×
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

Different results between NASTRAN and ABAQUS

Different results between NASTRAN and ABAQUS

Different results between NASTRAN and ABAQUS

(OP)
Hello everyone,

I made the same analysis in NASTRAN and ABAQUS in order to compare their performance and results.

It's a modal dynamic analysis (half sine shock), the shock is 0.011 s long and my analysis time is 0.22 s in order to see the behavior of the structure after the shock.

In ABAQUS I used the following command lines:

*STEP, INC=200
*MODAL DYNAMIC, CONTINUE=NO
0.0011 , 0.22
*MODAL DAMPING,MODAL=DIRECT, DEFINITION=FREQUENCY RANGE
0.0,0.03
400.0,0.03
*SELECT EIGENMODES, DEFINITION=FREQUENCY RANGE
0.0,400.0
*BASE MOTION,DOF=1,AMPLITUDE=CHOC_11ms,SCALE=9.81,TYPE=ACCELERATION

Where CHOC is an input file where my half sine coordinate are set.

For NASTRAN I used the following commands:

SOL 112
DLOAD = 101
TSTEP 100 200 0.0011 1
TLOAD2 101 101 ACCE 0.0 1.1E-2 45.45455270.0
TABDMP1 4 Q
+ 0.0 16.7 400. 16.7 ENDT
SPCD 101 174482 1 9.81
ENDDATA

SOL 112 is based on a cosine so I used a phase of 270 in order to obtain a sine.

The thing is that if I plotted the acceleration OUTPUT of the same node from both analysis I have a similar behavior but I observe differences (see attached picture).

I do not know where the differences come from, do you have an idea?

The blue curve is NASTRAN and the orange one is ABAQUS

Thks

RE: Different results between NASTRAN and ABAQUS

You have a very slight differnce in fundamental freq. There may be a difference in how the finite elements are treated, differences in meshing, or differences in how the diff. eqtn. is solved (newtonian iteration or runge-kutta or ...?)

RE: Different results between NASTRAN and ABAQUS

(OP)
The analysis is based on the same FEM model (made in Hypermesh and exported in .inp for ABAQUS and .dat for NASTRAN) so I have the same number of nodes, elements, materials.

I made a previous modal analysis and I obtained the same frequencies, modes and effective masses with both codes.

Yes this is MSC NASTRAN.

I first thought that it was problem of a difference between the sine defined by ABAQUS and NASTRAN but I plotted the curves of total acceleration at the excitation nodes to see if both codes used the same input excitation. They are the same, so I think maybe the problem comes from the damping coefficient.

n NASTRAN I have the following values for the damping (I used CRIT type): Q=30, G/2=1/2Q so G=0.03333 and CRIT=0.01667

In ABAQUS I put G as the modal damping values (don't know if it's the right approach)


RE: Different results between NASTRAN and ABAQUS

"maybe"? Of course the damping affects the fundamental frequency.

RE: Different results between NASTRAN and ABAQUS

(OP)
Of course I agree it is important in this kind of analysis my point was about the origin of the difference between results.

Well in fact I am not sure it is the source of my problem here. I just run a sine sweep frequency on both codes and I obtained the same curve for the acceleration vs frequency (following the direction of the sine sweep). So I suppose my damping coeff are good here.

So I join you on your first impression it's maybe the way the diff eqt are solved.





RE: Different results between NASTRAN and ABAQUS

"a cosine so I used a phase of 270 in order to obtain a sine" ... 270deg ? not 90 deg ??

another day in paradise, or is paradise one day closer ?

RE: Different results between NASTRAN and ABAQUS

(OP)
In order to have a positive input signal.

I agree with you, I first put 90 deg but my input signal was negative and I had to apply a -1 factor to my shock in order to have the same input than the one in ABAQUS. I then tried 270 deg and I have a positive signal without adding my -1 factor.

By the way in both case (phase=90 and -1 factor and phase=270 without -1 factor) give the same results (the curve in my first post)

RE: Different results between NASTRAN and ABAQUS

"half sine shock" ... =0 at t=0, =max at t=0.011 ? (a sine wave period = 0.044sec ?)

sin(x) = cos(x+270)

another day in paradise, or is paradise one day closer ?

RE: Different results between NASTRAN and ABAQUS

(OP)
Yes

So adding a phase of 270 is right we are agree?

My half sine shock is 0.011s long so the max is at 0.0055s, so a period of 0.022s.

RE: Different results between NASTRAN and ABAQUS

sounds right ...

another day in paradise, or is paradise one day closer ?

RE: Different results between NASTRAN and ABAQUS


The critical damping you calculate is 0.01667, but that not what you have entered in your nastran SOL112??

RE: Different results between NASTRAN and ABAQUS

just eyeballing your 2 inputs....

You use a 0.03 (or 3%) modal damping in ABAQUS analysis whereas for NASTRAN you use a Q damping of 16.7. Which equates to a critical damping ratio of 1/(2*16.7) = 3%, so your modal damping becomes =2*3% = 6%. This doesn't explain the phase shift that you see but maybe you can redo your analysis with consistent inputs for both solvers.

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