Introduction

In many applications, a prestressed structure is subject to dynamic events that occur over its usable life.  Simulating such prestressed dynamic events is a cost-effective means of assessing the capability of the structure to withstand such loading prior to costly validation prototyping and testing.  LS-DYNA is the industry standard simulation tool for simulating such events.

Until recently, developing an LS-DYNA model to first prestress a structure followed by a dynamic event loading was conducted almost exclusively using LS-PrePost or other third-party preprocessors.  Various standard methods exist to perform the prestress analysis:

1. dynamic relaxation with bolt pretension
2. implicit static or dynamic prestress
3. explicit, damped dynamic prestress
4. linked LS-DYNA and LS-DYNA Restart systems in Workbench
5. ...

In this article, we are going to utilize Ansys Workbench to pre- and post-process a prestressed structure that is subject to a ball impact using method 3.  As will become evident, with a few LS-DYNA keywords added to a standard Workbench LS-DYNA model, this process is very straightforward.

Example Model

To illustrate to process of setting up the model in Workbench LS-DYNA, we will utilize a model of a Nylon 6 cover that is mounted to a (rigid) steel plate, sealed with a Neoprene O-ring, fastened with four bolts.  After the bolts are tightened, a rigid, steel ball will impact the cover with an initial velocity generated from a drop at a certain height, a common regulatory test for electronics enclosures.

As shown in the second image, the prestress step consists of tightening the bolts to specified compression of the O-ring, typically expressed in %-compression, followed by large artificial damping to mollify dynamic effects.

The timeline of events is detailed in the following table:

Workbench Model Setup

In this article, we detail the model setup in Workbench LS-DYNA that is specific to the method of this article.

Contacts

The contacts that need special attention are between the nuts and bolts.  In order to displace the nuts followed by locking their position, duplicate contacts are needed: frictionless contacts between the nut hole (ID) and bolt body (OD) that will be converted to bonded (tied) contacts at 30 ms.  The following figure shows these contacts within the Connections branch:

In order to convert the (second set of) contacts to tied contacts at the correct birth time of 40 ms (bt=0.04), the following keyword snippet must be applied to each such contact:

Finally, the (top set of) frictionless contacts must be deactivated in order for the tied contacts to take over.  A small overlap time was chosen, thus by using a Contact Properties object for each frictionless contact, the death time can be implemented.

Nut Displacement (Bolt Tightening Prestress)

A Displacement boundary condition scoped to each of the four top nut faces accomplishes the bolt tightening prestress.  Using Birth and Death, we kill the displacement at 40 ms so that the tied contacts take over:

Damping

Using the Keyword Manager, we use the *DAMPING_GLOBAL and *DEFINE_CURVE keywords to implement the artificial damping from 31 - 39 ms.  The damping load curve definition and its implementation in *DAMPING_GLOBAL is shown here:

Initial Velocity Generation

To commence ball impact at 40 ms, *INITIAL_VELOCITY_GENERATION and *INITIAL_VELOCITY_GENERATION_START_TIME cards must be defined.  The *INITIAL_VELOCITY_GENERATION card is defined as follows, noting that the units are in mm-N-s-tonne, and that the highlighted entries are required in order to start the initial velocity of a rigid body at a time after the initial time:

To define the *INITIAL_VELOCITY_GENERATION_START_TIME card using the Keyword Manager, Beta options must be turned on, otherwise a standard keyword snippet would be required:

*DATABASE_BINARY_D3PLOT (Optional)

This (optional) step is used to customize the time interval for writing results to the d3plot files for finer results resolution during the dynamic event with coarser resolution during the prestress time.  To implement this, we define the *DATABASE_BINARY_D3PLOT and *DEFINE_CURVE keywords using the Keyword Manager to define the output intervals over the time of the simulation via a load curve.  The database output intervals are shown here:

Finally, the *DATABASE_BINARY_D3PLOT card is configured as follows:

LS-DYNA Model Branch Snapshot

The following image shows a snapshot of the LS-DYNA model branch with all of the defined controls implemented; the Connections branch is not shown here:

Results

The following videos show the action of the bolt tightening prestress followed by the impact of the ball.  Note that in this model, the mesh is very coarse, and the material properties of the Nylon cover are linear therefore the stress values are very unrealistic.  Thus, this model would require much refinement before using its results for decision making.

Conclusion

Conducting a prestressed structural simulation on a system subject to a subsequent dynamic event is possible and straightforward in Ansys Workbench LS-DYNA.  Here, we chose to utilize explicit dynamics throughout a single simulation timeline in order to align with typical LS-DYNA modeling.  Additional methods are available for computation of the prestress using dynamic relaxation or implicit methods which have pros and cons associated with them; the correct method depends on the model as always.  Linked analysis systems through Workbench, i.e., an LS-DYNA system connected to a LS-DYNA restart system, is yet another potential method.  In conclusion, conducting sophisticated Ls-DYNA analyses using Workbench LS-DYNA is not only possible, but very straightforward, requiring a few keywords, made accessible through the Keyword Manager. 

Going Further

• Apply the same methodology to your model.
• Compare the model setup and results when using the method mentioned in the article versus using dynamic relaxation for the preload analysis.
• Implement the preload step using LS-DYNA implicit static or dynamic analysis followed by switching to explicit analysis for the impact analysis. 

Downloadable Resources

Model Archive (2024 R2 SP3)