I have tried to simulate the Vickers hardness on a substrate with a coating on it. I am really struggling to get it to work as the deformation is far too big. I have added the pictures of my model. Is there anyone that can help me with this?

# Simulation of Vickers hardness test on a substrate with coating

- 208 Views
- Last Post 3 weeks ago

Here are four suggestions.

(1) It will be much better for you to suppress the Force and use a displacement to move the indenter into the material. You can Probe the reaction force for Displacement 2 over the distance it moves. You will want to turn Automatic Time Stepping On and specify a large number of substeps, like 100 for both the Initial and Minimum number of Steps. You can set the Maximum number of steps to 500.

(2) Since the indenter has 2 planes of symmetry, you could start with a 1/4 model initially.

(3) You will also get a lot further before element distortions cause the solver to stop if you make a nice hex mesh rather than the tet mesh you have. I can also help with mesh controls to do that.

(4) You must have plasticity in the material model for the sample, preferably Multilinear Plasticity.

(5) Turn on Large Deflection. Under Analysis Settings. This is essential when using a plasticity model that will see large strains.

If you want further help, select Mesh, and Clear Generated Data, then save the Project and use File, Archive... to create a .wbpz file. You can attach that file to your post above like you did the .jpg files

There is a kind of chicken-and-egg problem here. To simulate the Vickers test, you need to know the yield strength of the material sample, but the Vickers test is often used to estimate the yield strength of a material. I assume you have an independent measure of the yield strength. Do you also have the full stress-strain curve from a tensile test sample? If so you can create the Multilinear Plasticity material model by following this discussion.

I have attached the file into the original post.

(4) You must have plasticity in the material model for the sample, preferably Multilinear Plasticity.

**Question:**

What do you mean by this and how is this done? is it something to do with the properties of the material in engineering data?

There is a kind of chicken-and-egg problem here. To simulate the Vickers test, you need to know the yield strength of the material sample, but the Vickers test is often used to estimate the yield strength of a material. I assume you have an independent measure of the yield strength. Do you also have the full stress-strain curve from a tensile test sample? If so you can create the Multilinear Plasticity material model by following this discussion.

**Question:**

The problem is that the specimen is with a coating as well so I have the young's modulus of the coating, indenter and substrate? Would this be enough? I'm not too sure about this part. This actual aim of this simulation is to look at the stresses acting on the coating during indentation.

I have been stuck with this for a very long time and I really appreciate your reply, thank you.

Here is a reference you should read. Here is a paragraph from that reference.

The basis of static indentation tests is that an indenter is forced into the surface of the material being tested for a set duration. When the force is applied to the test piece through contact with the indenter, the test piece will yield. After the force is removed, some plastic recovery in the direction opposite to the initial flow is expected, but over a smaller volume. Because the plastic recovery is not complete, biaxial residual stresses remain in planes parallel to the free surface after the force is removed. The hardness value is calculated by the amount of permanent deformation or plastic flow of the material observed relative to the test force applied. The deformation is quantified by the area or the depth of the indentation. The numerical relationship is inversely proportional, such that as the indent size or depth increases, the hardness value decreases.

In order to have permanent deformation in the simulation, you have to have a plasticity material model. Without plasticity, you can only create deformations that are elastic. To limit the deformations to the elastic range, you can't have an infinitely sharp point on the indenter, since that creates an infinitely high stress (zero area). You could have a ball indenter.

To add plasticity to a model, you just drag a plasticity model from the toolbox onto your material, but you have to have the data to fill out the parameters.

Here is a small model with 1/4 symmetry.

I'm sorry for the confusion, I was just wanting to look at the stresses on the coating and I'm just interested in looking at the elastic-plastic model.

Another thing, I was wondering if I have defined the contacts between the substrate and coating and the indenter to coating correctly?

(the contact between the coating and substrate is bonded and the contact between the indenter and coating is frictionless).

The picture above shows a paper that has been published and a like to the paper is attached above. In this, the model created is elastic-plastic.

Would you be able to send me the geometry that you used to create the mesh shown above please so I can compare the results?

In ANSYS, when there is a bond between two materials such as a substrate and coating, they can each have their own material properties, and the two bodies which share a common surface can be meshed so that they are sharing common nodes on the shared surface. That means there is no need to use contact elements to connect the two bodies. You can post-process the stress for each body without averaging across the bodies.

I duplicated Coating and Structural Steel, appending EPP to the names. I added Bilinear Kinematic Plasticity to each EPP material and entered a yield strength of 250 MPa just for the purpose of a demo. You can type in another value. By typing 0 for the Tangent Modulus, that creates an Elastic, Perfectly-Plastic material. As soon as the material reaches its yield stress, the material flows plastically.

When I get a model that makes some progress, I will attach it for you to use.

That would be extremely helpful if you could send me the model. Also, when you when you said "By typing 0 for the Tangent Modulus, that creates an Elastic, Perfectly-Plastic material". Does this mean elastic plastic?

Elastic Plastic and EPP mean the same. When you replace the 0 with a slope, that is defining a strain hardening portion of the stress-strain curve and the material increases stress while building up plastic strain.

Here is the convergence plot for the attached model.

It gets nearly 10% of the way to the displacement of 0.8 mm before having problems with element distortion. That is typical of the workflow necessary when including large deformation plasticity.

Here is the stress in the coating.

Notice that the maximum stress is about 250 MPa. It's not going to get any higher than that because that is the yield strength for this elastic plastic material.

I need smaller elements to get the solution to go further, but that will take longer to solve.

Hi there, the mesh looks much better now, thank you very much.

I was wondering how you would be able to see the finial solution as a 3D model? As you have symmetry in the model, you should be able to see the full model in 3D, is that correct?

Also, I have had the simulation running on the computer for the past 2 hours, and unfortunately, it still hasn't managed to solve the results half way through. Would there be a way to reduce the time taken for the simulation to run?

I'm really sorry to bother you again, I was unable to access the geometry file that you sent and I was unable to change the thickness of the coating. The required thickness is 300 micro meters. The diameter is 20 mm. I tried to change the geometry and tried to measure it but I was unable to do so. Would please be able to help me?

I also noticed that the displacement is set to 0.8 mm but the maximum deformation only goes to 0.07 mm. What is the reason for this?

Thank You

**Displacement**

The archive you provided showed a 1 mm displacement. That is why I thought you wanted to to displace 1 mm, which would be very challenging. I'm glad it's only 0.07 mm. I will use that in any new models.

**Geometry Editing**

I used DesignModeler, which is a geometry editor that is provided by ANSYS for preparation of CAD geometry for analysis. If you right click on Geometry, you can open the DesignModeler editor, but then you would have to know how to operate it. Better to edit in SolidWorks. I have SolidWorks 2017 so I could have used that but I didn't. The current coating thickness is 1 mm or 1000 micrometers. I can change it to 0.3 mm for you. Forget about the diameter, you can model a sample much smaller since the deformation is so very local, you get the same answer at 5, 10 and 20 mm diameter samples, but the larger samples just waste computer time.

**Solve Time**

1) Use the fewest number of nodes and elements possible. That is one reason why we use symmetry.

2) Enough RAM so solver runs completely in RAM. A statement in the Solution Output says the memory required.

3) Use more cores. If you have HPC licenses, find a computer with more cores, it will solve faster than a 2 core computer.

**Expanding Symmetry**

In Workbench, Options, Appearance, scroll to the end and check Beta Options.

In Mechanical, Click on Symmetry and fill out the Details below. I have to review this myself.

**Meshing**

Given the much smaller indentation depth, I decided small square block for the 1/4 model.

This is extremely helpful, would you be able to attach the file once you have figured the symmetry part please?

I have attempted to make the geometry on solid works and import it to ANSYS, I would not need to add the contact between the substrate and coating, is that correct?

Thank You

See above for the archive.

Yes you will need contact after you import SW geometry unless you open the geometry in DesignModeler and make a multibody part.

Unfortunately, the last archive came with the geometry distorted as you can see here.

The indenter is off set from the coating and substrate. Would it be possible for you to send a new one please?

Thanks

If you look at it from a good angle, you can see that the corner is just touching the face of the indenter. You can double click on Geometry to open DesignModeler then File, Export, and select Parasolid as the type. Then you can open the Parasolid file in SolidWorks to check it there.

I deliberately extended the side faces of the indenter to potentially help the contact algorithm.

The solver gets into trouble around 27% of the way to the 0.07 mm displacement.

Here is the stress on the coating at 26% of the way to 0.07 mm.

Since the element is about to collapse, I don't think the solver will be able to continue past this point.

On the other hand, the element has exceeded 100% plastic strain.

I could turn off plasticity, but then there would be no indentation when the indenter was raised up.

Instead, I will increase the Tangent Modulus and rerun the simulation.

Now the model has made it 65% of the way to 0.07 mm and has shown the first sign of trouble.

The solver needed 13.5 GB of RAM to run this model and ran for 9.2 hours on 8 cores to get here.

I set a minimum of 100 substeps but it looks like I could cut that in half and the solver might get to this point in half the time since there are many increments that are below the Force Criterion line and few that are above.

The plastic strain is at 50% and elements not yet in contact are deforming elastically. These will spring back after the indenter is removed. This model must eventually consist of 2 steps, the first step is to move the indenter down 0.07 mm, the second step is to move it up 0.07 mm so that the indentation can be measured after the elastic strain springs back to a new indented equilibrium.

Look below at how low the stress is in the coating. I could cut the size of the sample down by half easily.

Instead of 2 mm on a side for this 1/4 model, I can use a 1 mm on a side model and use fewer elements.

I made the above changes and also turned up the Tangent Modulus to 1E5 MPa to help the solver get to 100% of the load. That file is attached and is currently running on 8 cores. With less elements, the solver only needs 2.1 GB of RAM to run in memory.

Okay, the attachment above didn't make it all the way. The first element can't compress the second element. I changed the Sweep on the coating and removed the bias to make the element taller. That model failed in a different way. An hourglass mode appears in the elements down the center of the symmetry axis. There are some element Keyop settings that may help.

I turned on Reduced Integration instead of Full Integration on the Elements and set Keyop(2)=1 and Keyop(6)=1 and this got rid of the hourglass mode in the elements, but the solver still stopped before getting to 100% of the load. This model only made it to 51%.

At last, 100% of the 0.07 mm displacement was applied.

There was some residual stress when the indenter was retracted, but not much of an indent.

This model had a very high Tangent Modulus of 1E5 MPa. I will run another simulation with a lower value.

I have had a talk with my supervisor and changed the specs, he wants me only to locate the maximum and minimum principal stresses and total deformation without considering the plasticity or any other property. He was involved in the article that I sent earlier and I briefly had a chat to the person who done the simulation and he also said that the plasticity was not considered. I am trying somewhat to reproduce that particular simulation but instead of doing a 1/4 model, I am doing a 3D model. This is why I was worried that the indenter already being partially in at the geometry, so when the symmetry is applied, it would not be a perfect symmetry?

Also, I realised that the maximum displacement set to the indenter was 0.15 mm. I realise that even 0.07 mm was very hard to get it to work, but would it be easier not considering the plasticity as you mentioned earlier?

He also said that with the 0.15 mm indentation, there should be a force of around 500N, I don't think I am getting that though. I am very worried that I might not be doing what is required.

Also, The archive files that has been sent, I was unable to run the solutions on my system as it took a very long time and also came up with an error later.

Again, I'm very sorry to have to bother you again.

"I could turn off plasticity, but then there would be no indentation when the indenter was raised up.

Instead, I will increase the Tangent Modulus and rerun the simulation."

What is meant here, sorry?

Let me explain what I've been doing for the last 3 days before you changed the specs...

You provided the Young's Modulus of 1.3E5 MPa and a Poisson's Ratio of 0.23 for the coating. If you simulate pushing an indenter into a linear elastic material, you can create deformation, which is elastic strain, which is related to stress. When you remove the indenter, the material returns exactly back to where it started. You can plot any stress component you want at the point of maximum indentation in a simulation, maximum principal, mininum principal, etc.

When physical samples are tested with an indenter, the size of the indentation after the indenter is removed is measured. In order to simulate the observation of the size of the indentation after the intender is removed, you can't use a linear elastic material. You use a material model that includes plasticity, which describes the behavior of materials past their yield point. ANSYS has plasticity material models. The simplest model has two inputs, the yield strength and the Tangent Modulus. This is what I used. That way, when you remove the indenter, there is an indentation in the material.

The coating material was assigned a material model called Bilinear Kinematic Plasticity with a yield strength of 250 MPa. If the Tangent Modulus is zero, that is an elastic, perfectly-plastic or just elastic, plastic material model. This is the Stress Strain curve for this material.

A Tangent Modulus of 5,000 MPa is shown below.

Here is the tangent modulus for 50,000 MPa.

Tangent Modulus of 1.0E5 MPa.

Any material that exceeds 250 MPa will undergo plastic deformation, so that when the load is removed, the material will not return exactly to where it started, it will be permanently deformed.

The indender as pushed down 0.07 mm per your earlier specifications. Using the material with the Tangent Modulus of 5,000 MPa, the deformation of the 1/4 model at the maximum displacement is plotted below.

After the indenter is removed, there is some permanent deformation.

Below is the Max. Principal Stress of 8.4 GPa at maximum load.

Note that the stress will be much higher for a linear elastic material with no plasticity.

I used a Tangent Modulus of 1E5 MPa, which is so high, it's almost linear elastic.

Below is the Max. Principal Stress of 52.1 GPa from that simulation.

On the topic of symmetry, the material has symmetry planes so can only see the indenter in its quadrant, so the coating deformation is symmetric. It does not matter that the indenter goes beyond the symmetry plane as there is no material there. Below is the expansion of symmetry to a full model.

On the topic of simulation time, these models take about 90 minutes to solve on 8 cores, but that is to go down and up. It will take maybe 60 minutes to go down 0.07 mm if the indenter doesn't have to go up. Turning off plasticity may reduce the time a little, but traveling twice the distance will certainly increase the simulation time.

When you do a 1/4 model, you have to multiply the reaction force by 4 to get the force for the full model. Below is a plot of the reaction force on the 1/4 model for plasticity with a 5,000 MPa Tangent Modulus. It's 5.84 N for the 1/4 model or 23.3 N for a full model to indent 0.07 mm. The reaction force is much higher for a linear elastic material at 282 N for a full model at 0.07 mm, and will be much higher at 0.15 mm indent. Unfortunately, the model that was carefully tuned to reach 0.07 mm of indentation cannot reach much past 0.08 mm before stopping.

I will post this now and take a break from indentation for a while.

"On the topic of simulation time, these models take about 90 minutes to solve on 8 cores, but that is to go down and up. It will take maybe 60 minutes to go down 0.07 mm if the indenter doesn't have to go up. Turning off plasticity may reduce the time a little, but traveling twice the distance will certainly increase the simulation time."

I am unfortunately only able to access a i5 PC currently, would it be possible to solve these simulations using these PC's? Could this could be the reason why some of the simulations are not working You also mentioned that it will reduce the time if the indenter does not have to go up, how do I stop it from going up?

"The reaction force is much higher for a linear elastic material at 282 N for a full model at 0.07 mm, and will be much higher at 0.15 mm indent."

I was wondering if this model considered the Tangent Modulus of 1E5 MPa when you said 282 N for linearly elastic? Also when you mentioned turning off plasticity in the model, do you mean turning off Bilinear Kinematic Plasticity and not adding a yield strength?

Would you be able to attach the final file foe the indentation with the tangent modulus of 1E5 MPa that goes all the way to 0.07 mm please?

Also, I would like to thank you very much for your help so far, at the start of this I had very limited knowledge about this topic.

How many cores are on your i5? Some of them are quad core such as i5-6300HQ. Look up your Model number here. If you have 4 cores instead of 2, then you must follow this setup to use them. If your processor can solve a model at all, it will solve this model, it will just take longer than it takes me on my 8 core computer.

To make an indenter go up after it went down, you just make the number of steps in the Analysis settings to be 2 steps instead of 1 step, then you get a second row in the table of displacements and you type 0 in the second row. For the attached model, the first step is 0.07 mm and the second step is 0.15 mm, which is the total, not an incremental amount. Maybe by doubling the size of the elements, you can get this to reach 0.15 mm. Good luck!

The 282 N reaction force was for linearly elastic. For a Plasticity material with a yield strength of 250 MPa and a Tangent Modulus of 20000 MPa, the reaction force was 70 N for a full model. That material is called Coating WH in the model. The material called Coating is linear elastic and has no yield point.

##### Search

##### Categories

##### This Weeks High Earners

- peteroznewman 53
- Raef.Kobeissi 10
- vganore 10
- Billy 5
- minko 4
- Hassaan 3
- Sachin 3
- cylindrax 3
- emirdegirmenli 3
- Paca 2