iMechanica - Delamination in Patterned Films - Comments

Hi Xiao, I am trying to

Biswas — Mon, 02 Apr 2007 03:18:33 -0400

Hi Xiao,

I am trying to implement a method to compute K for interfacial crack using ANSYS APDL. But my problem is to get the nodal force data at the crack tip (I am trying to use virtual crack closure technique). Could you please help me regarding this matter? If possible, please let me know the APDL command to get nodal force data.

Thanks.

Regards,

Biswas

"steady state"

Xiao Hu Liu — Fri, 22 Dec 2006 18:35:48 -0500

Hi Nanshu,

Thank you for the comments. As the delamination elongates infinitely, the energy release rate diminishes in all cases. Although it is hardly discernable in Fig. 7 for small w/h but it can be seen for w/h=1.5. The "steady-state" term is misleading; I should have used other one, "plateau" is probably appropriate, since the curves tail off to zero slowly as compared to the variation of the curves at small crack length.

The dotted curves in Fig. 7 are not of interest practically, as we discussed it in the paper, together with Fig. 8. Because, for a larger crack length, a significant portion of the crack surfaces behind the crack tip penetrate into each other. To resolve the artifact one need to include the contact in the model but this is not expected to give a larger driving force for the delaminaton. So we have no motivation to go further.

"Steady State" in Fig.7

Nanshu Lu — Thu, 21 Dec 2006 13:27:45 -0500

Hi, Xiaohu,

I read your paper carefully because I am doing research on stiff islands/ stretchable substrate interface delamination in flexible electronics. The paper is very well organized and gives very good analysis. I learnt a lot from it actually.

However, I have one question regarding to Fig. 7 in your paper. We can see a clear "steady state" for 2a/h>4. However, intuition tells us if the crack tip is far away enough from the gap, the gap infuluence will deminish which will result in no driving force. I am wondering if it is proper to call this "steady state" and from which point on the driving force begins to drop and eventually goes to zero.

I am using it now!

Ying Li — Thu, 21 Dec 2006 11:51:11 -0500

Now I am using the ANSYS to solve many questions about the biomechanics . If you have any questions ,you can contact me at the email : Lee2002hu@yahoo.com.cn

I think we can learn many things from our disgussion.

Can we get people from ANSYS involved in this discussion?

Zhigang Suo — Wed, 20 Dec 2006 11:18:34 -0500

Any of you know people working in ANSYS? Please forward this thread (http://imechanica.org/node/429) to them and urge them to participate in the discussion. In another thread about FEM, people from ABAQUS made valuable contributions.

ANSYS UPF

Xiao Hu Liu — Wed, 20 Dec 2006 10:51:51 -0500

You may want to check the Guide to ANSYS User Programmable Features after looking at the excellent introductory article User Programmable Features in The Focus. There is a user forum xansys where you can ask/answer questions. Sheldon's ansys.net is a great resource for ANSYS users.

ANSYS user programmable features not well documented

ruogang zhao — Tue, 19 Dec 2006 20:05:18 -0500

I’ve been recently looking into both Ansys and Abaqus for my research project. When I looked through Ansys manuals, I realized there are some manuals missing on the user defined material (USERMAT) in the standard released documentation. So I contacted the Ansys local support team. Surprisingly, they do have it! I guess those manuals are not included because you’ll be “using ANSYS in a nonstandard way”. I agree with Jie-Hua‘s comments, Ansys want less trouble when providing user programmable features.

More on ANSYS vs. ABAQUS

Jie-Hua Zhao — Tue, 19 Dec 2006 14:39:42 -0500

The other issue is the cost. Historically, ABAQUS charged much more to commercial users. ANSYS had more options on pricing, which cost much less. To universities, it was a different story.

Nowadays, PC with multiprocessors, multicores and multi-threads are widely used in the industry. The price issue is more prominent. ABAQUS charges by number of concurrent processors, ANSYS charges by number of concurrent jobs (when using its sparse and PCG solvers). This makes a huge difference in pricing. Say if I have a Windows XP 64 machine with dual-core, dual processor running with multi-threading on. I have effectively 8 processors to the FEM solver. When I run ANSYS, I pay $6600/year maintainance fee since we have bought perpeptual licenses long time back. If I run ABAQUS, I need 12 solver tokens plus one CAE token. ABAQUS sells their license by leasing. This will cost me about $30000/year. We just can not afford of having 10 simultaneous ABAQUS jobs running. However, we are doing this on ANSYS almost everyday.

In case of non-linear analysis, ABAQUS does have its advantage. But the gap is closing up after ANSYS implemented the 180 series elements.

ANSYS also has its user programable features, however, they tend to de-emphasize the capability. In releases 8.0 and 9.0, they even took the documentation of these features out from the standard CD distribution. You have to specially order the hard copies. I think this is because of their ISO9001 certification. They want less trouble with the auditors.

ANSYS vs Abaqus

charliezhai — Tue, 19 Dec 2006 01:07:21 -0500

Zhen,

Coincidently I recently discussed with Xiao-hu in the same context of your question: why ANSYS is more popular than Abaqus in the industry.

First off, I am not sure that's an absolutely accurate statement as both Intel and Motorola are populating Abaqus (explicit and implicit) in their companies as the main FEA code.

But I do want to offer a few possible reasons if your assessment is actually true. 1) ANSYS since day one has been a self-sufficient package with good preprocessing and postprocessing while Abaqus used to be standalone solver. I still remember 10 yrs ago I had to do all the pre-processing in Ideas before bringing it into Abaqus. Abaqus however has bought Patran and since then it seems a lot mroe attractive to me. 2) ANSYS actually has pretty good documentation, as opposed to what you said, in both theory manual and operation manual. and ANSYS scripting (APDL) is a mighty tool for coders like us. 3) Because of 1 and 2, ANSYS has a larger customer base.

However, every coin has a flip side. ANSYS is lagging behind Abaqus in developing new elements, incorporating new methodology (as VCCT, etc), User subroutine and UMAT, etc. The material library is also not as good. so we do see a potential shift from Ansys to Abaqus. ANSYS' recent acquisition of many CFD softwares (Fluent, CFX) is an effort to provide a full FEA solution with FEA as well as Finite volume, etc. Their integration efforts were simply horrible as I found the workbench plus so many adds on are just a mess of distraction rather than help.

Why industry usually use ANSYS instead of ABAQUS?

Zhen Zhang — Mon, 18 Dec 2006 22:37:39 -0500

Hi, Xiaohu, Jie-Hua, and Charlie,

Because all of you work in industry and are familiar with FEM softwares. I have a question. I just wonder why industry usually use ANSYS instead of ABAQUS? Last year, I was an intern in Fairchild, they also use ANSYS. So I had to use it. But I found that model tree in ANSYS is redundant and usually override each other, e.g. definition of reference temperature (maybe it is a small bug, and has been fixed). Another point I want to make is that the documentation is really not good. I cannot find the theory they use. But ABAQUS does it very well. And also an interesting phenomenon is that academia prefers ABAQUS instead of ANSYS. Why ? Could you please share the opinions with me?

Also I hear from my friends that sometimes the results from ANSYS are not reliable. How do you guys think?

More on VCCT

charliezhai — Mon, 18 Dec 2006 17:26:01 -0500

VCCT is the most convinient way of calculating G in a commercial FEA code. THe benefit becomes more obvious as it's applicable to both interfacial and homogensous crack. However it is limited in LEFM only and it's hard to calculate phase angle (can't identify the characterization length) explicitily.

While we opt to use APDL to code VCCT in ANSYS, Abaqus has VCCT built in its recent release. Another useful approach is cohesive zone, which is also built in Abaqus and ANSYS. However it's almost a nighmare if you try to get it converge ever in ANSYS.

ERR computation by Virtual Crack Closure Integral method

Jie-Hua Zhao — Mon, 18 Dec 2006 15:11:53 -0500

Along the line of "brute force computation", I want to add the following point:

A computational error check was made recently. It turns out that one can control the error well below 1% for a very abroad range of material mismatch if a special variant of the method is used. (see, J-H Zhao, Engineering Fracture Mechanics, 72 (2005) pp1361–1382). This kind of accuracy is comparable to the domain integral method.

ANSYS does not have the built-in command for contour integral calculation. However, its "Ansys Parametric Design Language" helps a lot. The flexibility of APDL makes the ERR calculation possible during postprocessing when using the virtual crack closure integral method. I will say if using ANSYS, VCCI may be the most suitable method to calculate ERR.

ERR computation

Xiao Hu Liu — Mon, 18 Dec 2006 10:44:46 -0500

Hi Zhen,

1. To calculate the energy release rate using the crack opening displacement one has to refine the mesh around the crack tip, usually within the range of about 1/10 of characteristic length, which, in our case, is the cap thickness. As long as the mesh is fanned out from the crack tip, the size of the finite element model can be controlled and the computation is tractable on a workstation. When fitting the displacements, one wants to make sure that only the displacements of the nodes within the K-controlled region are used. In our calculations a ring of singular elements are focused at the crack tip. But do not use the displacements at the 1/4 nodes where the results are usually poor. Using the displacements at the first few corner nodes from the crack tip, the energy release rate can be obtained with an accuracy of within few percent. Since I do not have access to ABAQUS 6.4, and ANSYS can only calculate K in a homogeneous material, I implemented the method to compute K for an interfacial crack using ANSYS APDL script.

ABAQUS uses domain integral (energy interaction integral) to compute the energy release rate. At relatively coarse mesh it often yields pretty accurate results.

2. This method was explored in the early days of computational fracture mechanics. The brute force computation usually does not yield accurate results, although other variants have been developed along the line to improve it.

Questions about the calculation of G

Zhen Zhang — Wed, 13 Dec 2006 17:29:23 -0500

Hi, Xiaohu,

This is an interesting study. It makes me learn more about the real problem in real structure. I have two questions.

Calculation of energy release rate. You use the fitting method. As we know, it is quite mesh dependence unless you use very fine mesh around the crack tip. But hc is smallest geometric feature size in your case, so the mesh size is at least several order of magnitude smaller than hc. The total calculation cost could be huge. From ABAQUS version 6.4 or above, it supplies G and mode angle directly as output, calculated by contour integral. It requires quite coarse mesh, compared with stress (or displacement) fitting. What’s your opinion and experience about this benefit of ABAQUS?
Two-slices method for Gss=U1-U2. In this situation, the difference between U1 and U2 are quite small, compared with U1 or U2 themselves. The numerical error could be on the same magnitude as U1-U2. So how did you solve this issue?

stress singularity could explain this

Zhen Zhang — Wed, 13 Dec 2006 16:57:03 -0500

Hi, Charlie,

About the effect of via-fill or crack-stop on the CPI type of delamination, I think the understanding from stress concentration might be helpful. Let’s think the Figure with two dissimilar materials, the singular stress field around the corner can be expressed by a power law relation stress ~ r^(-p), with r the distance from the corner and p the singularity exponents, by solving an eigenvalue problem as Williams (1959) or Bogy (1971). The larger the value of p is, the more singular the stress field is. And physically the stress concentration around the corner is due to the elastic mismatch and geometry discontinuity in this domain. So if there is no via-fill or crack stop, the local geometry is looks like bimaterial wedge. There is an open space, equivalently a material with modulus zero. If we put via-fill there, then the local geometry becomes a triple junction with three materials. The singular stress field can be solved in the similar way and also expressed as stress ~ r^(-p), but here p becomes usually much smaller. From pointview of mechanics, the singularity exponent p can be solved quantitatively for both cases. The results obviously show that triple junction is of smaller singularity than bimaterial wedge. Qualitatively, this can be understood as follows. In triple junction structure, the elastic mismatch is smaller than that in bimaterial wedge, and also the geometric discontinuity is closed. This is why the via-fill or crack-stop can effectively enhance reliability.

Delamination in Patterned Films

Xiao Hu Liu — Tue, 14 Nov 2006 11:57:09 -0500

When the dielectric constant of an insulator in an interconnect is reduced, mechanical properties are often compromised, giving rise to significant challenges in interconnect integration and reliability. Due to low adhesion of the dielectric an interfacial crack may occur during fabrication and testing. To understand the effect of interconnect structure, an interfacial fracture mechanics model has been analyzed for patterned films undergoing a typical thermal excursion during the integration process. It is found that the underlayer pattern generates a driving force for delamination and changes the mode mixity of the delamination. The implications of our findings to interconnect processes and reliability testing have been discussed.

Delamination in Patterned Films
Liu, X.H.; Lane, M.W.; Shaw, T.M.; Simonyi, E.
To appear in International Journal of Solids and Structures. 2007