Nonlinear Analysis

[ToohTaah]

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

 

[fsi]

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.

 

[ToohTaah]

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

 

[fsi]

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.

 

[theArcher]

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.

 

[elogesh]

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

 

[fsi]

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

 

[elogesh]

Hai,

Thanks Fsi.

Star for helpful/expert post.

Regards,
Logesh.E

 

[Cmfg]

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

 

[ToohTaah]

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

 

[fsi]

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

 

[Denial]

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.

 

[brad]

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

 

[ToohTaah]

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

 

[fsi]

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

 

[ToohTaah]

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

 

[thirumalai]

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.

 

[fsi]

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.

 

[ToohTaah]

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

 

[thirumalai]

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.