Are there any example or test inputs that model the failure of a material under load?
I was trying to model a 1 mm cube of acrylic glue between two steel bars under tension. The stress in the cube of glue was 1 GPa which was significantly above the 1 MPa strength of the glue. Why didn’t it fail?
I was looking at the cube of glue as a start to looking at the fracture behaviour of the glue when tape with acrylic glue is peeled off from a surface.
I used FreeCAD to look through the test examples that came with Calculix ccx_2.23 when I compiled it. I didn’t find any fracture test examples.
Are there any fracture test examples that are supposed to have come with ccx_2.23?
The CalculiX solver doesn’t support direct failure analysis, to the best of my knowledge.
What you can do is make stresses (or strains) that are too large visible in cgx, e.g. like this:
# Define the view.
rot y
rot r 135
rot u 30
# Set up the presentation
cmap jet
view sh off
# Everything outside minc/maxc is colored magenta.
asgn minc m
asgn maxc m
# Material is aluminium 6060 T66.
# Youngs modulus 68 GPa, proportional limit 170 MPa.
# 0.2% permanent deformation gives a total strain of:
# 170e6/68e9 + 0.2/100 = 0.0045
minc -0.0045 el
maxc 0.0045 el
# Read result data
read job.frd
frame
read capt.txt
ulin Signed von Mises strain [-]
# Display signed von Mises strain
ds 2 e 26
view disp
After that has identified elements where the stress is too high, you could e.g. use the *CRACK PROPAGATION keyword, but I’ve never tried it.
Alternatively, you could use *MODEL CHANGE to remove “damaged” elements.
There are many different failure modes and they can depend on factors that are hard to capture in an FEA model.
Over the course of my career, I have done and comissioned quite a bit of bonding tests. Getting consistent test results is always a challenge.
And extrapolating those simple tests to predict real product failures is hardly possible, since any real joint will invariably have a much more complicated combined load than simple tests.
Since CalculiX 2.23, there’s also *DAMAGE INITIATION with two criteria available (Rice-Tracey and Johnson-Cook). But there’s no *DAMAGE EVOLUTION, unlike in Abaqus.
You may want to try other solvers, such as OpenRadioss, for this kind of application.
Having done quite a bit of work on lap joints recently, I have found that the stress concentrations at the end of the lap joint is very dependant on substrate thickness. Standard shear tests like ISO-4587 are more peel tests than real shear tests because the substrates are relatively thin and not stiff enough to prevent peeling.
Acrylic pressure sensitive adhesives (“PSA”) are viscoelastic, and I would hesitate to describe them as solids. See e.g. Rheological and Mechanical Properties of an Acrylic PSA. Picking a decent material model for FEA for a material like this sounds like a challenge.
I have just looked at OpenRadioss and they have a tensile specimen example. When the tensile specimen stretched, it reached its ultimate tensile strength and failed. When I tried to do that with CalculiX, the bar wouldn’t fail, even when I put notches in the bar.
OpenRadioss will take input from FreeCAD, either as an .inp file or with an available application. The post processor is also free, which makes these programs a complete set, in effect.
So, I will leave CalculiX and start to work with OpenRadioss.
The focus of my problem isn’t the fracture / failure of the acrylic adhesive. I know that the acrylic PSA is viscoelastic and I have seen a couple of papers and theses published.
My real focus is the stresses in the substrate when the adhesive tape is peeled from the substrate. The tape holds down delicate components for cutting, which are as thin as 30 microns. I have seen these thin substrates flex as the tape is being peeled away. This substrate flexure is not good.
I am more concerned on getting the yield strength and ultimate tensile strength reasonably close for initial analyses. As I get better at using the software, i will add better models.
Thank you for the paper. It is useful in giving my insights as to the adhesive behaviour.
I am going to use OpenRadioss since it will do dynamic FEA. One of their examples is a tensile bar specimen which is pulled to failure. I wasn’t able to do this with FreeCAD / Calculix package.
No solver can show failure (by that, I assume you specifically mean element deletion and thus fracture of the specimen) without a damage model or failure criterion. There must be a rule when an element is considered failed and removed from the mesh. Various approaches exist. Abaqus has progressive damage models (damage initiation followed by damage evolution), but also some simpler criteria.
For glued connections and delamination, there also special approaches available in some sofware, such as cohesive elements or cohesive contact. They also need some failure criteria (such as traction-separation laws). Abaqus has several methods to model that, but OpenRadioss (and possibly also Code Aster) should offer quite a few options too.
This is a really insightful discussion. I agree with the points raised by @rsmith, @Calc_em, and @xyont regarding the current limitations of failure modeling in CalculiX.
From my experience, what often surprises new users (as in the original question) is that exceeding a material strength does not automatically lead to failure in standard FEM formulations. As @rsmith pointed out, ccx will continue solving unless failure is explicitly introduced through additional modeling assumptions (e.g., element removal or crack propagation strategies).
The recent addition of *DAMAGE INITIATION mentioned by @Calc_em is definitely a step forward, but without a corresponding damage evolution law, it remains difficult to capture progressive degradation or material separation in a physically meaningful way.
I also agree with @xyont that extending CalculiX through MFront or cohesive zone approaches is currently one of the most promising paths for realistic failure modeling.
If helpful, I would like to point to a work that discusses progressive failure modeling frameworks and material degradation strategies using material subroutines (UMAT), which adapted for use with CalculiX:
These ideas may be particularly useful when implementing:
a UMAT-based approaches
MFront material laws
or element deletion strategies
CalculiX provides a solid FEM foundation, but realistic failure modeling still requires user-defined extensions or coupling with more advanced material models.
Many thanks for your advice and suggestions. I do not have the programming background or experience, let alone be able write up something for Calculix. I am surprised that I didn’t mortally wound myself trying to install and compile Calculix. I am just trying to survive by helping a colleague by myself with what I can find on the internet. I have no funds for any programming training / classes which I think will need to be eventually high level to do the UMAT approaches or MFront material laws.
I will continue to investigate and learn what I can.
Veering off-topic, but it doesn’t sound like PSA tape is a good solution for this application? If your substrates can withstand ≈70°C, you could try mounting wax or shellac als alternatives. If the substrates can withstand acetone, then cyanoacrylate adhesive could also work.
The best way to describe the situation is that the companies are processing 300mm disks with 50+ integrated circuits on them that are worth easily more than $10,000 each. These disks are going through the system at a brisk pace. The companies that do this would have already looked at the various mounting techniques such as CrystalBond, mounting wax, or shellac. The processing would involve bonding, processing, debonding, and cleaning, all to very high precision so that the processing doesn’t result in damage. I would assume that these mounting methods would have taken too much time to use and that the circuits would be too sensitive to any solvent and bonding materials or method. The PVC-acrylic adhesive tape is the cheapest, cleanest, and quickest method. Now, they are trying to increase the yield of circuits and decrease the number of broken ones.
That sounds like silicon wafers? Those are routinely cleaned with almost boiling acetone. Compared to the stuff (like 40% hydrofluoric acid) they use for actually etching silicon, acetone is almost like a spring breeze.
Yes, silicon wafers. Acetone is fun because it is hygroscopic and will readily suck moisture out of the air. They don’t use 40% HF. That is way too strong and aggressive. They want a controlled etching rate, so they use maybe 2% HF plus various flavours and wetting additives.
usually, i started with simplest one of material models with limiting capabilities before going through in advanced of plasticity and damage. There is Compression_Only material available, tension stress can be set to some limit values as example below.
That is a good picture you have. Looks very much how a lap joint will behave, either riveted or glued, under tension. I am still trying to figure out how to run OpenRadioss_gui. I am not a programmer. My last bit of programming was with punch cards. My background has been metallurgy and materials processing. Fun in the lab.
I have reread your message after drinking some tea. My brain is working now, I think.
I looked at adjusting the tension stress max and min values by changing the material property yield strength and ultimate tensile strength and maximum strain. I can see where the adhesive material starts to fail, where the stresses are maximum. Exactly where I expected failure to start.
But the model I am trying to make is basically peeling tape from a substrate. The adhesive material needs to fail in order for the tape to move. As the adhesive fails and the tape moves, I need to calculate the stresses in the substrate. That is the goal.
In FreeCAD 1.0 and 1.1, I use the Calculix solver but I have reached the limits to those programs. I tried setting up Calculix ccx_2.23 but it is complicated to use. I am moving on to use OpenRadioss which looks at non-linear materials failure which is what happens to the adhesive material.
personally, i will stick with CalculiX as one solver since learning another new is not easy task for me. MFront integration with CalculiX made material library is rich complete enough and it seems material models of adhesive with damage has been develops since 2022 (link) but i’m not sure is it has published or not, you may ask the author directly.
right, it is distributed as dynamic link library (DLL) in Windows available in this forums and just simple copy in the same directory of CalculiX solver to ready to use. I successfully test of large material models of plasticity and damage, it’s fast and stable to beat compete with another commercial solver to fulfill CalculiX material libraries internal solver limitation.
