitude options.
Associated Face
Select Face	Appears when Type is set to Edge-Face.Lets you select a face on which to apply an edge-face force load. The force load must be adjacent to the selected edge.
Direction
Method	Appears when Type is set to Magnitude and Direction and Simcenter Nastran, MSC Nastran, or Samcef is the specified solver.Controls whether you are specifying a static, concentrated force or a force that follows the movements of selected nodes in the analysis.Note: The option you select from the Method list also affects the corresponding bulk entry that the software creates when you export or solve your solution.**Along Vector (FORCE)**Defines a static, concentrated force. You define the direction of the force by specifying a vector.**Along 2 Nodes (FORCE1)**Defines a follower force. You define the direction of the force by specifying two nodes. These direction nodes define the vector that controls the direction of the force.**Normal to 4 Nodes (FORCE2)**Defines a follower force. You define the direction of the force by specifying four nodes. The direction of the follower force is parallel to the cross product of the vectors from Direction Node 1 to Direction Node 2, and from Direction Node 3 to Direction Node 4.
Specify Vector	Appears when Type is set to Magnitude and Direction.Defines the direction of the load.For more information, see Vector dialog box.To reverse the direction of the vector, click Reverse Direction .
Select Direction Node	Appears when Method is set to Along 2 Nodes (FORCE1) or Normal to 4 Nodes (FORCE2).Lets you select the nodes that define the motion of the follower force.
CSYS	Appears when Type is set to Components, Spatial Table or Node ID Table.Sets the coordinate system that the software uses to apply the force load. You can select the Global Cyclic Analysis or the Global coordinate system, or you can create one of the following types of local coordinate systems: Cartesian, Cylindrical, Spherical.Note: The Global Cyclic Analysis coordinate system is available only if it is defined in the FEM.
Components
Appears when Type is set to Components, Spatial Table, or Edge-Face.
Magnitude	Appears when Type is set to Components, or Spatial Table.Specifies the magnitude of the force load.
Fx, Fy, Fz****Fr, Ft, Fz****Fr, Ft, Fp****Radial Force, Axial Force	Appears when Magnitude is set to Expressions.Sets the force magnitude for each component. The components available depend on the coordinate system type.
Specify Field	Appears when Magnitude is set to Field or when Type is set to Spatial Table.Lets you select or define a field.
Scale Factors	Appears when Magnitude is set to Field or when Type is set to Spatial Table.Sets the scale factor (for each component) to apply to the field.The components available depend on the coordinate system type.
Shear Force	Appears when the Type is set to Edge-Face.Sets the magnitude of a force tangent to the selected edge.
In Plane Force	Appears when the Type is set to Edge-Face.Sets the magnitude of a force that is normal to the selected edge and tangent to the selected face.
Out of Plane Force	Appears when the Type is set to Edge-Face.Sets the magnitude of a force that is normal to the selected face.
Follower
Appears when Samcef is the specified solver and Method is set to Along Vector (FORCE).
Follower Force	Lets you define a follower force. Only valid for a structural nonlinear solution.
Follower Force Option
Appears when Abaqus is the specified solver.
Follower	Specifies that the direction of the force should rotate with the node to which you apply it, defining a follower force.
Distribution
Appears when Type is set to Magnitude and Direction, Normal, Components, or Edge-Face.
Method	Defines how the force load is distributed over the selected objects. Total per ObjectApplies the magnitude specified to each selected item. Because the force load needs to be applied at node locations, it is distributed over the region based on each area. For example, suppose you select two faces and specify a force load of 1000 N. Each face has a force load of 1000 N applied to it, regardless of its area. Then, the 1000 N force load is dispersed to the associated nodes based on its area contribution (associated element areas).Geometric distributionDistributes the total force load over all the selected items based on the area. All the nodes on the selected items then get a fraction of the force load based on the area of the associated elements. For example, suppose you select two faces that have areas of 40 mm2 and 60 mm2 respectively, and then specify a force load of 1000 N. A force load of 400 N is applied to Face 1, and a force load of 600 N is applied to Face 2. Then, the face load is dispersed to the individual nodes based on its area contribution (associated element areas). The total force load over the selected faces will always total 1000 N.Spatial, Spatial - Load Conservation, Spatial - Components, and Spatial - Components - Load ConservationDistributes the total force based on dimensionless spatial fields.The spatial fields are always mapped to global or Cartesian coordinates, even if they are defined in cylindrical or spherical coordinates. These distribution methods require special considerations. For more information, see Special considerations for specifying magnitude and distribution in separate fields.Note: The Spatial - Components and Spatial - Components - Load Conservation options appear when Type is set to Components.
Distribution Field
Specify Field	Appears when Distribution is set to Spatial, Spatial - Load Conservation, Spatial - Components, or Spatial - Components - Load Conservation.Defines how the force load is distributed over the nodes in the selected area.
Node Search Tolerance
Appears when Type is set to Spatial Table.
Tolerance	Sets the distance from each specified location that the software searches for the nearest node. If no nodes are within the specified tolerance of a location point, that location in the magnitude field is ignored.
Scaling ID Table
Appears when Type is set to Node ID Table.
Specify Field	Lets you use a node ID table to scale the force magnitude for the components of specific nodes.
Card Name	Displays the name of the solver card for the load.

How do I

Define a force or moment load using magnitude and a single direction

Define a force or moment load normal to the model

Define a force or moment load using components

Define a force or moment using a node ID table

Define a force or moment load on an edge

Learn more

Force load

Quick links

Command reference

Pre/Post video examples

Bulk Entry Descriptions

Simcenter 3D tutorials

Browse Simcenter 3D help by product area

Force dialog box, 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 } });