Calculate Mass
Use the Mass tool to calculate the mass, center of gravity (COG), and moments of inertia (MOI) of the model.

From the Validate ribbon, click the Mass tool.

Click on the guide bar to set your
desired options.
 Results type
 Defines the calculation as Mass, Center of Gravity and Inertia, or, Mass values only.
 Consider Time Step Mass
 Activates the calculation of solver numerical added mass due to
elemental time step.Restriction: This option is only valid in the Radioss and LSDYNA profiles.
 Time Step Definition
 Set the method to retrieve the Time Step value.Restriction: This option is only valid in the Radioss and LSDYNA profiles.
 User Define: the Time Step Value field becomes active and has to be set.
 From Control Card: the time step value is directly read from the
*CONTROL_TIMESTEP keyword.Restriction: This option is only valid in the LSDYNA profile.
 Axes
 Defines the coordinate system axes in which the CoG and MOI values are computed. It can be the Global System or a Local System. If Local System is selected, a System selector appears on the guide bar to select the system in the model.
 MOI Center
 Defines the center location used for the moment of inertias calculation. It can be "at CoG" or "at System Center". Example: If the Axes option is set to Global System, MOI Center set to "at System Center" means that MOI values are calculated around (0,0,0) point location.
 Consider Lumped Mass
 Allows you to consider the lumped masses for the calculation of the CoG and MOI on the component level. This option is off by default, which respects the solver behavior.

Restriction: This option is only valid in the Radioss and LSDYNA profiles.
 Show center of gravity
 Enables the creation of a marker in the modeling window to visualize the CoG location of the model.
 CoG Node
 Creates a free node at the CoG location of the model.
 Context numerical format
 Defines the format of the numerical format and precision of the values exposed in the results table
 Use the dropdown menu to group values based on assembly or include.

Click Compute.
The detailed mass values are displayed in a table.CoG and inertia selected as the Result Type, per component:
 Total Mass
 Represents the engineering mass as:
 Total Mass = Structural Mass + NonStructural Mass
 Structural Mass
 Represents the physical mass of the structure, calculated from the property and material characteristics assigned to the FE mesh.
 NonStructural Mass
 Represents the additional solver masses added on the structural mesh.

 In the LSDYNA profile:
 *ELEMENT_MASS_PART
 *ELEMENT_MASS_PART_SET
 MAREA value in *SECTION_SHELL
 NSM value in *SECTION_BEAM
 Lumped Mass
 In the Radioss profile:
 /ADMAS/3
 /ADMAS/4
 /ADMAS/6
 /ADMAS/7
 Lumped Mass
 In the PAMCRASH profile:
 NSMAS /
 NSMAS2 /
 In the LSDYNA profile:
 Lumped Mass
 Represents the portion of the nonstructural mass, which is distributed on structural nodes.

 In the LSDYNA profile:
 *ELEMENT_MASS
 *ELEMENT_MASS_NODE_SET
 *ELEMENT_INERTIA
 *ELEMENT_SEATBELT_ACCELEROMETER
 In the Radioss profile:
 /ADMAS/0
 /ADMAS/1
 /ADMAS/2
 /ADMAS/5
 In the LSDYNA profile:
 Mass in Rigid Body
 Represents the mass of the nodal rigid body elements in the collector.

 In the LSDYNA profile:
 *CONSTRAINED_NODAL_RIGID_BODY
 In the Radioss profile:
 /RBODY
 In the LSDYNA profile:
 Transferred Mass
 Represents the nodal mass transferred to the nodal rigid body elements or rigid Parts.

 In the LSDYNA profile:
 Nodal mass transferred to *CONSTRAINED_NODAL_RIGID_BODY
 Nodal mass transferred to rigid *PART connected with CONSTRAINED_EXTRA_NODE or CONSTRAINED_RIGID_BODIES.
 The lumped mass defined on nodes is also transferred to the rigids.
 In the Radioss profile:
 Nodal mass transferred to /RBODY
 The lumped mass defined on nodes is also transferred to the rigids.
 In the LSDYNA profile:
 Solver Mass
 Represents the mass as it is calculated by the solver.

 In the LSDYNA profile:
 For deformable *PART, the Lumped Mass is not
considered:
Solver Mass = Structural Mass + NonStructural Mass + Transferred Mass – Lumped Mass on nonrigid nodes
This value can be compared to the total mass of part in mass properties of part written in the d3hsp file.
 For rigid *PART, the lumped mass is
considered:
Solver Mass = Structural Mass + NonStructural Mass + Transferred Mass
This value can be compared to the mass of rigid body in mass properties of rigid body material written in the d3hsp file.
 For deformable *PART, the Lumped Mass is not
considered:
 In the Radioss profile:
 The Lumped Mass is not considered into the /PART
mass.
Solver Mass = Structural Mass + NonStructural Mass + Transferred Mass – Lumped Mass on nonrigid nodes
 The Lumped Mass is not considered into the /PART
mass.
 In the LSDYNA profile:
 Total Mass
 Represents the total engineering mass of the model and is the sum of the values in the Total Mass column of the table.
 Total Structured Mass
 The sum of the values in the Structural Mass column of the table.
 Total NonStructured Mass
 The sum of the values in the NonStructural Mass column of the table.
 Total Rigid Body Mass
 The sum of the Mass in Rigid Body column and represents the total mass of the nodal rigid body elements in the model.
 Total Transferred Mass
 The sum of the Transferred Mass column of the table.
 Total Solver Mass
 The sum of the Solver Mass column of the table.
 Total Model Mass
 Represents the final total mass of the model as it is calculated by the solver:

 Total Model Mass = Total Solver Mass + lumped mass on
nonrigid nodes
For LSDYNA, this value can be compared to the total mass in summary of mass written in the d3hsp file.
For Radioss, this value can be compared to the TOTAL MASS value written in the 0.out file.
 Total Model Mass = Total Solver Mass + lumped mass on
nonrigid nodes