Engineering analysis + design software

User Area > Advice

How do I define a point mass?

In V14 there are two ways to define a point mass. The easier option is to use:

Attributes > Mesh > Point > Point Mass or Joint > Non Structural Mass

This could be assigned to points that are part of the model.  

In LUSAS you can also use line and surface mass only elements in addition to point mass elements.  

These specific lumped mass elements are for distributed lumped mass.

The mass element appear as Non-Structural mass in the mesh description field when defining the mass element dataset. See LUSAS Element Reference Manual for further details of the mass elements. In general they are as follows:

            Point (PM2, PM3)

            Line (LM2, LM3, LMS3, LMS4)

            Area (TM3, TM6, QM4, QM8)

After defining the mesh, you need to assign a material to the Mass elements too. For this purpose define mass via:

Attributes > Material > Specialised > Mass

This material attribute is then assigned to the relevant features.

The second option is to use a joint element at the desired location

  1. Create a new point near to each point at which the lumped mass is required.  In this instance a gap between the two joint nodes is not significant in fact it is actually helpful when assigning the mesh/material properties.

  2. Define an appropriate joint element point mesh. 1 element division is automatically used for a joint point mesh.

  3. Define a local coordinate attribute such that (preferably) the local x direction lies along the length of the joint.

  4. Assign the mesh to both points.  On the mesh assignment form choose the option to select the local coordinate dataset.  Don't assign the local coordinate dataset directly to the line as this has a different effect and purpose.  The local coordinate system is needed because the joint elements and their stiffnesses/masses work in local coordinates, hence, specifying it directly lets you know which stiffness/mass operates in which direction.

  5. Define a joint geometric attribute and enter a value of zero for eccentricity if none is required.

  6. Assign the joint geometric attribute to the points (only really required on the 'Master' assignment points).

  7. Define a joint material (use "General" properties).  The material properties defined are in terms of the local coordinate system used in the joint mesh assignment.  Local element axes can be visualised by selecting the option "Show element Axes" from the Mesh layer in the Layers tab of the Treeview.  The stiffnesses should be input as zero and the masses in accordance with those required.

  8. The mass location is dependent on the order of the points selected.  The first node corresponds to the first point that was selected when defining the joint.  The first point is where the joint mesh marker is displayed (a Z symbol by default). Make sure that the mass is operating at the correct location (pay attention to the Mass Position in the input dialog).  

  9. Assign the joint material to the points (only really required on the 'Master' assignment points).

  10. Fully support the new point that you defined in step 1 above.

In the image below the horizontal line has been assigned with 3D thick beam elements.  The vertical line represents the joint to which the lumped mass has been added.  Note the local coordinate system definition and the local element axes for the beam and the joint element.  The mass has been applied at the first node and therefore at the end of the beam.  The point at the other end of the line has been fully fixed.

innovative | flexible | trusted

LUSAS is a trademark and trading name of Finite Element Analysis Ltd. Copyright 1982 - 2022. Last modified: November 29, 2022 . Privacy policy. 
Any modelling, design and analysis capabilities described are dependent upon the LUSAS software product, version and option in use.