Your Partner in Simulation Technology

How to Create a Flexible Body for the SimXpert Motion Workspace

Published 2013-05-16

To create a flexible body for the SimXpert Motion workspace is very easy and simple for simpleparts or for parts where a uniform mesh is sufficient, but in some cases, to obtain the required mesh, you might need all the tools from the Structures Workspace to create it,


maybe you have an existing FE model of a part that you want to use as a flexible part in a SimXpert Motion model, so

How do you create a flexible part (for the Motion Workspace) in the Structures workspace?

This tutorial assumes you can create a finite element model allready and only need the steps to set it up for use in the Motion workspace.


Summary (process in brief):

1) Remove any existing loads or boundary conditions.

2) Define interface nodes.

3) Create a list of the interface nodes

4) Setup a Modal Analysis (SOL103)

5) Submit the Analysis

6) Replace the rigid part with the flexible part

7) Complete and simulate the model in the motion workspace

Detailed Steps:

1) Remove any existing loads or boundary conditions.

The flexible part will be constrained in the motion model and external loads will also be applied there (loads in the structures model will be ignored in anycase but constraints will affect the flexibiltiy of the part dramatically and should therefore be removed when preparing the flexible body).

2) Define interface nodes.

You need to consider how this flexible part will be connected in your Motion model.

In some scenarios a flexible part will only interact with the rest of the parts in the Motion model throught contact (and not be connected directly), in which case you may skip this step, but such cases are rare and only adds to model complexity and long analysis times.

i) In most cases the part will have predefined attachment points (areas) where it will be connected throught joints to other parts. In the motion workspace these joints need a unique location for which you need to provide a single node in you FE model. Let's call this the interface node.

ii) Since your part will not be connected to only this single interface node (which will most likely be an ill representation of the reality and only cause extremely high and localised stresses) you should define the load transfer face in your model. In the FE model you do this by connecting the interface node with all the nodes on the area where the load transfer will occur with an RBE2 (or CBEAM, CQUADR, CTRIAR or RBAR elements since these elements supports 6 degrees of freedom at each node).

The image below highlights the surface through which forces between the conrod and the piston head will be transfered.

EnginePiston 02

Therefore we will create an interface node in the centre and connect it to all nodes on this surface with an RBE2 element. Using the "Mid Location" option below creates the location node automatically in the mass centre of the surface. If this node is required elsewhere, the node can be created manually and referenced using the "Specify Node" option.

EnginePiston 03 EnginePiston 04

3) Create a list of the interface nodes

The interface nodes need to be put in an analysis set (the ASET) since SimXpert will not make any assumptions on your behalf as to which nodes it will be.

EnginePiston 05

It is assumed at this stage that you have assigned material and properties to your part (NB: Ensure that density has been specified for the material)

4) Setup a Modal Analysis (SOL103)

After creating a modal anlysis job in SimXpert, a few aditional solver settings has to be set in order for SimXpert to know that an MNF (Modal Neutral File), also called a flexible body, has to be created for the motion workspace (or for use in Adams).

These settings are set under Solver control as shown below.

EnginePiston 06

i) The creation of a Flex Body is requested.

ii) The number of modeshapes are requested.

This is the number of dynamic modes that will be calculated. In this example the possible total number of modes in the MNF will become 10+2x6=22 since there are 2 interface nodes with 6 DOF each.

iii) Select all the required output for visualization purposes.

iv) Eventhough the analysis will be done for the complete model, the shown stress results could be reduced to only certain parts to reduce file sizes by excluding unnecessary data. In this model the conrod was the only part that was meshed so it was only important to select it at least.

v) Select the created ASET from Step 3.

EnginePiston 07

vi) Select Grid Point Stress output request (otherwise no stress results will be availble for display in the Motion workspace on the flexible body)

EnginePiston 10

5) Submit the Analysis

Submit the analysis and after completion, an MNF will be availble.

6) Replace the rigid part with the flexible part

Open the part's properties and under the Flexible Body tab, tick Model Part as Flexible and point to the newly created Modal Neutral File.

EnginePiston 08

7) Complete and simulate the model in the motion workspace

EnginePiston 09

Leave a Reply

Your email address will not be published. Required fields are marked *

One comment on “How to Create a Flexible Body for the SimXpert Motion Workspace”

crossmenu linkedin facebook pinterest youtube rss twitter instagram facebook-blank rss-blank linkedin-blank pinterest youtube twitter instagram