×
INTELLIGENT WORK FORUMS
FOR ENGINEERING PROFESSIONALS

Log In

Come Join Us!

Are you an
Engineering professional?
Join Eng-Tips Forums!
  • Talk With Other Members
  • Be Notified Of Responses
    To Your Posts
  • Keyword Search
  • One-Click Access To Your
    Favorite Forums
  • Automated Signatures
    On Your Posts
  • Best Of All, It's Free!
  • Students Click Here

*Eng-Tips's functionality depends on members receiving e-mail. By joining you are opting in to receive e-mail.

Posting Guidelines

Promoting, selling, recruiting, coursework and thesis posting is forbidden.

Students Click Here

Jobs

ANSYS - Plastic strain energy

ANSYS - Plastic strain energy

ANSYS - Plastic strain energy

(OP)
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

RE: ANSYS - Plastic strain energy

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:

CODE --> APDL

outres, erase, all
outres, all, all 

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

CODE --> APDL

/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

RE: ANSYS - Plastic strain energy

Jason:

Is there a difference between using

send, plastic / eppl, eqv

and

send, elastic / epel, eqv ?

RE: ANSYS - Plastic strain energy

Hi L_K,

Quote (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

Red Flag This Post

Please let us know here why this post is inappropriate. Reasons such as off-topic, duplicates, flames, illegal, vulgar, or students posting their homework.

Red Flag Submitted

Thank you for helping keep Eng-Tips Forums free from inappropriate posts.
The Eng-Tips staff will check this out and take appropriate action.

Reply To This Thread

Posting in the Eng-Tips forums is a member-only feature.

Click Here to join Eng-Tips and talk with other members!


Resources


Close Box

Join Eng-Tips® Today!

Join your peers on the Internet's largest technical engineering professional community.
It's easy to join and it's free.

Here's Why Members Love Eng-Tips Forums:

Register now while it's still free!

Already a member? Close this window and log in.

Join Us             Close