Learning Forum

[Rafael Gomes]

Hello everyone!

I'm using the Workbench Autodyn to perform a simulation of a tubular structure using a honeycomb unit cell under compression displacement. I need to plot the graph Force x Displacement. Is it possible to generate this graph using Autodyn? I'm only aware of the stress x strain.. 

Thanks in advance!

[Chris Quan]

Are you trying to obtain the total force on the unit cell with the displacement of the cell? 

If yes, before you run the model, in Autodyn GUI at cycle 0, you need to activate External Force Variables via OUTPUT -> HISTORY -> SELECT PART SUMMARY VARIABLES and check appropriate boxes for total external force, external contact force, external coupling force, or external boundary force. When calculation starts, AUTODYN will write these forces to ident.sum file. You can view the time history of total forces through HISTORY -> PART SUMMARIES after the calculation has finished.

To convert the time history to Force vs Displacement curve, you need to put gauge points at nodes of the face where the force is applied at cycle 0, activate displacement variables via OUTPUT -> HISTORY -> SELECT GAUGE VARIABLES, and check appropriate boxes for displacement components. When calculation starts, AUTODYN will write these displacements to ident.his file. You can view the time history of displacement compoenent through HISTORY -> GAUGES POINTS after the calculation has finished.

Finally, you can write both outputs using History -> Write Text Output to text files and then use Excel to edit them to get the Force vs Displacement curve.