×
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

Nonlinear Analysis

Nonlinear Analysis

Nonlinear Analysis

(OP)
I am performing a nonlinear analysis of a titanium tube using in hydraulic application on I-DEAS. My stress-strain curve has zero slope in non-linear range. This is the first time I use the program to do nonlinear analysis. Before this, I used NASTRAN to do the job. The result from NASTRAN looks good to me. However, for the result from I-DEAS, I got the maximum von-mises stress more than the yield stress. If I understand correctly, the max von-mises stress at the critical load should be not more than the yield stress. I don't know what I did wrong. Here is the information of my model.

- nonlinear analysis of titanium tube using in hydraulic application.
- Arc length method to find the maximum internal pressure.
- Yield strength = 105 ksi
- Young's modulus = 15000 ksi in elastic range and 0 in inelastic range
- Ultimate strength = 125 ksi
- poisson's ratio = 0.361

Can anyone tell me how to perform nonlinear analysis using I-DEAS?

TIA

RE: Nonlinear Analysis

I use the load control method not arc length.
If you have specified 0 for your plastic modulus I am surprised that you did not get errors because element stiffness becomes 0 once you pass yield. How can pastic modulus be zero when ultimate is 125 ksi and yield is 105 ksi, you have an increase in stress for increase in strain.
You can not perform classical plastic analysis (no increase in stress for increase in strain) in IDEAS because element stiffness becomes zero. Could you do classical plastic analysis in NASTRAN? I am not familiar with nonlinear NASTRAN. What you should do is enter your strain data for corresponding yield and ultimate stress and some points in between if you are using isotropic hardening if you are using kinemtic hardening you can only have a bilinear stress strain curve ie yield and ultimate only in material properties.

RE: Nonlinear Analysis

(OP)
fsi, thank you for you reply.

Yes, you are right. My ultimate stress can not be 125 ksi if the plastic modulus is zero. Actually, I have to run 2 cases. The plastic modulus will be zero for the first case and some number for the second case. Therefore, the ultimate of the first model should be 105 and 125 for the second one.

For the question you asked about nonlinear in NASTRAN, yes, we can do classical plastic analysis. You will just input zero for plastic modulus and 105 for the yield strength. However, I have no idea about the theory behind the code.

Here are my questions according to your reply,
1. How can I set the load step if I decide to use load control in my analysis (sorry, I am very new to I-DEAS)?
2. I still don't understand the difference between isotropic hardening and kinemetic hardening.

Thanks

RE: Nonlinear Analysis

1. GOTO
 Solution set
 Examine/Modify loading  
 Loading and Solution Control
 Add  
 Endtime Point enter value  Ok
 Highlite time interval
 Subincrement enter value
 Ok Ok Ok
2.Isotropic hardening assumes the yield surface expands uniformly. Kinematic hardening allows the yield surface to translate, but the size and shape remain constant.

RE: Nonlinear Analysis

Finite element programs use an extrapolation method to calculate stresses at nodes (from stresses at integration points). this extrapolation some times gives higher results than expexted. I suggest to use values of stresses at integration points or use finer mesh at your interest position.

RE: Nonlinear Analysis

Hai,

  Fsi:-

  From your explanation,I interprted as tangent modulus(In plastic region) is same in tension as well as compression.

  But in kinematic hardening,the tangent modulus differs,depending upon which side yield surface moves!


 Am I right? If wrong, please correct.


Regards,
Logesh.E

RE: Nonlinear Analysis

Hi
Logesh
You are right. In kinematic hardening for example if material goes plastic in tension then the compression yield is reduced. For steady loading isotropic hardening is acceptable but for cyclic loading isotropic hardening assumption is not correct. I usualyy use Ziegler/Prager Kinematic hardening if I have cyclic loading.
I am referring to steel here.
fsi

RE: Nonlinear Analysis

Hai,

  Thanks Fsi.

  Star for helpful/expert post.

 Regards,
 Logesh.E

RE: Nonlinear Analysis

ToohTaah:

You have zero slope in the engineering stress-strain curve.
For nonlinear analysis, you should give the true stress-strain curve, in that curve you won't have zero slope.

e_true=ln(1 + e_engineering)

CMFG

RE: Nonlinear Analysis

(OP)
CMFG,

I just wanted to test the if I performed nonlinear analysis correctly. That was why I have two models. The zero slope model is for testing. My real model has nonzero slope.

ToohTaah

RE: Nonlinear Analysis

CMFG
 Can you give me the reference handbook where u got the formula:
e_true=ln(1 + e_engineering)
thanks, fsi

RE: Nonlinear Analysis

The answer to fsi's question comes from basic definitions, not from a book of formulae.

Engineering strain is change in length divided by unstressed length.  This is a convenient approximation that is acceptable for small strains.

True strain is calculated with the denominator being the actual length at every stage along the way.  Expressed mathematically this becomes:

e_true = integral of (1/L) with respect to L, from L to L+E

where L is the unstressed length and E is the overall extension.

This evaluates to ln(L+E)-ln(L), which simplifies to the formula CMFG gave.

RE: Nonlinear Analysis

Just a quick caveat; make sure that you know what data the code which you are using is expecting (true stress, true strain, plastic strain, etc.).

Even though two codes can use an identical constitutive theory, they may (especially for metal plasticity) request different input, even though they ultimately operate in the same fashion.  I've been burned in this before. My recollection (and I could be wrong) is that Nastran requests true total strain as input, not plastic strain.

Brad

RE: Nonlinear Analysis

(OP)
fsi,

How can I put yield stress, ultimate stress and stress-strain data to my model? It seems that the result is not correct. I think I did something wrong in material properties input phase or setting up the analysis phase. If possible, could you please explain me how to do such things?

Thank you so much, ToohTaah

RE: Nonlinear Analysis

1.goto
material
create
change statics linear material to statics nonlinear material
properties
stree strain data
choose method (function,table,constant,etc)
enter stress strain values
2.goto
physical properties table
modify ur solid element type
plastic yield function=1
plastic hardening rule=#depends on your application

RE: Nonlinear Analysis

(OP)
fsi,

I did exactly the way you explained. My stress strain data is constant and displays correctly when I plot it. However, the analysis seemed not to stop when the stress reached the ultimate value. If I understand correctly, in static nonlinear material analysis, there is no field to put ultimate and yield stresses. How can I tell the program to stop at the ultimate stress?


ToohTaah

RE: Nonlinear Analysis

hi tooh taah,
             You cannot tell the system to stop at ultimate since itz doing simply number crunching. so if the value found to be high then your model is failing subjected to your loads & BC.

RE: Nonlinear Analysis

What do u mean by "If I understand correctly, in static nonlinear material analysis, there is no field to put ultimate and yield stresses. "?
Did not enter these values in ur stress strain data?
If the structure stress passes the ultimate stress IDEAS uses the slope of the last line segment for stiffness calculation
and it will even go to infinity if your model stresses happen to be that high. It will not stop at ultimate stress.
Does NASTRAN stop at ultimate stress automatically?
Look at your stresses and if your stresses are higher than ultimate that means the structure has failed or collapsed is a better term because sometimes failure is referred to yield stress.

RE: Nonlinear Analysis

(OP)
fsi,

Yes, I did put those values in the stress strain data. What I thought was the program would use only the stress strain data I input which has the ultimate stress at the upper bound (i.e. it will not extrapolate the value outside the range I gave). Now I understand how the program works. Thank you so much for all helps.

ToohTaah

RE: Nonlinear Analysis

hi toohtaah,
            One more point i want to add. The values yield & ultimate you are giving are used simply to find the slope of the curve after yield. If that curve is plotted the program gets the stress value from the obtained strain. So the stress will be taken depending on strain whatever the ultimate stress may be. The slope of the curve is going to be the same till you give the next entry as subsequent slope.

RE: Nonlinear Analysis

hi toohtaah,
            One more point i want to add. The values yield & ultimate you are giving are used simply to find the slope of the curve after yield. If that curve is plotted the program gets the stress value from the obtained strain. So the stress will be taken depending on strain whatever the ultimate stress may be. The slope of the curve is going to be the same till you give the next entry as subsequent slope. Hope you understood better.

RE: Nonlinear Analysis

Any one has any comparative data results between NASTRAN and IDEAS for a specific case of plastic analysis?
thanks

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