Load Step: CLOAD

In the CLOAD-Force dialog, define the *CLOAD card for dofs 1 through 3 and the CLOAD-Moment for dofs 4 through 6.

In Abaqus, *CLOAD can have degrees of freedom (dof) 1 through 6. In HyperMesh, concentrated loads with dofs 1 through 3 are called force and those with dofs 4 through 6 are called moments. The force and moments are two separate entities that are defined from separate panels. Their graphical displays are also different. As a result, the Step Manager has two distinct tree options for *CLOAD: CLOAD-Force and CLOAD-Moment.

Open Concentrated loads in the tree, select CLOAD-Force or CLOAD-Moment, and a load collector from the Load collector table to open the corresponding dialog in the right-most section of the Load Step window.

It is recommended that you do not use both CLOAD–Force and CLOAD-Moment in the same load collector in HyperMesh. If you need to use both types of *CLOAD in the same STEP, define each type in a separate load collector and add them to the same load step.

Load Step: CLOAD: Define Tab

In the Define tab, define *CLOAD (force or moment) cards on individual nodes or geometry (points). You can also define the *CLOAD on node sets.

You can define CLOAD-Force/Moment on nodes/geometry or on node sets. For Define CLOAD-Force/Moment on:, the following options are available:
  • Nodes or geometry
  • Node sets

The layout of the Define tab changes based on your selection.

Define CLOAD-Force/Moment On: Nodes or Geometry

Use the Define CLOAD-Force/Moment on: Nodes or geometry option to define *CLOAD (force or moment) on individual nodes or geometry.

The concentrated loads created on nodes have special graphical display in HyperMesh. Loads created on geometric entities such as surfaces, lines, or points are automatically mapped to FEA mesh on export. They can also be mapped using the Map Loads on Geometry button.

The Define tab for Define CLOAD-Force/Moment on: Nodes or geometry contains the following buttons:
Table 1.
Button Action
Define from 'Forces'/'Moments' Panel Opens the HyperMesh Forces or Moments panel to create/update a CLOAD.

To create a CLOAD on nodes, go to the create subpanel, select nodes using the switch, pick the desired nodes from HyperMesh graphics, select the global/local system, select a vector, input a magnitude, and click create.

To create a CLOAD on geometry, go to the create subpanel, select points using the switch, pick the desired geometry from HyperMesh graphics, select the global/local system, select a vector, input a magnitude, and click create.
Note:
  • Loads created on geometric entities are automatically mapped to FEA mesh on export. You can also map them using the Map Loads on Geometry button.
  • You can also update an existing force or moments from the update subpanel.
  • While you are in the forces or moments panel, press the H key to view panel-specific help.
  • When you finish creating or updating CLOAD, click return to update the Step Manager with the new loads.
Map Loads on geometry Opens the HyperMesh Loads on Geom panel to map loads on geometry to FEA mesh entities.
Click Map loads to map all geometric loads in the current load collector to FEA entities.
Note:
  • You can also pick other load collectors by clicking on the loadcols button and map loads in all of them together.
  • While you are in the Loads on Geom panel, press the H key to view panel-specific help.
  • When you are finished, click return to update the Step Manager with the new loads.

Define CLOAD-Force/Moment On: Node Sets

The Define CLOAD-Force/Moment on: Node sets option defines CLOAD on node sets.

The node set names are used in the *CLOAD data lines instead of the individual nodes. Unlike Abaqus surfaces in HyperMesh, you can combine node sets with individual node IDs in the same *CLOAD card.
Note: Loads created on sets are not graphically displayed in HyperMesh. Therefore, when you review a load collector in the Step Manager, only loads created on individual entities are highlighted. For loads defined on sets, the underlying nodes or elements are highlighted.
This Define tab for Define CLOAD-Force/Moment on: Node sets includes a Node sets menu containing a list of existing node sets. A data line input table also appears on the Define tab. The table contains the following columns:
Table 2.
Column Description
Nodeset The name of the node sets. Node sets are added or removed using → or ←, respectively.
Comp_x The component in x direction. The x-direction indicates dof 1 for force and dof 4 for moment.
Comp_y The component in y direction. The y-direction indicates dof 2 for force and dof 5 for moment.
Comp_z The component in z direction. The x-direction indicates dof 3 for force and dof 6 for moment.
Magnitude The magnitude. This column is non-editable. The magnitude is calculated based on the Comp_x, Comp_y, and Comp_z defined for each node set when you click Update.
Load Id The ID of the load collector.

For tips on entering information and navigating in the Define tab, see Step Manager Tab Environment.

The Define tab for Define CLOAD-Force/Moment on: Node sets contains the following buttons:
Table 3.
Button Action
Review Set Reviews the selected node sets by highlighting them in the HyperMesh graphics. Right-click Review to clear the review selections.
Create/Edit Set.. Opens the Entity Sets panel in HyperMesh. When you finish creating/editing the set, click return. The Step Manager is updated with the new set appearing in the element set list.
Display/Review from panel Opens the appropriate HyperMesh panel. Use the review button to expand the loads and constraints on the sets for visualization purposes.
→ Add the selected node set from the drop-down menu to the data line table on the right.
← Delete the selected node set from the data line table.
Define by vector Opens the HyperMeshvector selector panel. Pick a vector and click proceed. This vector is used to define the Comp_x, Comp_y, Comp_z, and Magnitude of the CLOAD for the selected node set.
Create/Edit vector Opens the Vectors panel in HyperMesh. When you finish creating/editing the vector, click return.
Review Creates special review forces or moments in HyperMesh graphics for the selected node set. These review forces or moments take into consideration the *TRANSFORM cards that may be associated with nodes in the node set. Right-click Review to clear the special review loads and highlighting.
Update Updates the HyperMesh database with the data lines defined in the table. By default, HyperMesh does not display loads defined with sets.

Load Step: CLOAD: Delete Tab

In the Delete tab, delete *CLOAD and other loads.

There are three deletion options:
Table 4.
Option Description
All loads in current collector The Delete button deletes all the loads from the current load collector.
All 'CLOAD' in current collector The Delete button deletes only *CLOAD loads from the current load collector.
By selection The Pick Loads button opens the HyperMesh load selector panel. Pick the loads you want to delete and click proceed.

The corresponding Reset button resets the selected loads.

The Delete button deletes the selected loads.

Load Step: CLOAD: Parameter Tab

In the Parameter tab, define optional parameters for the *CLOAD card.

The supported parameters are: Amplitude, OP, Load Case, Cyclic Mode, Follower, and Region Type.

Click Update to activate the optional parameter selection in the HyperMesh database.