Cohesive Zone Modeling of FRP Pull-Out Test in Grooved Concrete – Best Approach for Adhesive Layer in Abaqus?"

[Roshaan]

I’m currently working on simulating a pull-out test using Abaqus, and I’m facing some confusion regarding how best to model the adhesive interface using Cohesive Zone Modeling (CZM). I would greatly appreciate any guidance or suggestions from the community.

Experimental Setup:​

• A concrete block (200 mm × 200 mm × 400 mm) with a groove cut in the middle.
• Groove dimensions: 7.1 mm width, 20 mm depth.
• A FRP laminate (3.6 mm width × 16 mm depth) is embedded in the groove.
• The epoxy adhesive was poured into the groove to bond the FRP and concrete.

Modeling Approach:​

• I am trying to model the epoxy adhesive using cohesive elements (element-based CZM).
• I’ve defined traction-separation behavior with damage initiation and damage evolution criteria for the cohesive layer.
• Due to the groove geometry, I'm unsure whether I should model the adhesive layer as a U-shaped cohesive element around the FRP, or use a rectangular cross-section of cohesive elements and embed the FRP into that.

Specific Questions:​

1. Geometry:
   Should the cohesive layer follow a U-shape conforming to the FRP-concrete interface, or can I simplify it as a rectangular adhesive block and embed the FRP inside it?
2. Interactions:
   If I use cohesive elements, should I tie them to the concrete and FRP? I’m concerned that doing so might create a perfect bond, which contradicts the purpose of using CZM.
   I’ve also run models with just nodal connectivity (i.e., shared nodes) between FRP, epoxy, and concrete, but results did not match experimental data well.
3. Results So Far:
   • Using tie constraints gave better correlation with experimental data, but I’m still doubtful whether this modeling approach is physically correct.
   • I want to accurately capture the bond-slip behavior and debonding that occurs in the test.

Summary:​

I’m looking for the best practice to model an adhesive layer with finite thickness between a grooved concrete block and embedded FRP, in a way that realistically represents the pull-out mechanism.


Any help, example models, or experience with similar simulations would be extremely helpful.


Thanks in advance!

 

[FEA way]

I would try cohesive contact first (it’s much easier to define than cohesive elements) but you can’t account for the thickness of the adhesive this way.

Both approaches to attach cohesive elements (tie constraints and shared nodes) are correct and should give equivalent results. One advantage of tie constraints is that you don't need matching meshes. You could also apply contact on one side of cohesive elements.

 

[Roshaan]

That is what I’m confused about — how exactly should I define the cohesive contact? Should I model the rest of the adhesive layer using a conventional material model? If not, then how can I define the cohesive contact properly?


I have already tried using matching nodes with the same mesh size for all components, including the FRP, adhesive, and concrete. However, the FRP doesn’t seem to stick when I apply a displacement-type loading. It simply moves out without generating any reaction force. Similarly, when I apply a load on the far end of the FRP, it just starts moving into space — there doesn’t appear to be any kind of resistance at all, even with matching nodes.


I also tried defining contact interactions — using cohesive elements for the adhesive and assigning interaction properties (tangential and normal behavior) between the FRP–adhesive and concrete–adhesive interfaces. Still, I’m only able to get somewhat better results when using tie constraints, although they still don’t match the experimental results.


Additionally, could you please clarify if I’m defining the stiffness of the epoxy correctly? For E/Enn, I assign the full value of the elastic modulus, and for defining the section, I use nodal coordinates. Is that the correct approach? Could it be affecting the results?

 

[Roshaan]

@FEA way Can you please help I am really stuck

 

[FEA way]

Should I model the rest of the adhesive layer using a conventional material model? If not, then how can I define the cohesive contact properly?

Cohesive contact is meant to replace the adhesive so that you don't have to model it directly but you don't take its thickness into account. It's just a sticky contact property.

I have already tried using matching nodes with the same mesh size for all components, including the FRP, adhesive, and concrete. However, the FRP doesn’t seem to stick when I apply a displacement-type loading. It simply moves out without generating any reaction force. Similarly, when I apply a load on the far end of the FRP, it just starts moving into space — there doesn’t appear to be any kind of resistance at all, even with matching nodes.

Are you sure the nodes are shared and not only coincident ? You can achieve that with the Edit Mesh tool.

I also tried defining contact interactions — using cohesive elements for the adhesive and assigning interaction properties (tangential and normal behavior) between the FRP–adhesive and concrete–adhesive interfaces. Still, I’m only able to get somewhat better results when using tie constraints, although they still don’t match the experimental results.

Contact should be applied only to one side.

Check the documentation chapter Elements --> Special-Purpose Elements --> Cohesive Elements --> Modeling with Cohesive Elements (paragraph "Connecting Cohesive Elements to Other Components").

Additionally, could you please clarify if I’m defining the stiffness of the epoxy correctly? For E/Enn, I assign the full value of the elastic modulus, and for defining the section, I use nodal coordinates. Is that the correct approach? Could it be affecting the results?

This is explained in the chapter Defining the Constitutive Response of Cohesive Elements Using a Traction-Separation Description (paragraph "Interpretation of Material Properties").