Physical properties

This command allows to create during the modeling, an operation "Physical Properties" usable during this modeling. For example during the creation of an Assembly, it is possible to find the Center of Mass of several parts and to use it to built another Part. Unlike the Physical Properties of the Part or the Assembly command which creates these parameters only in Analysis Stage (it means regarding the finished Part or Assembly), this command creates an operation in the modeling Stage.

To not modify the file or to just consult Physical Properties, Use the Analyze physical Properties command.

Creation stages / Use:

Select the Analysis > Physical Properties... command from the drop-down menu.

Select the different entities to use.
Check the different physical properties to be managed: Mass, Center of mass, Moments of inertia, Surface area, Volume. These properties can also be used with local parts.
Validate.

By validating, an operation "Physical Properties" is created in the operations tree. It is usable like all other operations regarding the history.
A folder with the same name is also created in the Parameters folder of the entities tree.
The checked physical properties are visible, but non-modifiable in the Parameters folder in the entities tree.

The mass, the center of mass and the moments of inertia must be managed for the dynamic simulations.
Calculating the physical properties of an assembly does not account for welds and local modifications in the assembly.
Parts and sub-assemblies without mass are ignored in the calculation of the total mass, without displaying a warning message. It is the same for other calculations (surfaces, volumes, ...)
When activating the center of mass or inertia calculation in an assembly, they are materialized in the Points and Frames folders of the entities tree. These values are relative to the assembly in the position defined by the detailed configuration.
When a physical properties analysis operation is used with synchronized parts, the calculation is done at this time of the chronology and is based on their geometry of this time. This excludes for example, parts where the mass is manually given in the analysis stage.
To display the physical properties in the entity tree, switch to analysis mode.

Available Options:

Hide:

The box allow to hide selected entities during the use of the command, to be able to select other entities more easily, especially those who were behind.

Strict Mode:

When a part has no material or when its material is not correctly defined, the calculation of the mass of the assembly mass gives an incorrect result. In order to avoid errors, this option, when checked, does not allow you to calculate the mass of the assembly if one of the parts has no mass.