Learning Forum

[Ajay Vignesh Natarajan]

Hello all,

I am working on a project where I have to perform two impacts, where the second impact should incorporate the deformations from the first impact. I am using the full deck restart method with d3full from first impact as the restart file. I have the keyword *STRESS_INITIALIZATION in the master file of second impact, but still I don't see any deformations from the first impact in my model. I have prestress in my model model using dynamic relaxation. Can anyone please guide me on how to incorporate the deformations from the first impact?

Thanks in advance!

[Reno Genest]

Hello Ajay,

Do you have the original input file (first_Impact.k) and the restart file (2nd impact; restart.k) in the same folder? You should have results of the first impact (include dynamic relaxation state at time=0) in the d3plot. When you restart, LS-DYNA will continue the d3plot file series as d3plotaa and keep adding results. It should look like this:

So, when you open the d3plot file, you will get results from the first and second impacts.

I recommend doing some tests with a simple cube model. This way you will be able to run quickly and make changes as needed.

Here is the full restart procedure from our knowledge database:

"Changes of a general nature can be made in a full restart, including addition of parts, loads, and contacts.  

 Sample execution line  

SMP:  lsdyna i=fulldeck.k  r=d3dump01

MPP:  lsdyna i=fulldeck.k  n=d3full01

where fulldeck.k is a complete keyword input deck for the model you want to use moving forward in time.  

Copyright © 2003-2012 by LIVERMORE  SOFTWARE  TECHNOLOGY  CORPORATION                        

Full Restart (cont’d)

 Guidelines for fulldeck.k 

 Include keyword input for anything that is to be retained from the original run… (*PART, *SECTION, *MAT, *CONTACT, *LOAD, etc.).  Normally, you would just copy the original input deck and strip out anything you don’t want to retain.  

 Also include keyword input for new parts, materials, contacts, loads, etc.

 Include all relevant *DATABASE and *CONTROL commands.

 Include the command *STRESS_INITIALIZATION.

 Signals to LS-DYNA this is a full retart and that stress, strain, displacement, etc. are to be initialized for specified, pre-existing parts.

 Do not use *INITIAL_VELOCITY for nodes carried over from previous run.  Use *CHANGE_VELOCITY_option  to modify velocities of such nodes.

 Preexisting contacts that are to be retained should include the _ID option so that the contact ID numbers in the original input deck match those in the full restart input deck. 

 Regarding output from a full restart:

 Binary output (d3plot) from a full restart will blend seamlessly with previous output.  

 ASCII output (glstat, matsum, etc.) from a full restart appends to pre-existing ASCII output only if *CONTROL_OUTPUT with IASCII=1 in included in the full restart deck.

 Without this command, ASCII output from full restart overwrites pre-existing ASCII output.

 Lastly, there may be a suitable alternative to using a full restart.  

 For example, a “dynain” file can be written at the conclusion of the original run by including the command *INTERFACE_SPRINGBACK_LSDYNA in the original input deck.   This dynain file can be included in a subsequent keyword input deck to initialize nodal coordinates and element history variables (stress, strain, etc). "

https://ftp.lstc.com/anonymous/outgoing/support/FAQ_docs/restart.pdf

https://ftp.lstc.com/anonymous/outgoing/support/FAQ/restart

 

Let me know how it goes.

Reno.

[Reno Genest]

Hello Ajay,

We recommend doing a small restart if possible; small restarts are usually more stable than full restart.

 

Reno.

[Reno Genest]

 

Hello Ajay,

An alternative to a full restart would be to use the dynain.lsda file to initialize the model (nodal displacements, stresses/strains, etc.) in a second analysis. Have a look at Appendix X in the LS-DYNA User Manual Vol I:

https://lsdyna.ansys.com/manuals/

 

Reno.

 

[Ajay Vignesh Natarajan]

Hello Reno,

Thank you for your response. I tried the small restart method, it worked and I have the deformations from first impact. In the original input file, I have included two impactors and defined initial velocities for both impactors using *INITIAL_VELOCITY_RIGID_BODY (as 0.0 for second impactor). I am using *CHANGE_VELOCITY_RIGID_BODY in the small restart deck to change velocity to the second impactor, but it does not work. I have also tried using *CHANGE_VELOCITY_GENERATION and still I could not get the second impactor to move. Please help me with this issue.

Thank you!

[Reno Genest]

Hello Ajay,

Are you getting error or warning messages in the messag or d3hsp files?

I recommend building a simple cube model to perform a small restart. Get the process working on a simple model and then move on to a more complex model.

Note that Ansys employees are not allowed to download or upload files on the Ansys Forum.. If you are a commercial customer, please create a support case and we will have a look:

customer.ansys.com

 

You can still post your model here on the Ansys Forum and other users might be able to help you.

 

Reno.

[Ajay Vignesh Natarajan]

Hello Reno,

There were no error messages. I used the small restart and it worked. The solution was to include the second impactor in the original input file without any velocity definitions to it. Then in the restart file, I assigned velocity to it by using *CHANGE_VELOCITY_RIGID_BODY.

BR,

Ajay.

[Reno Genest]

Hello Ajay,

Ok, thank you for letting us know. Your solution might benefit other users.

Have a great day!

 

Reno.