how do i input stress strain data for a mat into abaqus from lab tests

[matthat]

i have a sheet of plastic tubes that i have done a compression test on and i have the stress strain data that i have converted to true stress and true strain as it says to do in the manuals. it is an elastic plastic and has a typical stress strain curve, how do i put this into abaqus, it is not simply input xy data in as abaqus wants only ascending data , the data i have is not ascending, it has the initial elastic peak then the plstic curve. i ahve youngs modulus and poisson ratio.
i want to be able to do impact tests using a striker on the material with an anvil underneath
any help out there

 

[matthat]

here is my stress stain data

 

[curlyq]

I'm not sure about impact tests, I've never attempted to simulate these, but I ran into the same problems you are with non-ascending data from tensile testing. The problem is that for some stress values you have the same strain. Essentially, you have two Y's for a single X. I had to input my data into a stats package (I used OriginPro8.1), and was then able to "average" the curve which interpolated between the data points and reduced the number of data points. This essentially eliminated the irregularities. Good luck.

 

[matthat]

im not sure if it just the case of smoothing because i have the initial elastic peak then it drops before the plastic curve, should i just be putting in the plastic part of the curve in up to its peak?

 

[curlyq]

I think you are going to need a full material model, not just the plastic region. Otherwise, how is ABAQUS going to know what to do before the plastic region is reached?

I might be confused from your material data, though. I see an initial point of strain=0.687789991 and stress=0.101316845, the final strain=0.288831924, stress=18.1861244. So is this actually all upside-down? Shouldn't the smallest strain be first, and increment to larger strains? This could be part of the problem since ABAQUS requires the strain be in ascending order. Furthermore, I see in the file you posted, that the 3rd and 4th strain levels are the same, yet have different stress values. ABAQUS has a really hard time with this. You can only have one Y (stress) value for any one given x (strain) level.

Finally, where is the data for everything leading up to the data you posted? I have my excel plot attached here just to make sure we're thinking of it in the same way. (is Stress in Mpa?)

 

[matthat]

this data is from a compression test i attatch the data here
force vs displacement on a 15mm thick piece surface area 89mm
youngs modulus 76mpa poisson 0.3

 

[mrgoldthorpe]

Engineering strain in Col F should be A/15 (deformation over original length), not C/15. Strain will then sensibly increase with load, not decrease.

Having done that, is the region with strain below 0.12 a proper material response or are we just seeing 'settling in' of the test, followed by elastic response? If the latter, I suggest you adjust the stress and strain origins to remove this initial behaviour.

Is the elastic overshoot, followed by softening, then hardening expected behaviour of the plastic? I'm not too familiar with plastics; but I suppose it could be.

In any case, I suggest you follow curlyq's advice and smooth the data. I use Excel and undertake a 'n'-point averaging process, using increasing values of true strain as the independent variable.

 

[mrgoldthorpe]

I get the elastic modulus to be about 1200 MPa (1.2 GPa), assuming your units are N and mm. This seems reasonable, though perhaps a bit on the low side:

http://www.matweb.com/reference/tensilestrength.aspx

http://www.engineeringtoolbox.com/young-modulus-d_417.html

 

[mrgoldthorpe]

addendum 2:

I see it's a compression test. You must take proper account of the sign of the strain (as you do implicitly in cols C and D) and of course the stress. The resulting behaviour presents a different picture for compressive stress versus compressive strain following initial yield.

 

[matthat]

the material is a sheet of plastic tubes 0.08mm thick walls with 6mm diameter, after the initial lplastic peak the tubes start to crumple and then harden as it is crumpled,
thanks for your help i will try sorting out the strain now

 

[curlyq]

I am not extremely familiar with compression testing, but is this type of test an accurate material test? You are not only testing the material, but also the geometry and any initial conditions and imperfections of the tube. I'm just tossing an idea out. I would agree with the others with their thoughts on the sign of the strain.

To mrgoldthorpe - the softening and subsequent hardening of plastic materials (at least in tension) is typical of plastics. The polymer chains initially yield, then realign in the direction of the tension.

I wonder if the stress/strain response you are seeing after your initial yield is an accurate response, however. Also, is this only a singular test? If so you should have more to average the curves. Material properties based off of singular tests are not entirely reliable.

 

[matthat]

i have done 4 tests with results identical
. the material is very consistant

 

[curlyq]

If you already have four tests, a simple average should go along ways to helping your material data be in the ascending order as ABAQUS needs. Remember that ascending refers to the strain values, you don't need ascending stresses.

 

[matthat]

right i have taken the deformation over original length to get the strain ascending and this seems to be working. now all i have to do is work out how much force is transfered to the anvil, i need to replicate a force transducer, any ideas,
i have an impactor falling onto the anvil with the platic in between