Learning Forum

[Mahmoud_87]

Dear All, 

 

How to use a Prestressed LS-Dyna analysis? I need to use the date of static structure in LS-Dyna wrkbench module.

 

 

[Ram Gopisetti]

Hi, with the new versions of ANSYS 2022 and above, you can bing the dynain file which has the prestress data but this is corrsponding to lsdyna to lsdyna, however, you can export the deformed shap and export the stress at last time step and use external data to map into LSDYNA. but recent update will allow you to read the dynain.k file into structural analysis via mechanical model.

Cheers, Ram 

[Reno Genest]

 

 

 

Hello,

There are a few ways to calculate prestress in LS-DYNA. You could use explicit dynamic relaxation directly in WB LS-DYNA (no need to do an Ansys Static Structural analysis). This will use the LS-DYNA explicit solver to apply preload.

If you right click on the Dynamic Relaxation object in Mechanical, you will have options to add General preload (gravity, etc.) and bolt pretension.

Dynamic relaxation is an analysis that occurs before time 0 to apply the pre load and calculate prestress. Explicit dynamic relaxation is similar to performing an explicit dynamic analysis with some damping to find the static equilibrium under pre loads before time 0. We call this pseudo time.

Explicit dynamic relaxation is a good option if the preload is highly nonlinear and/or if you have rigid body motion. Using an implicit solver will not work well or not at all for those cases.

You will find more information here:

 

 

 

http://ftp.lstc.com/anonymous/outgoing/support/FAQ_docs/preload.pdf



Reno.

[Reno Genest]

 

 

Hello,

Another option is to do an implicit dynamic relaxation directly in WB LS-DYNA inside Mechanical (no need to do an Ansys Static Structural analysis). This will use the LS-DYNA implicit solver to apply the preload:

 

Reno.

 

 

[Reno Genest]

Hello, 

Or you could apply the preload using Ansys Static Structural and connect to an LS-DYNA system in WB:

In this case, in LS-DYNA Mechanical, you have to set the Dynamic Relaxation to "Explicit After Ansys Solution":

You will find more information in the Ansys documentation:

https://ansyshelp.ansys.com/account/secured?returnurl=/Views/Secured/corp/v231/en/lsdyna_ug/exd_ag_lsdyna_DR_kwds.html?q=dynamic%20relaxation

 

Let me know how it goes.

 

Reno.