I want to visualize my results of the XFEM crack growth in form of a diagram with the time increments or the crack length on the horizontal axis and the Griffith' energy release rate G or the stress intensity factor K on the vertical axis. I am using the energy-based damage model.
I don't know, where to activate those values. The best solution for me is, if the energy release rate G can be transformed into the stress intensity factor.
When I do it for my own, I can use the formula:
G = KI² / E'. In my case, I have an axis-symmetric problem (crack propagation in a screw thread). Which E' can I use? That one of a plane strain problem type (E' = E/(1-v²) )?
Thank you for help,
Thomas
Hi,
On my knowledge, recent versions of Abaqus use XFEM to model crack propagation by choosing a difined criterion. If the model is well built there are several posibilities to perform post-processing treatment if the parameters are defined a priori. I think SIFs or crack tip position can be known easily when the crack propagates.
I could not find the option. I activated several parameters in the "Output History". These parameters are saved in the calculation,but these parameters are energy parameters and something like that. The crack length is also available. But I cannot find the option for the fracture parameters like SIFs or Griffith parameter.
Can you give me the value that I have to activate?
I know :-). But my task is trying out XFEM as newer alternative without remeshing.
Apart from that, XFEM works also with VCCT. Therefor I assume that there is also a possibility to get the G-values.
When I will do a calculation with VCCT (remeshing) later, I at least know who to ask.
how to calculate the energy release rate in ABAQQUS ? please
For those still unsure about this issue, one can simply add ENRRTXFEM to the field output requests, i.e. something like:
*Element Output, directions=YES
S, STATUSXFEM, ENRRTXFEM
To do so, either modify the input file, or edit the model's Keywords from CAE.
I think, STATUSXFEM, PHILSM and PSILSM are values, I can get in CAE by clicking. But those values have no really importance for fracture mechanics.
The value ENRRTXFEM seems to be very interesting, because it includes "all components of strain energy release rate when linear elastic fracture mechanics with the extended finite element method is used." (eXtended Finite Element Method (XFEM) in Abaqus by Zhen-zhong Du). I am using the linear elastic fracture mechanics. Is the strain energy release rate the same like the Griffith' energy release rate? In the theory, the Griffith' energy release rate is determined with the strain energy, when I remember correctly.
I checked it with an arbitrary 3D-model and my 2D-model, but in both cases, I got the value of 0,0 despite crack opening in the Visualization module. You know why?
Griffith was the first to compute the strain energy release associated with crack growth, which is probably why you refer to it as the Griffith' energy release rate. I am not aware of any distinction between the two, please notify me if one does exist.
The value ENRRTXFEM is not available via clicking, which is why I included it via a Keywords change.
On your question regarding the 0,0 value; in my model this is also the case for crack initiation, i.e. until XFEM predicts the crack entering the second element. Afterwards nonzero values arise. Do you have the same or are zeros predicted throughout the whole crack development?
I included it also with "Edit Keywords". It is quite easy. If this is the final solution, it would be very nice for me. But why is Abaqus not able to include it in CAE since v. 6.9?
Maybe, my model does not calculate correctly. I have in the moment just a crack prediction, but it doesn't really open (in the Visualization module). This could rather be the problem. Have you experience with this problem? In my screenshot, the crack seems not to open in the crack tip. There is still the highest stress intensity in the former crack tip. The crack flanks seem still to be connected to each other. What can be the problem here?
I will try to find out, if this is the same energ release rate like the Griffith' one. I will later solve the problem by remeshing the crack tip after each step. You have for this purpose the option to use the Griffith' release rate in CAE, I think. So I can compare the solutions.
Sorry, I've not yet seen this kind of behavior. Is this for a simple mode I loading case or are you subjecting your geometry to complex loads? Maybe try a simple model first (eg square plate with a notch and mode I pressure load on the exterior) and subsequently move on to this complex case?
Feel free to keep me informed on your progress, and I'd like to hear the outcome of the comparison to the remeshing case.
It is just a axissymmetric model of a screw thread with contact to a nut thread (see pictures). The load is static. The only complex thing is the contact maybe, but this shouldn't make a problem. The calculation without crack works fine.
Optically, it is imagined like a "zero energy mode". But I think, there should not be a correlation to the given problem. What kind of elements would you take for this? And which material law? Maybe it is meshed too fine? The arbitrary 3D-block, I have modelled, does also not really work. The crack is respected, but it doesn't open.
What are you doing with XFEM? Can you maybe send me a working input for comparision?
I suppose meshing too fine isn't possible when vcct is considered. I suggest you take a look at this very simple tutorial I appended by Matthew Pais. Also take a look at his website, where some examples are provided: www.matthewpais.com, if you haven't already. Note that this one is his only example where ENRRTXFEM is used to extract energy release rates. It should at least help you identify why your arbitrary block doesn't show opening.
Personally I am exploring the use of XFEM in combination with the Abaqus Direct Cyclic approach to predict fatigue crack growth in (simple) test samples. But this is also still a work in progress.
Thanks! I just downloaded it myself yesterday on Scribd. I found this on iMechanica. It looks as if the energy release rates are the same (in this paper). In the moment I am making an easy axissymmetric sample to compare the release rates from the XFEM solutions with the Griffith' release rates of a sample solved by remeshing. The solutions deviate about 20% from each other. I cannot estimate, if this could be normal.
My final aim is also loading the screw thread by a cyclic tensile loading. But I have not yet an idea now, how to handle this problem. I have a little problem with understanding the theory for this. If I want to get a SIF-crack length-curve, I have somewhere to input the Paris' law, not? This is in my view the only solution, that makes sense.
I didn't follow this tutorial since I only found it after I got it working. How exactly do you conclude that the energy release rates look the same, since the legends aren't included in the graphs? Does mesh refinement (for the XFEM problem) increase the correspondence between the two approaches?
If your final problem concerns non-critical fatigue crack growth, i.e. with stress intensity factor/energy release rate below the critical SIF/G, than you can not create such a graph without such an approach with the Paris law, or equivalently a damage propagation law, since the static crack would simply not propagate. If you'd know the path of crack propagation you could however obtain the graph you request by hand, but this doesn't seem to be the case. Personally I found the paper "Development of a Benchmark Example for Delamination Fatigue Growth Prediction" by Krueger (2010) very explanatory. Note however that he applies it to a debonding scenario. For XFEM approaches see the Abaqus Benchmarks Guide; search for: "crackprop_hole_fatigue_xfem".
Again the incorporation of the fatigue behavior (Paris law) is not available via CAE.
No, it doesn't increase. I do not think, that I made a mistake. I try it tomorrow with Franc2D as independent software. This was an axissymmetric problem. I will also try it with plane stress or plane stain. Maybe it does only work with plain elements. I indeed do not know why, but maybe.
I will take a look in those papers. They seem to be informative. I of course will deal with the Benchmark Guide. I have two ones. They both are good.
In Abaqus are the two commands *fatigue and *direct cyclic. They both can be used, but I have until now no idea, what to do with them.
Is it with the contour integral possible to let the crack propagate? I didn't find the function. Is it the same with power law and something like that like in XFEM?
I haven't tried axisymmetric elements, but they should be working since Abq v6.12. As far as I'm aware the fatigue command goes hand in hand with the *direct cyclic keyword, I am not aware of a specific *fatigue keyword. The usage of these should become clear when you start investigating the direct cyclic approach (paper from Krueger, etc.).
I did not yet try the contour integral within Abaqus yet to predict SIF/SERR, but I did try the 3D tutorial from Matthias Pais I posted here earlier and it doesn't seem to work. Specifically requesting the contours in the history output is not allowed, I receive the error:
The following history output requests are applied to XFEM cracks which are not stationary XFEM cracks.
So this leads me to think it isn't possible to use contour integrals from propagating cracks, but this assumption might still be premature.
Edit: I made one small error following the tutorial, indeed NOT allowing the crack to grow makes the derivation of the SIF contours possible.
Hello Thomas, did you solve that problem?
Is it possible to calculate the griffith' energy release rate G or the stress intensity factor K ?
I didn't get better results than I described in the comments. I will try it next week again.
I think so that Griffith's energy model is somewhat (how to say politely?...) ... not true for some forms of Cracks' propagation .....
sir can anyone help me.? I want to calculate the energy release rate for crack propagation in XFEM using a "cohesive segment approach".what type of output request we select.?
- Badges
- Science topic