The Load sub-menu contains the following options:

• Create.
• Edit.
• Duplicate.
• Preview.
• Propagate.
• Hide/Show.
• Delete.

The types of loads and their options are listed below:

Concentrated force #

• Name.
• Region.
• Force components – components of the concentrated force per node:
  • * F1 – force in the X axis.
  • * F2 – force in the Y axis.
  • * F3 – force in the Z axis.
• Magnitude – resultant force (it’s calculated automatically when the components of the force are specified).
• Phase – force phase (for steady state dynamics only).
• Amplitude.
• Coordinate system – Global or user-defined one.
• Color.

Moment #

• Name.
• Region.
• Moment components – components of the moment per node:
  • * M1 – moment about the X axis.
  • * M2 – moment about the Y axis.
  • * M3 – moment about the Z axis.
• Magnitude – resultant moment (it’s calculated automatically when the components of the moment are specified).
• Phase – moment phase (for steady state dynamics only).
• Amplitude.
• Color.

Uniform pressure #

• Name.
• Region.
• Magnitude – value of the pressure load.
• Phase – pressure phase (for steady state dynamics only).
• Amplitude.
• Color.

Hydrostatic pressure #

• Name.
• Region.
• First point coordinates – by selection or by direct input of coordinates:
  • X. Y. Z.
• First point pressure magnitude – pressure magnitude at the first point.
• Second point coordinates – by selection or by direct input of coordinates:
  • X. Y. Z.
• Second point pressure magnitude – pressure magnitude at the second point.
• Pressure change direction – by selection (two points) or by direction components:
  • * N1 – direction component in the direction of the first axis.
  • * N2 – direction component in the direction of the second axis.
  • * N3 – direction component in the direction of the third axis.
• Phase – pressure phase (for steady state dynamics only).
• Cutoff: None / Positive cutoff / Negative cutoff – positive pressure cutoff sets all positive pressure values to 0 while negative pressure cutoff sets all negative pressure values to 0.
• Amplitude.
• Color.

Imported pressure #

• Name.
• Region.
• Import from File – OpenFOAM (.foam) file from which the pressure results will be imported.
• Interpolator: Closest node or Closest point – the first method takes the value from the closest node on the source mesh while the second method interpolates the closest three nodal values.
• Magnitude factor – pressure magnitude scale factor.
• Phase – pressure phase (for steady state dynamics only).
• Scale factor – imported geometry scale factor.
• Amplitude. – Color.

Surface traction #

• Name.
• Region.
• Force components:
  • * F1 – force in the X axis.
  • * F2 – force in the Y axis.
  • * F3 – force in the Z axis
• Magnitude – resultant force (it’s calculated automatically when the components of the force are specified).
• Phase – surface traction phase (for steady state dynamics only).
• Amplitude.
• Coordinate system – Global or user-defined one.
• Color.

Normal shell edge load #

• Name.
• Region.
• Magnitude – value of the shell edge load.
• Phase – edge load phase (for steady state dynamics only).
• Amplitude.
• Color.

Gravity #

• Name.
• Region.
• Gravity components:
  • * F1 – gravitational acceleration in the X axis.
  • * F2 – gravitational acceleration in the Y axis.
  • * F3 – gravitational acceleration in the Z axis.
• Magnitude – resultant acceleration (it’s calculated automatically when components of the force are specified).
• Phase – gravity load phase (for steady state dynamics only).
• Amplitude. – Color.

Centrifugal load #

• Name.
• Region.
• Rotation center coordinates – by selection or by direct input of coordinates:
  • X. Y. Z.
• Rotation axis components:
  • * N1 – axis component in the direction of the X axis.
  • * N2 – axis component in the direction of the Y axis.
  • * N3 – axis component in the direction of the Z axis.
• Magnitude – rotational speed around the axis defined by a point and a direction.
• Phase – rotational speed phase (for steady state dynamics only).
• Amplitude.
• Color.

Pre-tension #

• Name.
• Type: Force/Displacement.
• Region.
• Auto compute: Yes/No – automatic computation of the pre-tension direction.
• Magnitude – force or displacement magnitude for the pretension load.
• Amplitude.
• Color.

Defined Field #

Defined fields are used to prescribe predefined values to the nodes. The types of predefined fields and their options are listed below:

• Temperature – can be used to specify temperature field for static step
  • Name.
• Define temperature: By value.
  • Region.
  • Temperature.
• Define temperature: From file
  • Results file .frd.
  • Step number.

Postscript #

Concentrated force load applies the specified force to each node belonging to the selected region. Thus, if this load is applied to a surface, each node on that surface will be subjected to the specified force which is usually not desired. Thus, surface traction load should be used to apply force to surfaces.

Hydrostatic pressure is defined using pressure magnitudes at two points with given coordinates and the direction of the pressure increase (specified by selecting two points or by providing the vector components directly). This tool can be used to define not only the hydro-static pressure but also general linearly varying distributed load (triangular or trapezoidal), not associated with the presence of a fluid.

Imported pressure uses pressure results from OpenFOAM CFD simulation as loads in a structural analysis. Both ASCII and binary OpenFOAM results are supported. A file with .foam extension is needed for this type of load. It’s an empty (dummy) file used to access folders with OpenFOAM results. If parallel processing was used for OpenFOAM analysis, the reconstruct Part command needs to be utilized after the CFD simulation to merge the results from different processors. It’s not necessary to import the same file with geometry as the one used for CFD analysis but the geometry has to be located in the same place in a 3D space and use the same units of length as the ones used in OpenFOAM. The user needs to be careful with units since the pressure in OpenFOAM results might be given as kinematic pressure (pressure divided by density). The scale factor can be used to compensate for this. Preview option allows users to ensure that the imported pressure load is defined correctly – the applied pressure multiplied by the scale factor is visualized there along with the distances (closest distance between the Solvix mesh and the OpenFOAM mesh). Those distances should be small since they are the result of non-coincident meshes.

Surface traction load internally applies concentrated forces to each node on the selected surface. Their values sum up to the total magnitude specified in the load definition window. If multiple surfaces are selected, the load acting on each of them sums up to the value specified in the load definition window.

Despite the name, gravity load can be used to prescribe any type of translational acceleration to the structure (such as deceleration due to braking or acceleration of the vehicle).

Pre-tension is a specific type of load that requires some special considerations. Prior to defining it, a boundary layer needs to be created. Pre-tension load should be disabled in the second step of the analysis, when actual loading is applied to the model. This can be done by changing the displacement-type pre-tension setting to Fixed.

Items such as constraints, contact pairs, steps, boundary conditions and loads can be activated or deactivated (excluded from the analysis without the need to delete their definitions completely).

Below the menu bar there is a Symbols drop down list, that allows the selection of how the symbols are displayed (None, Model, Step-1, …).