How to calculate stress intensity factor using LUSAS FEA software 1

[aircraftengr]

Hi,
I was wondering if it was possible to calculate the stress intensity factor, of a specimen using Finite Element Software, specifically the LUSAS (London University Stress Analysis Software) software. Usually stress intensity factors,K require the slightly more complicated Mode I and Mode II calculation before proceeding to obtain the value per se. I have been able to use the software to calculate stress concentration factor, by obtaining the nominal stresses and maximum stresses.
If this software cannot be used for this particular calculation, what other Finite element software is recommended? I have Algor, Patran, Nastran and Marc

 

There are a number of methods you can use with any FE code to get K, but probably the most reliable and least mesh density intensive is to first obtain the energy release rate and then calculate K. The reason I say this is that the FE solution for strain energy converges relatively rapidly (at least compared to stress). You can also use the displacement extrapolation method with approximately the same degree of accuracy as the energy release rate method for a given mesh density. I'll outline the energy release rate method below since this is a fairly general procedure.

To speed up solution convergence I would recommend using 8 noded quadrilateral elements and modifying the elements at the crack tip to a degenerate triangular form using the quarter point technique - this will force the displacement functions to contain a root r radial dependence and the stress field to contain the inverse root r singularity characteristic of LEFM. Note that you do not have to use the quarter point technique with the energy release rate method, but you'll want to make sure that your strain energy solution is well converged before attempting to calculate the energy release rate.

Simply model the structure with crack lengths of "a" minus "delta a/2" and "a" plus "delta a/2", where "delta a" is "small" relative to the crack. For each solution, extract the total strain energy and calculate the energy release rate as G = (1/B)(dU/da), where B is the thickness, dU is the differential strain energy, and da is the associated change in crack length. Then relate the energy release rate to stress intensity using the appropriate equation ... K = sqrt(G*E) for plane stress or K = sqrt(G*E/(1-v^2)) for plane strain.

Piece of cake.

 

[aircraftengr]

Visitor 2002,
Thanks a lot for the info. Using the energy method is tedious but looks like there's no choice.

 

No prob -

By the way, you eluded to mixed mode loading in your original message. As a reminder, the procedure I outlined is only valid for single mode loading. It will work for any mode, but each mode has to be considered independent of the others (this is actually a fundamental concept). Anyway, simply apply mode I loading alone to get GI and KI and then apply mode II loading alone to get GII and KII.

Also, there are FE codes out there that provide post processing capabilities to obtain stress intensities in a fairly direct manner. ANSYS, STAGS, StressCheck and Mechanica all come to mind, and I'm sure there are others, but I don't think ALGOR has this capability, and I'm pretty sure PATRAN does not either (at least the version I use does not).

Cheers!

Good luck

 

[KSshopper]

Most of the crack growers I know use FRANC2D/L exclusively, which, convienent enough, is available free through KSU. Download at

http://www.mne.ksu.edu/~franc2d/.

Franc has a feature which lets the user insert a crack tip then automatically and incrementally extend the tip to record a new stress intensity. This feature will also automatically remesh the crack tip and adjacent area with each new increment!

It will then give you Stress Intensity for Mode I, Mode II and the J integral. It has one drawback: it's only applicable to through the thickness cracks. For part through cracks I've used Franc to create a weight function.

 

[aircraftengr]

Visitor 2002,
I see. So I basically apply one mode at a time on the displacement extrapolation method. I was advised by someone to assign the initial value (for example) of 1.000 and then a second value of 1.001 to obtain the difference in energy. I assume it applies to both Mode I and Mode II. Is that similar to "Simply model the structure with crack lengths of "a" minus "delta a/2" and "a" plus "delta a/2", where "delta a" is "small" relative to the crack."?
By the way, I'll check out ANSYS, STAGS, StressCheck and Mechanica. Have you heard of ABAQUS? Will that code be helpful for stress intensity factor?

 

aircrafteng

The displacement extrapolation method is different from the method I outlined (I outlined an energy approach). The displacement extrapolation method is actually a more simple method, but it requires a highly converged displacement solution which may prove difficult depending on the resources you have at your disposal.

The advice you received regarding the incremental crack lengths for use with the energy method is good. If you're interested in the stress intenstity for a crack length of 1.000, it might be better, though, to bound this value so as to reduce differential error - i.e use crack lengths something like .995 and 1.005. Apply mode I loading alone to get GI amd K1. Apply mode II loading alone to get GII and KII.

philcondit had a good suggestion as well. FRANC2D/L is available at no charge and is a useful tool in obtaining stress intensities. If the problem you are working on is work related and a fairly quick answer is required, I too would recommend at least looking at FRANC2D/L.

However, if you are doing more fundamental research you will likely want to use a more generic/more capable FE code. ABAQUS would be a good choice in my opinion as would ANSYS. Both of these codes have extensive element libraries, very good non-linear capabilities, and are widely used in the research community.

In your original message you mentioned that you have access to a PATRAN pre/post processor and both NASTRAN and MARC solvers. The PATRAN/NASTRAN package is used extensively in the aerospace community as a generic finite element code. It is a pretty good combination though NASTRAN is limited in its ability to model contact and non-linear problems in general. MSC markets the MARC solver to provide, among other things, more capability in these areas. Anyway, the combination of PATRAN/NASTRAN and/or PATRAN/MARC should do nicely, though you may need to do a little more manual post processing (for fracture problems) than you would with some of the other codes mentioned here.

Cheers!

 

[aircraftengr]

Actually, I'm doing more fundamental research. Might be publishing a paper of the findings. I just completed my thesis entitled "Finite Element Analysis of Notched Specimens with satellite holes around the notch". This is basically an extension of the said project.

Unfortunately my University has limited FEA codes/packages. So I don't have access to many software. By the way, I did check out FRANC2D/L and ANSYS (trial package). Can ANSYS be obtained free?

Cheers!

 

I've been researching wake effects using ANSYS ... more specifically, how contact, friction, and large displacements effect near tip fields. ANSYS works well for this application, but it is pretty expensive, and I wouldn't be using it if my University wasn't able to supply it.

I would say that if you have access to the MSC code listed in your original message (PATRAN/NASTRAN/Marc), I would recommend using this. Your handle is aircraftengr, so I assume you are interested in working in aerospace. Its been my professional experience that most aerospace companies use MSC software in some capacity, so getting used to using it would be a good thing. Also, the combination of PATRAN/NASTRAN/Marc, is pretty comprehensive. You should be able to model virtually any behavior you're interested in studying with this.

Best of luck

 

[aircraftengr]

Yes, I'm studying Aerospace Engineering and majoring in Aeronautics. However, I've decided to specialize in the strength and behaviour of materials.

I'm trying to get used to all the FEA software I can get my hands on. No such thing as knowing too much in this field.

Thanks, I need the all the luck I can get!