ANSYS - Plastic strain energy 1

[Fergus_b96]

Dear all,

I am currently undergoing my dissertaation on non linear FEA of pressure vessels. I am investigating certatin failure criteria of pressure vessels, and one requires me to calculate plastic strain energy for a given applied load parameter, in this case, internal pressure.

I see that ANSYS has a strain energy tool when calculating a solution. I am wondering if there is any way to calculate specific plastic strain energy, as opposed to total strain energy.

Thanks in advance.

Fergus

 

[scheah]

Hi Fergus,

Ansys strain energy SENE includes both elastic and plastic strain energy (link). You could use ETABLE to get plastic strain energy density and volume to calculate the plastic strain energy.

Before solving, remember to include all output:

outres, erase, all
outres, all, all

For a simple static case, my_sene = (my_sendE + my_sendP)*my_volu.

/post1
set, last
etable, my_sene, sene 

etable, my_sendE, send, elastic ! elastic strain density
etable, my_sendP, send, plastic ! plastic strain density
etable, my_volu, volu ! element volume

smult, my_seneE, my_sendE, my_volu, 1, 1
smult, my_seneP, my_sendP, my_volu, 1, 1

ssum ! Adds it up

! Extract energy sums
*get, my_sene_sum, ssum,0, item, my_sene   ! total strain energy
*get, my_seneE_sum, ssum,0, item, my_seneE ! elastic strain energy
*get, my_seneP_sum, ssum,0, item, my_seneP ! plastic strain energy

Kind regards,
Jason

 

[L_K]

Jason:

Is there a difference between using

send, plastic / eppl, eqv

and

send, elastic / epel, eqv ?

 

[scheah]

Hi L_K,

Is there a difference between using
send, plastic / eppl, eqv
and
send, elastic / epel, eqv ?

Please see link for equivalent strain calculations. This is different from energy calculations (link).

From ETABLE documentation:
send, plastic = plastic strain energy density
send, elastic = elastic strain energy density
eppl, eqv = plastic equivalent strain
epel, eqv = elastic equivalent strain


Kind regards,
Jason