Should strain energy be used as convergence criteria in ANSYS? 1

[neat nate]

In CREO Simulate (previously known as ProMechanica) I used the maximum strain energy and maximum Von Mises stress as my convergence criteria. I first look for a plateau in the strain energy value as the order of the elements increases. Next I look for a plateau in the value of the stress as the order of the elements increases. This method is what my instructor taught us and has worked well for me in the past.

I'm now using ANSYS. I've created a simple model; a quarter of a rod with symmetry constraints and an applied axial load at one end so as to mimic a full rod that is fixed at one end and loaded at the opposite end; material is steel. I am again using max strain energy and max Von Mises Stress as my convergence criteria. But this time instead of increasing the order of the elements as CREO is programmed to do I increase the number of elements in the model. I then plot the number of elements vs the max strain energy and max stress.

I've noticed that the max stress converges very quickly (I compared it to hand calculations). However the strain energy does not converge. It instead approaches zero.

Is this normal behavior in ANSYS? Is strain energy not the appropriate convergence criteria to use? If it is not what is the appropriate criteria to use?

Thanks.

 

[L_K]

If you look at the strain energy plot, you will notice that it is plotted for each element. Thus the maximum value in the legend is the
maximum strain energy found in one element. As you decrease the element size, this maximum value will also decrease.

The smaller the element, the less work can be stored in it.

 

[L_K]

Under solution information you can add a stiffness energy result tracker into your solution. If you parametrize this value,
you should see it converging as the number of elements is increased, similar to equivalent stress.

http://imgur.com/a/9TGTs

Also if you add a command snippet including the following command, energies should be written in solve.out.

PRENERGY,ALL

 

[neat nate]

Thanks L K
I found the Result Tracker but the Stiffness Energy option is grayed out. I have searched the ANSYS help file to see why this is but haven't found anything yet.