You are here
Simulate a uniaxial compression test
Hello all,
What is the step and load arrangement you impose on an ABAQUS model to simulate a uniaxial compressive stress test similar to that regularly performed on a concrete cube? Is it done on ABAQUS Explicit or Standard?
I believe the load rate is 6000 N/s untill complete failure of the specimen.
Thanks
Hussam Nasreddin
Forums:
Typically you will want the
Typically you will want the setup shown in the link below for any uniaxial tension test (if you can understand my terrible drawing). You create a unit cube (all sidea have length 1 to make the math easy later). You constrain the DOF at the nodes as shown. This will create a uniaxial tension stress state. To get compression, simply reverse the direction of the prescribed displacement.
http://i.imgur.com/fs7Nz.png
That said, there can be issues with compression tests that this wouldn't capture. If you were simulating something with large strains (rubbers and the like) you can get issues where in the experiment the loaded faces cannot move freely in the plane perpendicular to the loading due to friction. This makes your final stress state something other than uniaxial tension/compression.
As far as step type it comes down to your model. Are dynamic effects important? If so, use explicit. Is your material model sufficiently complex that Standard won't converge? If so, then you'll probably need to move to a quasi-static Explicit model. Barring those two situations, I'd go Standard, since it tends to be a lot faster.
My Company - Red Cedar Technology
Thanks
Thanks for your reply,
I am planning to do elastic analysis of a concrete cube which is assumed to have an initial elastic stress strain relation. So the material model is very simple as I just want to calculate strains at very low stresses. I guess dynamic effects wouldn't matter here and probably ABAQUS standard is good enough for the job.
I have looked at the figure in your link but I didn't quite understand the boundary conditions you are using. To simulate realistcally the compression test of a concrete cube, The two loaded faces of the cube will have restrictions in the x and z directions when the load is applied in the y direction (which you mentioned in your reply).
excuse my lack of knowledge here, I am not sure how I could make abaqus apply the load in increments of say 6000N/s for around 30 steps which should add up to 18MPa stress on 100mm cube. Barring in mind that I would like to examine the strains at each step when postprocessing the output data.
I hope this is not too much and thanks for the discussion
Regards
Hussam
The figure I included
The figure I included assumes the loading will be in the x-direction, but it doesn't matter as long as you apply the BCs correctly. Choose three adjacent faces, and make sure each cannot move in the direction perpendicular to it. This allows the cube to expand freely perpendicular to the load direction. You get uniaxial tension because Poisson effects are allowed to cause strain but do not induce any stress. If you're not sure, I would actually just build it quickly in a FE tool and run a linear elastic material model. You'll see that the cube will expand in the y- and z-directions according to the Poisson's ratio of the material, but the stress will be uniform throughout the cube. You should have S22, S33, S12, S23, S13 = 0 as well.
While you can implement the 6000 N/s load in Abaqus, I don't think you need to. Ultimately you're looking to compare the material model to the experiment via a stress-strain curve, correct? In that case, you can just apply a displacement to the cube in order to get the desired final strain which will allow you to compare against the experimental data. Is it necessary to get the data points lined up in terms of applied load? If not, you can just apply the displacement as I said and put maximum step size of something like 0.1. That will guarentee 11 points (counting (0,0)) on the stress-strain curve from Abaqus, more if it has to cut back for convergence. Decrease this value if you want more steps.
I hope that helps!
My Company - Red Cedar Technology