simulating bonding

lil_luca_p_18

(hypermesh 2025.1)

I would like to simulate some Ergall ribs bonded to a carbon fiber shell. What is the best way to simulate this bonding?

Until now, I have used freeze contacts, but with this method the bonding becomes infinitely stiff. Since I am using ductile adhesives that can bridge gaps of up to 3 mm (in my case only 0.5 mm), I would like to model the adhesive with its actual thickness. What would you recommend?

I was thinking about creating 3D elements with the same thickness as the adhesive layer and using contacts between the adhesive-Ergall and adhesive-carbon interfaces. Then I would assign the adhesive material properties to these elements.

What I would like to analyse is how much the adhesive deforms and how much it contributes to the total wing displacement, as well as the actual stresses in the adhesive.

This is particularly important because, in reality, I have had several problems with adhesive joints that were predicted to be safe by FEM but failed in real life.

Thank you everyone!

Jason_Craanen

This is a classic challenge in structural FEA. Moving away from "Freeze" or "Tied" contacts is the right move when the compliance of the adhesive significantly affects the global response or when you need to predict failure accurately.

For a 0.5 mm bond line using a ductile adhesive, your intuition to model the adhesive as a physical volume is solid, but there are a few industry-standard refinements that will help you avoid the "safe in FEM, failed in reality" trap.

1. The "Physical" Approach: 3D Solid Elements

Modeling the adhesive with 3D elements (Hexahedral/Bricks are preferred) is excellent for capturing the contribution to total displacement and actual stresses.

• Mesh Density: For a 0.5 mm thickness, you should aim for at least 2 elements through the thickness. A single element through the thickness cannot capture the "peel" (normal) stress gradient or the bending of the adhesive layer itself.
• Aspect Ratio: This is the biggest risk. If your adhesive elements are 0.25 mm thick but 10 mm wide, the high aspect ratio will make the results unreliable. Try to keep the aspect ratio below 1:10 if possible.
• Interface: Instead of standard "Contacts" (which can be numerically noisy), use Tied Contacts or Shared Nodes between the adhesive solids and the Ergal/Carbon parts. This ensures perfect displacement compatibility.

2. The "Gold Standard": Cohesive Zone Modeling (CZM)

If your main concern is why the joints fail in real life despite "safe" FEM results, you should look into Cohesive Elements. These are special elements designed specifically for interfaces.

• Traction-Separation Law: Instead of just a Young's Modulus, you define a relationship between stress and "opening" (separation).
• Energy-Based Failure: CZM accounts for the Fracture Energy (Gc​). Real-world adhesive failures are often driven by crack propagation (peel) rather than simple stress exceeding a limit.
• Thickness: Most solvers allow you to define cohesive elements with "physical thickness" (0.5 mm) so they contribute to the wing's displacement correctly.

3. Why FEM often "Lies" about Adhesive Safety

The reason your previous models predicted safety while the parts failed is likely due to Peel Stresses and Singularities.

1. The Edge Effect: In a "Freeze" contact, the stress at the very edge of the bond line is mathematically infinite (a singularity). If you just look at "Average Stress," you miss the fact that the bond starts unzipping from the edge.
2. Ductility: If the adhesive is ductile, it will redistribute stress. A linear elastic model will over-predict the peak stress but under-predict the total energy the joint can absorb.
3. Peel vs. Shear: Most adhesives are very strong in shear but weak in peel (tension normal to the bond). Solid elements will show you these peel stresses clearly, whereas "Freeze" contacts often mask them.