Load Step: DLOAD

In the DLOAD dialog, define the *DLOAD cards on individual elements or geometry (surfaces). You can also define the DLOAD on element sets.

To open the dialog in the Load Step window, expand Distributed loads in the tree, select DLOAD, and select a load collector from the Load collector table.

Load Step: DLOAD: Define Tab

In the Define tab, define *DLOAD cards on individual elements or geometry (surfaces) as well as on element sets.

There are seven different DLOAD types available: default (Pressure), centrifugal, rotary acceleration, gravity, pressure in pipe/elbow, hydro pressure, and hydro pressure in pipe/elbow.

Only default (Pressure) type DLOAD can be created on an individual element or geometry in HyperMesh. The other types are available only for element sets.

It is recommended that you use only one type of DLOAD in a load collector in HyperMesh. If you need to use multiple types of DLOAD in the same STEP, define each type in a separate load collector and add them to the same load step.

You can define DLOAD on elements, geometry, or element sets. For Define DLOAD on:, the following options are available:
  • Elements or geometry
  • Element sets

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

Define DLOAD On: Elements or Geometry

Use the Define DLOAD on: Elements or Geometry option to define the default (pressure) type of DLOAD on individual elements or geometric surfaces.

Pressure loads created on elements have special graphical display in HyperMesh. Loads created on geometric entities such as surfaces are automatically mapped to FEA mesh on export. You can also map them using the Map Loads on Geometry button.

The Define tab for Define DLOAD on: Elements or Geometry contains the following buttons:
Table 1.
Button Action
Define from Pressures panel Opens the Pressures panel to create/update DLOAD.

To create a pressure on elements, go to the create subpanel, select the elems button, pick the desired elements from the HyperMesh graphics, select nodes using the switch, pick two or three nodes from a face of a selected element, input the magnitude, and click create.

To create a pressure on geometry, go to the create subpanel, select the surfs option from the toggle, pick the desired geometry from the HyperMesh graphics, input the 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 DLOAD from the update subpanel.
  • While you are in the Pressure panel, press the H key to view panel-specific help.
  • When you finish creating or updating boundary conditions, click return and the Step Manager is updated with the new loads.
Map Loads on Geometry Opens the 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 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 finish, click return to update the Step Manager with the new loads.

Define DLOAD On: Element Sets

Use the Define DLOAD on: Element sets option to define various DLOAD types on element sets.

The element set names are used in the *DLOAD data lines instead of the individual elements. Unlike Abaqus surfaces in HyperMesh, you can combine element sets with individual element IDs in the same *DLOAD card.
Note: There is no graphical display in HyperMesh for loads created on sets. 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 dialog contains a element sets menu with a list of the existing element sets. There are two types of elsets in HyperMesh: components and entity sets. The Abaqus elsets that are linked to sectional property cards, such as *SOLID SECTION and *SHELL SECTION, become components in HyperMesh. Others become entity sets. To differentiate between these two types, there is a divider line "- - - - -" in the elset list that pops up if you click the element sets menu. The elsets listed below the divider line are components.

This dialog also contains a table for data line input. The table changes depending on the DLOAD type selected. The table contains the following columns.

For Default (Pressure) type:
Table 2.
Column Description
Elset The name of the element sets. Element sets are added and deleted in this column using → or ←, respectively.
Label The labels of pressure load. The available labels are: P1, P2, P3, P4, P5, P6, and P.
Magnitude The magnitude of the load.
Load Id The ID of the load collector.
For Centrifugal type:
Table 3.
Column Description
Elset The name of the element sets. Element sets are added and deleted in this column using → or ←, respectively.
Label The labels of centrifugal loads and Coriolis forces. The available labels are: CENTRIF, CENT, and CORIO.
Magnitude The magnitude of the load.
Coord1 Coordinate 1 of a point on the axis of rotation.
Coord2 Coordinate 2 of a point on the axis of rotation.
Coord3 Coordinate 3 of a point on the axis of rotation.
DirCos1 1-component of the direction cosine of the axis of rotation.
DirCos2 2-component of the direction cosine of the axis of rotation.
DirCos3 3-component of the direction cosine of the axis of rotation.
Load Id The ID of the load collector.
For Rotary acceleration type:
Table 4.
Column Description
Elset The name of the element sets. Element sets are added and deleted in this column using → or ←, respectively.
Label The labels of the DLOAD type. The available labels are: ROTA.
Magnitude The magnitude of the load.
Coord1 Coordinate 1 of a point on the axis of rotary acceleration.
Coord2 Coordinate 2 of a point on the axis of rotary acceleration.
Coord3 Coordinate 3 of a point on the axis of rotary acceleration.
DirCos1 1-component of the direction cosine of the axis of rotary acceleration.
DirCos2 2-component of the direction cosine of the axis of rotary acceleration.
DirCos3 3-component of the direction cosine of the axis of rotary acceleration.
Load Id The ID of the load collector.
For Gravity type:
Table 5.
Column Description
Elset The name of the element sets. Element sets are added and deleted in this column using → or ←, respectively.
Label The labels of the DLOAD type. The available labels are: GRAV.
Magnitude The magnitude of the load.
Comp1 1-component of the gravity vector.
Comp2 2-component of the gravity vector.
Comp3 3-component of the gravity vector.
Load Id The ID of the load collector.
For pressure in pipe/elbow type:
Table 6.
Column Description
Elset The name of the element sets. Element sets are added and deleted in this column using → or ←, respectively.
Label The labels of the pressure in pipe/elbow elements. The available labels are: PE, PI, PENU, and PINU.
Magnitude The magnitude of the load.
Diameter The effective inner or outer diameter.
Condition The end loading condition: CLOSE (default) or OPEN.
Load Id The ID of the load collector.
For hydro pressure type:
Table 7.
Column Description
Elset The name of the element sets. Element sets are added and deleted in this column using → or ←, respectively.
Label The labels of the hydrostatic pressure. The available labels are: HP.
Magnitude The magnitude of the load.
Zero press Z-coordinate of zero pressure level in three-dimensional or axisymmetric cases; Y-coordinate of zero pressure level in two-dimensional cases.
Press point Z-coordinate of the point at which the pressure is defined in three-dimensional or axisymmetric cases; Y-coordinate of the point at which the pressure is defined in two-dimensional cases.
Load Id The ID of the load collector.
For hydro pressure in pipe/elbow type:
Table 8.
Column Description
Elset The name of the element sets. Element sets are added and deleted in this column using → or ←, respectively.
Label The labels of the hydrostatic pressure in pipe.elbow elements. The available labels are: HPE, and HPI.
Magnitude The magnitude of the load.
Zero press Z-coordinate of zero pressure level in three-dimensional or axisymmetric cases; Y-coordinate of zero pressure level in two-dimensional cases.
Press point Z-coordinate of the point at which the pressure is defined in three-dimensional or axisymmetric cases; Y-coordinate of the point at which the pressure is defined in two-dimensional cases.
Diameter The effective inner or outer diameter.
Condition The end loading condition: CLOSE (default) or OPEN.
Load Id The ID of the load collector.
The Define tab for Define DLOAD on: Element sets contains the following buttons:
Table 9.
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.
Show Faces This option is only shown for Default (pressure) type. It is mainly used to review the face identifiers of elements in the selected set. It creates a temporary skin of the selected elset, opens the Element Selector panel, from which you can select face elements from this skin. When you return from the element selector panel, the selected faces display color-coded face identifier tags. In performance graphics, these tags are sometimes blocked by the solid mesh. You may need to rotate the model a little to view the tags.

Right-click the Show faces button to clear the face review.
Define by vector This option is only shown for Gravity type. It opens the HyperMesh vector selector panel. Pick a vector and click proceed. This vector is used to define the Comp1, Comp2, Comp3, and Magnitude of the gravity load for the selected element set.
Create/Edit vector.. This option is only shown for Gravity type. 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 create a display for loads defined with sets.

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

Load Step: DLOAD: Delete Tab

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

There are three deletion options:
Table 10.
Option Description
All loads in current collector The Delete button deletes all the loads from the current load collector.
All 'Distributed loads' in current collector The Delete button deletes all distributed (*DLOAD, *FILM) 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: DLOAD: Parameter Tab

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

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

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