User login


You are here

Tensile coupon test - simulation of tensile coupons (after necking)

I have carried out several coupon tests (rectangular coupons similar to
those of ASTM E8). Some of these tests have kind of weird behavior. The
problem arises when I simulate results with ABAQUS. It goes pretty well
until a few steps after necking. Test and ABAQUS results match exactly
until several steps before fracture. After this point, there is a
discrepancy between results and my attempts in capturing the observed
behavior was unsuccessful. (around 10% or more plastic strain).
FORCE-DISPLACEMENT curve from experimental result show a more plateau
type curve after necking, with a sharp decrease in force right before
fracture. I am unable to capture this part. I think it can be
attributed to the fact that stress, in experimental test, remains
uniform and no stress concentration or necking takes place until a
sudden necking followed by fracture.
In my models, I either have
necking take place, say right on time, or no such necking takes place
and strain remains uniform and entire length of the specimen takes part
in elongation.

Recently I applied a virtual load around the
center of the coupon where we should expect necking in ABAQUS. I used
second order accuracy and incompatible modes. All of these enabled me
to come up with the right deformation (necking at centre instead of
somewhere else or having multiple necking along the length of the

I would appreciate any suggestion.

Ron, PhD 


Image icon Problem-1.JPG124.99 KB


Hi Ron,

        The difference is due to this:

1) The conventional formulas used to calculate the true stress  after the point of maximum load are not valid because triaxial state of stress develops and stress cannot be calculated using the formula load/Instantaneous area..

2) And you might have entered the data calculated directly from Load/current C/S  in abaqus true stress vs plastic strain column..

One has to follow an iterative trial and error procedure to find the true stress-strain data after the point of maximum load in an uniaxial tension test..


Hi Rohith,


 Actually I am aware of this. I did three tests from one batch of specimens so they are supposed to have similarmaterial properties.

I can simulate the exact behaviour in one of the coupon specimens. For the second and third, I have the mentioned problem.

ABAQUS, itself, is quite sensitive, too. A very small change in material properties, say increasing stress equal to 2% at plastic strain equal to 200% and keeping the stress and strains up to necking, unchanged (changing the stress and strain in these two model, only after necking and equal to only 2%) has caused the specimen to change the behaviour like that the photo is attached.


Honeslty, I think the problem can be contributed to the initiation of multiple-necking type phenomenon or perhaps delay in necking due to continues uniform elanogationin entire the length of specimen.


While trial and error seems a good idea to develop a similar force-deformation curve up to the fracture, I believe, in any case, our stress values cannot be reduced and the rate must be always increasing (in other words, while a reducing true stress-true strain data can produce a similar force-deformation, we cannot use it as in reality this is impossible).


What do you think?


Hi Ron,

The first thing is to provide abaqus with perfect true stress vs. plastic strain data atleast upto 95% of the true strain...

And one more important point is real materials contain imperfections and voids etc which grows due to deformation and lead to failure. But the models which we built or the theory developed is for virgin materials. And if you want see a sudden decrease in load, you have to use damage mechanics theories which will consider the deterioriation of the material strength and they will match your load displacement perfectly.

As you are using dog bone specimens and the cross section of the gauge length is uniform. Neck will iniate at some point but I couldn't understand the concept of multiple necking. U can give a small imperfection of .1% in width at some section to localize the strain..

And rememeber FEM doesn't consider any failure phenomenon in it. 



I agree with 1% imperfection. About the failure, I already considered that the specimen experiences first cracks, leading to fracture as soon as a sharp sudden drop in the force-displacement curve. So, I already have neglected this part (and filtered the curve) in all test results.

As mentioned, in two (let's call in specimens 2 and 3) out of three specimens that I tested,  failure displacement were glamorously higher (between 14 to 24 percent higher). ABAQUS, on the other hand, is able to capture the force-displacement up to failure for the specimen with failure at lower displacement (specimen 1). So, I don't think this is attributable to the void or similar issues.

As I said, I think in the second and third specimens, an instability (say no necking or uniform elongation takes place in specimens). I cannot say that the state of stress is not triaxial as I can see the poisson's effects and therefore the triaxiality along the gage length (part of the coupon with shorted width). This means to me that the necking was not localized.

I am able to capture similar behaviour (uniform elongation up to higher strains) with ABAQUS but the last, say 5-10% of curve is not similar to the real test behaviour. 

My question is why the last 5% of the force-displacement is rather different? Perhaps a void is being grownyet the length of the void was not enough to cause the fracture.Still cannot believe that this small void can cause such a weird behaviour.

In simulations, we can play with the specimen such that it produce what we want. If we don't have the test results, how can we generate this result and say that the displacement at strains equal to maximum 100% are equal to for example 36 mm in ASTM E-8 (dog bone) coupons?




And one more thing,

Force-Displacement curve at the mentioned last 10% cannot be produced unless we change the material properties of the mild stees (True stress-Plastic strain) in ABAQUS entry such that thetrue-stress drops. This seems impossible to me as the true stress normally grows with increasing the true-strain. Of course, in this last 10% no fracture or visible cracks were observed and I neglected the part of curve after crack/fractur.

Hi ron,

The stress carrying capacity of a material element slowly degrades before failure and in our constitutive relations this phenomenon is not included where as a factor (1-D) incorporated in the constitutive relation will capture this behaviour where D is damage and its growth depends on stress triaxiality ...

The properties are different from specimen to specimen as during the processing of cold rolled sheets various degrees of anisotropy will come into the picture...



Hi Ron & Rohith,

I am quite new to this I-mechanica and found this interesting since i am stuck in similar situation. However, I am simulating it in Pamcrash with some subroutine at my disposal. But i guess, i am going wrong somewhere in predicting the force-deflection curve post-necking. Even if you simulate the tensile test with some standard material model in your respective sofwares i think until necking one has no problem. For example, the true stress true strain curve obtained from force deflection experimental data is valid only until necking. One can apply swift law to the same and find its parameter to implement in simulation (No need to use the data experimental data itself!!). In turn this will give good result until necking..quite close and good! But how do i extend my simulation in post necking areas. I am clueless coz neither true stress true strain formulas nor the mentioned Swift Law is valid after necking. I have read some where that inverse finite element analysis (assume that true stress true strain curve extends as piece wise linear function after necking ) could be used to troubleshoot this but have no idea how to go about it. Any help or suggestion would be appreciated. I think i understand the theory behind the phenomena but unable to simulate!



    Refer Chapter-3 in the following thesis


Thanks Rohith for giving link to the thesis.

I will get back to you after i implement the learning from the thesis to my simulation.




I have found out an inverse way for evaluating the post necking stress strain curve through simulation. I brief the steps below:

1. Experimental data from a uniaxial tensile test is used to define the stress strain curve until the onset of necking.

2. Post necking the equivalent stress is assumed to be a piecewise linear function of equivalent plastic strain.

3. Let us assume that strain at necking is called e1 and maximal strain at the onset of fracture is called e2. And the strain hardening modulus at e1 is called H1.

4. Let us assume at this time that stress strain curve is linear between e1 and e2, with a slope H, such that 0≤H<≤H1.

5. The aim is to find such a value of "H" for which the force-displacement predicted by the simulation corresponds to the experimental force-displacement curve. The portion of the stress strain curve comprised between e1 & e2 affects the simulated force displacement curve only beyond a critical displacement value.



Your approach seems fine, linear assumption may hold good. What are the accuracy levels, it would be bettter if u can post the simulated vs experimental stress/strain plot. The best way is to set up an optimization problem  and obtain the best fit of parameters for your model.



Due to the nature of this job, i cannot post any data but yes the resulting simulated ss plot is quite close and no where greater than 10% post necking until fracture. By the way, did you mean to set up the optimization problem in Excel SOLVER to determine the best fit model parameters? If yes, then in this case we can get parameters only until necking and predicting whole curve would not be right. What you say?


I actually didn't mean of using excel, but you can also try this. Using the data till necking. Make different fits for different plastic strain ranges like [0-0.1], [0-0.2], [0-0.3] etc. Compare the load displacement plots with these data and identify the best fit.


Hello Ron

I am trying to make a tensile test simulation in ABAQUS but ı have difficulty to implement damage criterions in model. I would be pleased if you can send a examle inp. file.

Thanks in advance 

Subscribe to Comments for "Tensile coupon test - simulation of tensile coupons (after necking)"

Recent comments

More comments


Subscribe to Syndicate