Borehole bottom axisymmetric analyses in abaqus

[benoitvalley]

Hello - I try to model displacements and stresses about a borehole bottom drilled in a rock mass with initial stress conditions. I want to start simple, elastic material properties, axisymmetric model. I use CAX8R elements. I use "*Initial conditions, type=stress" to set my initial in-situ stress. I use a static step to calculate stresses/displacement. I always get strange displacement pattern. Even in the case when I include no borehole centered on the model axis (just modeling a cylinder) and I pinned all boundaries, I get displacement which I do not expect.

See attached an image of my ABAQUS model output (displacements not as I expect) as well as for comparison the output for the same problem from another FEM package (Phase2, Rocscience) that produces the output I expect.

Any idea what's wrong in my abaqus model ?

Thanks- Benoît

 

[benoitvalley]

Hello.

I have done more tests on this issue and still do not understand what goes wrong. I believe now that the issue is with the initial stress conditions and the equilibration in the initial step. However, I don't understand what is going on during the initial step.

I build a very simple axysymmetric model (just a rectangular model, i.e. a cylinder), fixed all the boundaries and applied initial stress conditions (compressive). Since all is boundaries are fixed, I expect nothing to happen in this model, i.e. to obtain a homogenous stress state throughout the model equal to my prescribed initial stress. I get however unexpected results, with stress concentration on the model axis and displacement of the internal nodes toward the model axis. I attached the input file for this simple test. Did any body experienced this before ?

Thanks.

 

[IceBreakerSours]

Although I have not looked at the image carefully, are you sure you are consistent with your units?

http://www.eng-tips.com/faqs.cfm?fid=376

 

[benoitvalley]

Hello. I believe I am consistent with my units.

I use a linear elastic material with a Modulus of 65 GPa and Poisson ratio of 0.25 which is typical for a ~granitic rock.

I have in-situ stress conditions of -50MPa, -20MPa and -10MPa (negative for compressive stress) which corresponds to deep conditions with high differential.

Borehole size is not critical for the magnitude of stress concentration (in a linear elastic model). Displacement will scale to the opening size.

In the two images I am presenting in my initial post, I carefully selected the same model size, material properties, boundary and in-situ conditions. I think the different results come from the initial equilibration step. I am not sure what phase2 is doing (it is a black box) but the results are intuitively right. I don't understand what abaqus is doing either, but the results are intuitively not the expected one (in both presented cases, i.e. in my first post with the borehole model or in my second post with just simple cylindrical model).

... so I still struggling with this axisymmetric models .... any help is welcomed...

 

[IceBreakerSours]

Assuming you are simulating the exact same problem in both codes, I can not say for sure. But if you are not entirely sure, confirm the following:

Have you tried CAX8 elements, instead of CAX8R, in ABAQUS? Did you use an analogous element formulation in the other package? Although this may not be a factor, is the time-stepping for the static step the same in both packages?

http://www.eng-tips.com/faqs.cfm?fid=376

 

[benoitvalley]

Thanks IceBreakerSours for your advices. I'll follow up with your suggestions.

I will also follow up on another aspect they I may have wrong. I fund on-line a document describing geotechnical analyses with abaqus ([URL unfurl="true"]http://62.213.117.104/upload/upload/analysis-of-geotechnical-problems-with-abaqus.pdf[/url]). Concerning in-situ stress initialisation they mention the following:

In most geotechnical problems, a nonzero state of stress exists in the medium. [...]

ABAQUS provides the ∗GEOSTATIC procedure to allow the user to establish the initial stress state. The user will normally specify the initial effective stresses using ∗INITIAL CONDITIONS, TYPE=STRESS, GEOSTATIC and in the first step of analysis, apply the body (gravity) loads corresponding to the weight of the material.

Ideally, the loads and initial stresses should exactly equilibrate and produce zero deformations. However, in complex problems, it may be difficult to specify initial stresses and loads that exactly equilibrate. The ∗GEOSTATIC procedure is used to reestablish initial equilibrium if the loads and initial stresses specified are not in equilibrium. It will also produce deformations while doing this. If the deformations produced are significant compared to the deformations caused by subsequent loading, the definition of the initial state should be reexamined.

For my problem, I don't want to have a gradient with depth as implied by the *GEOSTATIC procedure (I am modelling deep conditions where stress gradient are insignificant over the length of my problem) and I used a *STATIC step. However, I did not pay any attention to the issue of stresses and load equilibration and I believe this is what is causing me some grief... Phase2, the other package I am using, is developed for Geotechnical analyses and I believe these things are dealt with implictely. I need then to figure out the proper way of initialising the stresses in my abaqus model and balancing the loads (possibly using *DLOAD ?). If any body knows precisely how to do that, advice are welcome and will save me some trial and error.

 

[benoitvalley]

I found my mistake: for my case, in a axisymmetric analysis, radial (x-direction) and out-of-plane (z-direction) initial stress magnitude must be equal, i.e. not only the problem geometry must be axisymmetric about the y axis, but also the stress state. For example the following will work properly:
*Initial conditions, type=stress
alle, -5e7, -2e7, -5e7, 0

Initially, I put different values for x- and z- initial stresses which results in an unbalanced situation that would lead to relatively large deformation at the first step in order to balance the problem. What confused me, is the referential in which the initial stresses are defined: global or local (axisymmetric ~ polar) coordinate system ? It seems that they are define the global coordinate system.

 

[IceBreakerSours]

Great! Thanks for posting the solution.

http://www.eng-tips.com/faqs.cfm?fid=376