Browsers provide a structured view of model data, which you can use to review, modify, create, and manage
the contents of a model. In addition to visualization, browsers offer features like search, filtering, and sorting,
which enhance your ability to navigate and interact with the model data.

FE geometry is topology on top of mesh, meaning CAD and mesh exist as a single entity. The purpose of FE geometry
is to add vertices, edges, surfaces, and solids on FE models which have no CAD geometry.

Tools and workflows that are dedicated to rapidly creating new parts for specific use cases, or amending existing
parts. The current capabilities are focused on stiffening parts.

Use PhysicsAI to build fast predictive models from CAE data. PhysicsAI can be trained on data with any physics or
remeshing and without design variables.

Explore, organize and manage your personal data, collaborate in teams, and connect to other data sources, such as
corporate PLM systems to access CAD data or publish simulation data.

Create concentrated moments by applying a load, representing moments, to a node or
set.

Moments are load config 2 and are displayed with a double-headed vector with the
letter M at the tail end.

Note: In the Radioss, Abaqus, and LS-DYNA profiles,
load entities are created immediately upon entering the tool. Use the Entity Editor to modify any properties. In all other solver
profiles, load entities aren't created until you make your selections then click
Create.

From the Analyze ribbon, Loads tool group, click the
Moments tool.

Select the keyword to create from the Load Type menu.

The available types depend on the current solver interface.

Choose the entities to which the moment will be applied.

Choose whether to create the forces in the global system or a local
system.

Specify the magnitude and direction of the moment.

Constant Components

Specify the direction and magnitude of the load by entering the X,
Y, and Z values of the components.

Constant Vector

Specify the magnitude, then use the plane and vector tool to specify
the vector along which the load should act.

Curve Components

Specify the X, Y, and Z components to define the direction and
magnitude, for example, (2,2,2) will be twice the magnitude of
(1,1,1). Next, select an existing curve. Last, specify a factor for
the curve’s xscale to use the same curve for many different cases,
but vary the scale of its intensity or time to match the needs of
your current load.

Curve Vector

When working with loads that are time dependent, use this method to
first specify a magnitude (yscale) for the curve. Next, select an
existing curve, then use the plane and vector tool to specify a
direction, if necessary. Last, specify a factor for the curve's
xscale to use the same curve for many different cases, but vary the
scale of its intensity or time to match the needs of your current
moment.

Equation

Specify the loading equation. Use the plane and vector tool to
specify a direction, then select the coordinate system to which the
vector corresponds.

Field Loads

Interpolate and extrapolate loads from existing loads. You can then
select the desired elements to which you wish to add loads, and any
existing loads on which you wish to base additional forces.

When you create, HyperMesh uses a
Green's function with the given boundary loads in order to create
the loads on all of the selected nodes. For smoothness, the gradient
at the boundary points is enforced to be zero; this ensures that the
extrapolated loads remain lower than the input loads. For this
reason it is recommended to use representative boundary values as
input to be able to capture the peaks reasonably.

Note: This version differs from linear
interpolation both in the way that the load magnitudes are
determined, and also in the fact that it can be applied to nodes
outside the boundaries of the chosen existing loads.

Linear Interpolation

Interpolate loads from a saved file or existing loads.

Note: Only available for shell
elements.

Each row of the input file contains the x,y,z coordinates of the
load followed by its three components. The data can be separated by
a space or tab.

You can then select the desired nodes to which you wish to add
loads, and pick 3 or more existing loads that enclose those nodes.
When you interpolate, a linear function is used to create additional
loads on the selected nodes, with magnitudes based on the magnitudes
of the loads that you had selected.

In the search radius field, specify the
search distance to find the loads which are within that distance
from a centroid or node on which a load is being interpolated. The
nearest 3 loads located within that distance are used to create the
load at the centroid or node by linear interpolation. Linear
interpolation uses a triangulation method, so if it finds fewer than
3 loads within that distance no interpolation takes place. While
reading the initial loads from a file, if linear interpolation is
not possible because the search radius is too small, the original
loads are simply applied to the nearest centroid or node.

Select fill gap to create a load at every
selected element centroid or node irrespective of the size of the
search radius.

Nodal distribution

Specify the magnitude, then use the plane and vector tool to specify
the vector along which the load should act.

Loads from files formatted as CSV (Comma Separated Values) or SSV
(Space-Separated Values) text files can be interpolated.

Field Loads will not overwrite any existing loads, so you can create an area
of loads via linear interpolation and then use field loads to expand the
load area without changing the loads already inside of the area.

If working in a controller, click Create.

Equations allow you to create force, moment, pressure,
temperature or flux loads on your model where the magnitude of the load is a
function of the coordinates of the entity to which it is applied. An example of such
a load might be an applied temperature whose intensity dissipates as a function of
distance from the application point, or a pressure on a container walls due to the
level of a fluid inside.

Functions must be of the form magnitude= f(x,y,z). The only
variables allowed are x, y and z, (lower case) which are substituted with the
coordinate values of the entity to which the load is applied. In the case of grid
point loads (force, moment or temperature) the grid point coordinates are used. For
elemental loads (pressure or flux) the element centroid coordinates are used. In the
event that a cylindrical or spherical coordinate system is used, x, y and z are
still used to reference the corresponding direction. Standard mathematical operators
and functions can be used; however, any functions requiring external data will not
be valid.

Note: If your equation contains a syntax error, no warning message will be
displayed, but any loads created will have a zero magnitude.