I would like to generate the stress strain curve for a cubic unit cell with many elements in Abaqus. Is it just outputting stress and strain of one element and combine them together? Thanks.
Hello Qingqing,
For one given element, you can extract any strain and stress time curve.
In the "Tools" menu of the postprocessor, select "XY Data" then "Create". Select "ODB field output" or "ODB history output" depending on how you chose to stock the results you want to combine.
Assuming you chose "ODB field output", in the pop-up window first chose the "position" of the output variables you want to combine (integration point in general but there are other possibilities). Then click on the "Elements/Nodes" tab, then "Edit Selection" : you can either chose to "pick from viewport", or enter "element labels", "element sets" or "internal sets".
Once you picked the element (or elements) you want to combine results on, go back to the variables tab and pick the ones you're interested in. Let's assume you're simulating a traction on a one element cube in the Y direction and you want to plot the normal-stress vs true normal-strain : pick S22 and LE22. Once you've done that, save these variables so ABAQUS keeps them in memory (for example, let's call S22 "normal stress" and LE22 "true normal strain").
Again, go in the "Tools" menu => "XY Data" => "Create" but this time chose "Operation on XY Data". In the "Operators" menu, look for and double click on "Combine(X,X)", then double click on the XY Data you want to use as input argument (LE22 so "true normal strain") and finally double click on the XY Data you want to use as output of your function (S22 so "normal stress").
Click on "Plot Expression" or "Save As...", and you have your stress-strain curve.
If you want to display the average stress in a mutli-element model vs the average strain, you can also create XY Datas containing stress and strain for each element, and then use the "avg((A,A,..))" operator in the "Operate on XY Data" menu, and finally combine the results. Though it can get pretty painstaking if you have a lot of elements, in which case I would recommend using a script.
It gives stresses and strains at each element. You can extract stress and strain variation with time and plot the stress-strain curve from that. If the geometry does not have any variation, you will have same stress and strain in each element.
Hello Qingqing,
For one given element, you can extract any strain and stress time curve.
In the "Tools" menu of the postprocessor, select "XY Data" then "Create". Select "ODB field output" or "ODB history output" depending on how you chose to stock the results you want to combine.
Assuming you chose "ODB field output", in the pop-up window first chose the "position" of the output variables you want to combine (integration point in general but there are other possibilities). Then click on the "Elements/Nodes" tab, then "Edit Selection" : you can either chose to "pick from viewport", or enter "element labels", "element sets" or "internal sets".
Once you picked the element (or elements) you want to combine results on, go back to the variables tab and pick the ones you're interested in. Let's assume you're simulating a traction on a one element cube in the Y direction and you want to plot the normal-stress vs true normal-strain : pick S22 and LE22. Once you've done that, save these variables so ABAQUS keeps them in memory (for example, let's call S22 "normal stress" and LE22 "true normal strain").
Again, go in the "Tools" menu => "XY Data" => "Create" but this time chose "Operation on XY Data". In the "Operators" menu, look for and double click on "Combine(X,X)", then double click on the XY Data you want to use as input argument (LE22 so "true normal strain") and finally double click on the XY Data you want to use as output of your function (S22 so "normal stress").
Click on "Plot Expression" or "Save As...", and you have your stress-strain curve.
If you want to display the average stress in a mutli-element model vs the average strain, you can also create XY Datas containing stress and strain for each element, and then use the "avg((A,A,..))" operator in the "Operate on XY Data" menu, and finally combine the results. Though it can get pretty painstaking if you have a lot of elements, in which case I would recommend using a script.
In accordance with Mr. Lebard, to plot stress_strain, use XY data => Field output=> choose the stress=> the single element or the hole model ( from elements/nodes)=> save
after do the same thing for the strain
After come back to XY data=> operate on XY data => choose "combine" from the the available operations and introduce your stress and strain => plot
I hope to help you
John
Hi Qingqing,
If you will be repeating this process for several models (with some differences between each), I would recommend putting this process into a script, which can then be run from the command line. It is relatively simple to create a script that loops over all elements, calculates average stresses and strains and then outputs them to a file.
food for thought . . .
1. The stress - strain curve is a material property which is dependent on a number of variables such as strain rate, orientation and thickness.
2. In the case of titanium sheet and plate, the elastic modulus can vary from 16 - 18*10^6 psi based on rolling method (actually, the texture.)
3. When performing analyses involving plasticity, it is proper to use the "true" stress strain curve rather than it common counterpart - the "engineering" stress strain curve.
4. Many papers available if you want to investigate.
According to Qingqing, I would like to have another question that what node or element should I choose to draw stress-strain curve?
Hi Sagar,
There is a feature in ABAQUS (at least v6.12 and the following ones) that records the actions you're doing (like clicking, selecting an element, etc.) and puts them in a script (in Python). I think it is called "Macro Manager". You can edit what' you obtain, test it until you have a functional script (which gets you the results you want).
hi
guys could you help me how can i analysis the micropile's behavior ?
specially in Abaqus.
i don't know which nodes i should to select.........
What if I want to calculate the homogenized stress and strain plot for which the formula is = STRESS(i)*EVOL(i)/Sum(EVOL)
If you are considering small strain for a tensile like test, I would recommend to apply the load to a reference point and couple the point to the end cross-sectional surface. Then request the force displacement and post process those to stress strain. For finite strain and plasticity involved consider the averaging as suggested by Etienne Lebard.
cheers!
how to go from the red curve to the orange what are modifiers that can i use?
Using combine function you can create the two XY data. Go to XY data>odb field output. Select stresses and strains for a node/element. Then close the window. Press again create XY data>operate on XY data> combine>add the 2 variables in the function and that's all.
- Badges
- Science topic