Simulation Mechanical Forums (Read-Only)
Welcome to Autodesk’s Simulation Mechanical Forums. Share your knowledge, ask questions, and explore popular Simulation Mechanical topics.
cancel
Showing results for 
Show  only  | Search instead for 
Did you mean: 

ADINA shell & plate comparison

3 REPLIES 3
SOLVED
Reply
Message 1 of 4
scudelari
1034 Views, 3 Replies

ADINA shell & plate comparison

Dear Friends,

 

I am running some tests in Autodesk Simulation in order to verify the software’s accuracy (and to learn more about the technique we are employing so far in our calculations).

 

Basically a partner company of ours prefers to use ADINA due to the academic background of its staff. Therefore we were running some comparisons but unfortunately the results found in Autodesk Simulation do not converge.

 

The problems we are trying to verify are described in the ADINA Verification Manual Report ARD 04-10 September 2004, and are, in the attached document, called respectively:

    A.32  Pinched cylindrical shell, quadratic shell elements (page 58-59)

    A.33  Pinched cylindrical shell, plate elements (page 60)

 

The problem consists of a cylindrical shell that is pinched at the middle on both sides.

problem.png 

 

One of the references (attached Lindberg) of the problem states (PDF page 30) that E * t * wc / P = -164.24 which is used by the ADINA document as the theoretical value.

 

For this problem in Simulation I used the Nonlinear analysis because I could not define the elements as Shell in the Linear Analysis. The mesh was refined around the force application point.

R=100 in ; t = 1 in ; E = 3e7 lbf/in2 ; P = 1lbf ; L = 200 in

 mesh.PNG

 

The shell elements have their midside nodes included and were calculated as “Large Displacement”

Here are the results:

 results.PNG

Therefore, the displacement under the force application point is of 2.2567e-5 inches. Which gives us:

E * t * wc / P = 3e7 * 1 * 2.2567e-5 / 1 = 677.01 != 164.24

 

What are the possible reasons for such difference? I woudl like to see if it is actually possible to get closer to the theoretical results.

 

I also have some other questions:

1-      Why are shell elements unavailable for a Linear Analysis?

2-      Why can’t I include midside nodes of plate elements in the Linear Analysis?

 

I really thank everyone for the help on this matter!

 

NOTE: I COULD NOT ADD THE MODEL FILE DUE TO THE FACT THAT IT WAS TOO BIG. IF NECESSARY, I CAN SEND IT BY MAIL.

3 REPLIES 3
Message 2 of 4
John_Holtz
in reply to: scudelari

scudelari,

 

My guess is 677/4 = 169.25 which is about 3% high. (The applied load P = 4* your load due to the  1/4 symmetry?)

 

I did a coarse linear model with 400 elements (20 along the length) and obtained 162 which is 1.4% low.

 

Just for everyone's knowledge, the ADINA solution is using linear assumptions, so the MES analysis should be using small displacements. Since the displacement is so small, there should be very little difference.

 

 



John Holtz, P.E.

Global Product Support
Autodesk, Inc.


If not provided already, be sure to indicate the version of Inventor Nastran you are using!

"The knowledge you seek is at knowledge.autodesk.com" - Confucius 😉
Message 3 of 4
klnkai
in reply to: scudelari

You said "For this problem in Simulation I used the Nonlinear analysis because I could not define the elements as Shell in the Linear Analysis."

But referring to Autodesk Wiki the "Plate-elements" in ASIM Linear Analysis have five degrees of freedom + an artificial stiffness for the 6th. Isn't that what usually is understood under Shell-elements in literature (a superposition of plate and membrane-theory)?

Message 4 of 4
scudelari
in reply to: John_Holtz

Hello,

 

I did try again and indeed you are correct. That you for the help.

 

I also tried with an insanely coarse mesh and the resuts were still good.

 

Thanks again!

Can't find what you're looking for? Ask the community or share your knowledge.

Post to forums  

Autodesk Design & Make Report