my suggestion is as below (which can be wrong but might be helpful)

Analysis of Your Simulation Images

Primary Cause: Incorrect Normal Contact Behavior

The most probable reason for this “sticking” behavior is the Normal Behavior setting within your contact interaction property. Abaqus allows you to define contact properties that prevent surfaces from separating once they have come into contact.

In the Interaction module, you define a Contact Property. Within that property, under the Mechanical -> Normal Behavior tab, there is an option for “Allow separation after contact”. If this checkbox is unchecked (or if the “Constraint enforcement method” is set to “No Separation”), Abaqus will essentially glue the surfaces together once they touch. This is the most common cause of the behavior you are seeing.

How to Fix It:

Here is what the dialog box should look like:

Secondary Cause: Severe Plastic Deformation and Mesh Entanglement

From your results (DuringSimulation.JPG), the stresses are over 4 GPa. This suggests that the fiber material has undergone massive plastic deformation.

When the mesh deforms so severely, nodes of the deformable fiber can get “trapped” or “snagged” on the facets of the rigid indenter. The contact algorithm can struggle to resolve this, leading to large, artificial adhesion forces that prevent separation. Essentially, the geometry becomes mechanically interlocked at the mesh level.

How to Investigate and Mitigate:

Tertiary Cause: The Role of the Cohesive Interface

You mentioned a cohesive surface between the fiber and matrix. The image DuringSimulation.JPG clearly shows the fiber separating from the matrix. This means your cohesive interface is working, at least partially. However, its behavior could be a contributing factor.

• Is the failure realistic? The fiber is being pulled out. This implies that the artificial “adhesion force” between the indenter and fiber is greater than the fracture energy of your fiber-matrix interface.
• Check Cohesive Properties: Ensure your Traction-Separation Law (TSL) parameters (e.g., Knn, Kss, Ktt, damage initiation stress, and damage evolution energy) are physically realistic. If the interface is too weak, it will fail easily as seen. The primary problem is still the indenter-fiber sticking, but a well-behaved interface is crucial for overall model accuracy. You can plot damage variables for the cohesive surface (e.g., CSDMG or SDEG) to verify that it is degrading as expected.

Summary and Recommended Workflow

Here is a step-by-step plan to debug your simulation:

Hi Amin Shamsabadipour ,

Thank you so much for the detailed answer.

I tried implementing the changes you suggested:

Now my system is showing negative eigenvalues. I’m not reaching the stage in the analysis where I can see whether the indenter is getting stuck to the fiber.

I’m confused about where exactly things are going wrong.

I've attached the MSG file for reference.

my suggestion is as below (which can be wrong but might be helpful)

### Analysis of the New Information

1. **`Jobmonitor.JPG` and `Trial6Job.msg.txt` - The Smoking Guns:**

* **"There are 2 unconnected regions in the model."**: This is the most critical warning. It means that during the initial check of your model (`datacheck`), Abaqus found two distinct groups of elements that are not connected to each other by elements, constraints, or contact definitions *at the start of the step*. One region is your main fiber/matrix block, which is fixed by boundary conditions. The other region is almost certainly your **rigid indenter**.

* **"The system matrix has [1, 4] negative eigenvalues."**: This is the direct consequence of the unconnected regions. A negative eigenvalue means the model has lost stiffness in some way, allowing it to deform or move without resistance. This is called a **numerical instability**. When a part of the model is "floating" (unconnected), it can undergo rigid body motion (move or rotate freely), which mathematically results in a zero-stiffness term in the global matrix, leading to negative eigenvalues.

* **Aborted Job and Cutbacks**: The Job Monitor shows the time increment (`Time/LPF Inc`) getting progressively smaller until it becomes tiny (`6.67e-05`) and the job aborts. This is the solver struggling desperately to find a stable solution, failing because of the instability, and cutting the time step back repeatedly until it gives up.

2. **Your Actions and Observations:**

* **Displacement Control**: Switching to displacement control was the right move for improving stability.

* **Mesh Refinement (`ModifiedTipcontactmesh.JPG`)**: Your new mesh looks excellent. The circular partitioning and biased seeding are good practice. This is not the source of the problem.

* **Cannot find PEEQ**: This is expected. `PEEQ` (Equivalent Plastic Strain) is a result variable that you must *request* before you run the simulation. It's not available by default.

* **Unconnected Region Diagnostic**: The command-line tool can be tricky. There's a much easier way to view these regions directly in the Abaqus/CAE viewer, which I will explain.

### Root Cause: Unconstrained Rigid Body Motion of the Indenter

The combination of the "unconnected regions" and "negative eigenvalues" warnings points to one primary cause:

**Your indenter's reference point (RP-2) is not fully constrained against rigid body motion before it establishes firm contact with the fiber.**

You have correctly applied a displacement in the Y-direction (`U2`). However, the indenter is still free to move in the X and Z directions (`U1`, `U3`) and free to rotate about all three axes (`UR1`, `UR2`, `UR3`). Even a tiny numerical imprecision can cause the indenter to drift or spin slightly, leading to the solver detecting rigid body motion and terminating with a negative eigenvalue error.

---

### Step-by-Step Solution

Follow these steps to resolve the issue.

#### Step 1: Fully Constrain the Indenter's Reference Point (Highest Priority)

This will eliminate the rigid body motion and should allow your analysis to run.

1. Go to the **Load** module in Abaqus/CAE.

2. Find the Boundary Condition (BC) you created for the indenter's reference point (RP-2). You likely have one that specifies `U2`.

3. **Edit this Boundary Condition.** In the BC editor, you need to constrain **all other degrees of freedom (DOFs)** to zero. The setup should be:

* `U1 = 0`

* `U2 = [Your prescribed displacement, e.g., -0.003]` (Keep this as is, linked to your amplitude)

* `U3 = 0`

* `UR1 = 0`

* `UR2 = 0`

* `UR3 = 0`

By setting the other five DOFs to zero, you are preventing any lateral movement or rotation of the indenter, completely eliminating the possibility of rigid body motion. This is standard practice for indentation simulations.

#### Step 2: Visualize the Unconnected Regions (For Confirmation)

Even though you'll fix the problem in Step 1, it's very useful to know how to visualize these warnings for future debugging.

1. After a job fails with this warning, open the `.odb` file in the **Visualization** module.

2. From the main menu, go to **Tools -> Display Group -> Create**.

3. In the "Create Display Group" dialog, under "Item", select **Internal Sets** from the dropdown list.

4. You will now see Abaqus-generated sets in the list, named something like `_UNCONNECTED_REGION-1` and `_UNCONNECTED_REGION-2`.

5. Select one of them (e.g., `_UNCONNECTED_REGION-2`) and click **Replace**.

6. The viewport will now show you only the elements belonging to that unconnected region. You will almost certainly see your indenter, confirming it was the "floating" part.

#### Step 3: How to Request PEEQ Output

To see the plastic strain in your next successful run, you need to request it as a field output.

1. Go to the **Step** module.

2. In the Model Tree, find **Field Output Requests**. Double-click the request associated with your analysis step.

3. In the "Edit Field Output Request" dialog, click the arrow next to **Plasticity**.

4. Check the box for **`PEEQ`** (Equivalent plastic strain). You might also want `PEMAG` (Plastic strain magnitude).

5. Click **OK**. Now, when you re-run the job, these variables will be written to the `.odb` file and will be available for plotting in the Visualization module.

#### Step 4: (If Needed) Use Automatic Stabilization

If you fix the rigid body motion and still encounter convergence difficulties (especially during the initial contact or when material damage occurs), you can use automatic stabilization. This adds a tiny, artificial viscous damping to the model to help it overcome moments of instability.

1. In the **Step** module, edit your analysis step.

2. Go to the **Other** tab.

3. Under **Stabilization**, select the option **"Use automatic stabilization with a dissipated energy fraction of:"**. A default value of `0.00005` (or `5e-5`) is a good starting point. You can also specify an adaptive factor.

This should be used as a last resort, as it adds non-physical energy to the system, but it is extremely effective for highly nonlinear problems.

### Summary and Path Forward

1. **Your immediate problem is unconstrained rigid body motion.**

2. **Fix it by editing the indenter's BC to constrain U1, U3, UR1, UR2, and UR3 to zero.**

3. Re-run the analysis. It is very likely to proceed much further, if not to completion.

4. Before you re-run, follow Step 3 to request `PEEQ` so you can analyze the material deformation properly.

5. Once the analysis completes, you can check if the original "sticking" issue is resolved. With displacement control and a fully constrained indenter, the behavior should be physically correct.

Thank you so much, Amin Shamsabadipour, for taking the time to explain everything in detail.

I was able to resolve the unconnected regions problem by enabling the “Adjust only to remove small overclosures” option in the interaction module.

I have already constrained all the DOFs except in the Y direction.

My model now runs, but I still encounter the issue of the indenter sticking to the fiber.

In the job diagnostics, when I expand all the steps and increments after running the analysis, I see that for each iteration within an attempt it shows Severe Discontinuous Iteration (SDI). In the related summary, it says Converged: NO. And also I see terms like Max Contact Force Error,

Max Penetration Error, Overclosure, Openings.

So, while the model runs without errors, all 26 increments report SDI and fail to converge.

I also tried adding stabilization, as you suggested, but the problem still persists.

By any chance, could the material properties of the fiber and matrix affect the performance? So far, I have only assigned Young’s modulus and Poisson’s ratio for both the fiber and matrix.

PFA my job diagnostics screen.

my suggestion is as below (which can be wrong but might be helpful)

=======================================================

The core issue you’re facing is a classic, and often challenging, problem in contact mechanics simulations, especially those involving friction and material deformation. The fact that your job “completes successfully” but all increments are “Severe Discontinuity Iterations” (SDI) and show Converged: No at the iteration level is a significant clue. It means Abaqus is not finding a true equilibrium solution at each step but is using its automatic stabilization or other cutback mechanisms to “push through” the analysis to the end. The “sticking” behavior is a direct physical manifestation of these underlying numerical difficulties.

Based on the provided PDF and your description, here is a detailed analysis and a set of recommendations.

Analysis of Your Job Diagnostics

Let’s look at the clues from the provided JobDiagnostics.pdf:

So, Why is it Sticking and Failing to Converge?

The issue is almost certainly a combination of your Contact Definition and Material Properties.

You asked: “By any chance, could the material properties of the fiber and matrix affect the performance?”

Absolutely. YES. This is very likely a primary contributor to your problem.

When you only define Young’s Modulus and Poisson’s ratio, you are defining a purely linear elastic material. This material has no mechanism for energy dissipation (like plasticity or viscoelasticity). In a contact simulation with friction, this is a recipe for instability.

Here’s the physical analogy: Imagine trying to slide two perfectly smooth, perfectly hard blocks of glass against each other. They will chatter, screech, and jump. There’s no “give” in the material. Numerically, this leads to:

• High Contact Stiffness: The surfaces are very resistant to penetration.
• Abrupt Stiffness Changes: A node is either “open” (zero stiffness) or “closed” (very high stiffness). This sudden change is a severe discontinuity.
• Frictional Instability: When a node is trying to slip, the friction model calculates a shear force. If the underlying material has no way to deform plastically, the energy has nowhere to go, leading to oscillations and non-convergence. The solver tries to resolve this by applying forces that manifest as “sticking.”

Recommendations for Fixing the Model

Here is a prioritized list of things to try, from most likely to least likely to be the root cause.

1. Add Nonlinear Material Properties (Most Important)

You must give the materials a way to dissipate energy. Even a small amount of plasticity can dramatically stabilize a contact simulation.

• Action: In the Property module, edit your material definitions for both the fiber and the matrix. Add plastic behavior.
• How to do it:Go to Material -> Edit. Under the Mechanical menu, select Plasticity -> Plastic. You need to provide at least one data point: Yield Stress vs. Plastic Strain. A simple starting point is perfectly plastic behavior. Enter a realistic Yield Stress for your material (e.g., for steel, maybe 250 MPa). For the Plastic Strain, enter 0. This tells Abaqus that once the material reaches the yield stress, it can deform without any increase in stress.

// Example Material Data:

// Elasticity:

Young’s Modulus = 200e9 (Pa)

Poisson’s Ratio = 0.3

// Plasticity (Perfectly Plastic): Yield Stress | Plastic Strain

250e6 (Pa) | 0.0

Even if your materials are brittle in reality, adding a small amount of plasticity gives the numerical solver a vital tool to handle the high localized stresses that occur at contact points.

2. Refine Contact Properties and Solver Controls

Your use of “Adjust only to remove small overclosures” was a good first step. Now, let’s refine the contact behavior itself.

• Friction: Is the friction coefficient you are using realistic? A very high friction coefficient can cause sticking and convergence issues. If you can, try reducing it to see if the simulation becomes more stable. If it does, your problem is highly sensitive to friction.
• Contact Stabilization: You mentioned you tried adding stabilization. This is the correct instinct. However, it needs to be done carefully.Go to Step Module -> Create Step. In the step editor, go to the Other tab and find Automatic Stabilization. Instead of using the automatic Factor, choose Specify and enter a very small Damping factor. Start with something like 1e-7 or 1e-8. The goal is to use the minimum amount of stabilization needed to get past the instability, not to power through the whole analysis. You can check the energy dissipated by stabilization (ALLSD) in your results to see if it’s a small fraction of the total internal energy (ALLIE). If ALLSD is large, your results are not reliable.
• Contact Controls: For very difficult contact, you can modify the solver’s contact controls.In the Interaction module, find Contact Controls in the menu. Create a new control. You can try enabling Automatic Tolerances and specifying a Max penetration tolerance. Under Stabilization, you can specify Contact stabilization with a small tangential or normal damping. This is another way to apply stabilization just for contact.

3. Mesh Refinement

The quality of your mesh at the contact interface is critical.

• Ensure the mesh is fine enough to capture the curvature of the fiber and the indenter accurately.
• Avoid highly distorted elements at the contact surfaces.
• Use continuum elements with reduced integration (like C3D8R) as they often behave better in contact, but be mindful of hourglassing (though Abaqus has built-in controls for this).

4. Step and Increment Size

Since the solver is struggling, you can give it more help by controlling the increment size.

• In the Step module, go to the Incrementation tab.
• Set a smaller Initial increment size (e.g., 1e-3 or 1e-4).
• Set a smaller Maximum increment size. This will force Abaqus to take smaller steps, which can help it navigate the severe discontinuities more carefully.
• Increase the number of allowed increments.

Summary of Actions

Start with the material properties. I am confident that introducing some non-linearity will have a significant positive impact on your model’s convergence and will likely resolve the “sticking” behavior by allowing the material to yield locally instead of creating numerical instabilities.