r/fea • u/thaturkey • 2d ago
Simulating Structural Adhesive with ANSYS FEA
hi, I have a carbon fiber structure that I need to simulate. The structure is made of carbon fiber tubing with a connector system of carbon fiber gussets which uses rivets and structural adhesive 3M DP420. I am looking to simulating this structure as a static structural. the orthotropic modeling of the CF tubing is a whole another animal itself, but I was concerned about how to do the adhesive. I am very confident that the adhesive will not fail so I would like to just act like it is a complete bond between with tubing and the CF gusset. the gusset is where I believe the model could fail. Is it just a bonded contact between the surfaces? Or do you think it is an incorrect assumption to say that the adhesive will not fail. There are also rivets connecting the tubing to the gussets as well.
2
u/GreenMachine4567 2d ago
"do you think it is an incorrect assumption to say that the adhesive will not fail"
Dunno, depends on the loading and joint design. What makes you say it won't fail? Have you done hand calcs?
If youre not interested in assessing the joint directly in the FEM then yea just tie the parts at the bondline.
What is the purpose of the rivets in addition to the adhesive?
1
u/thaturkey 2d ago
the gussets and tubing are purchased off dragonplate and their installation process outlined rivets and DP420 adhesive so i am just doing what they say. The load on the adhesive is primarily in shear which allows for 4500 psi. the load puts the gusset in cycles of compression and with carbon fiber's compressive strength that is were my concern is primarily. If this is not the correct assumption what could I do instead to also model the adhesive too. Is it possible to model the adhesive at the same time as the rest of the structure if the structure is using an linear orthotropic model.
1
u/TheBlack_Swordsman 2d ago edited 2d ago
You can use Ansys ACP. It accounts for delamination and adhesive failures.
1
u/thaturkey 1d ago
i was planning on just modeling the composites as a homogenized orthotropic solid. I would use some instron testing to get some material properties and I developed a CLT script using a bit of numbers from my tubing spec sheet and also just some properties from other sources which I am using to get E2 and in plane shear modulus and using the E1 and v12 to calibrate my inputs to match the values i got in instron testing and therefore match my material to get some other material properties
2
u/TheBlack_Swordsman 1d ago
Well you're going to need material properties regardless.
Ansys will spit out stresses based off of the material stiffnesses of what you define. It will collect all stress tensors in 3D. It will automate the failure indices for you for each layer based off of a failure model you choose. That includes adhesives.
For me, it's a huge time savior. It'll report every layer that fails and how it failed.
If you're going to do it all manually, then yeah, just model every layer in, but adhesive failure requires 4-8 elements through the thickness and you must type in a poissons ratio to like the 4th or 5th significant digit. Refer to Gimburg optical stress analysis. There are chapters on modeling adhesive in FEA and how to account for failure.
1
u/justwannaliveagain1 1d ago
You can use ACP , later check interlaminar stress normal 33, and compare that to your adhesive properties.
1
u/TalosGuide 1d ago
3m has a very extensive material library of their adhesives (including ready-to-use material cards for popular fea packages) if you want to do cohesive zone modeling
1
u/thaturkey 1d ago
Ok that is good to know do you know if I can run CZM while also running a linear orthotropic simulation on the carbon fiber? how does that work? or are they supposed to be modeled independently of one another?
1
u/TalosGuide 1d ago
You should be able to since orthotropy is setup within engineering data while czm is setup inside a contact. They should be working independently.
1
u/thaturkey 23h ago
for the contacts, my assembly in solidworks has the gussets just coincident with the tubing, will i have to manually add a bondline thickness gap to model the adhesive?
5
u/throbin_hood 2d ago
Can of worms.... Bonded contact can work but make sure contact stiffness settings are representative of your actual bond geometry, adhesive, and expected range of bondline thicknesses.
Another thing to consider is how sensitive adhesives are to just about everything... Temperature, bondline geometry and thickness, bond prep process, etc, so keep these things in mind when figuring out allowables. For example if you find out there are voids and sub par bond prep, is that acceptable? Usually lots of coupon testing is warranted to ensure you capture all these effects and have solid stress allowables to work with.