I have made a model of the Vickers indentation test on ANSYS but however, I do not know how I would be able to estimate the residual stresses within the coating. The model is of a coating, substrate and an indenter. Is there anyone that can help?
How to calculate the residual stress on a coating by Vickers indentation?
- 571 Views
- Last Post 22 February 2018
Residual stress will be present in a simulation that includes a plasticity material model. I posted some models of the Vickers indentation test that included plasticity in your other thread.
Here is the Max Principal Stress in the coating when the Indenter is pushed down 0.07 mm.
Here is the Residual Stress after the Indenter is raised up off the surface.
This model has a two-step time history. At t=1, the displacement of the indenter is 0.07 mm.
At t=2, the displacement of the indenter is 0.00 mm, which is where it started.
If you only use linear elastic materials, there will be no residual stress.
Can you explain why this model does not show the right values?
The problem with the last model shown was that the indenter is too sharp, there should be an angle of 136 degrees for the indenter. I am also considering the coating as elastic-plastic, does this mean set the tangent modulus to 0 in bilinear kinematic hardening?
Would it be possible to calculate the residual stress on this model? Also, why is it that it does not go past 0.07 mm, could you explain?
Also, how would you produce a load depth curve for loading and unloading of indentation?
When you use a displacement BC to move the indenter down 0.129 mm in step 1, you must use a value of 0 for step 2 to get the indenter to return to the start position. Then you can add a Force Reaction result that will plot the force. In this plot, it shows time, but t=1 is depth=0.129 mm so depth = 0.129*t for t <1, then depth = 0.129-0.129*(t-1) for 1<t<2 for the raising portion.
Below is the data from my model from the other thread.
Residual stress is just the stress at t=2 after you have made the correction to set the displacement to 0 instead of =0.129.
Elastic-plastic can mean Tangent Modulus = 0 or a non-zero value. You just need to say what is in your model. Perfectly-plastic means Tangent Modulus = 0.
To your first question, what are the "right" values if these are the "wrong" values?
is there anyway to produce the cure on ANSYS? The P vs h or the load vs indentation depth?
with the x-axis being the displacement and the y-axis being the load?
Copy the cells out of the Force Reaction and paste into Excel, then create the formula I provided above to convert time to Indentation depth. Below is the data from your model, after I forced minimum substeps = 20 for steps 1 and 2, with the force multiplied by 4 for a full model result.
Do you see how the curve from your model has some kinks in it compared with the smooth curve I show from my model above? That is because you have a coarse mesh. If you refine the mesh, and request more sub-steps, you should get a smoother curve.
Also, if you slice your symmetry planes to align with the edges of the indenter the way I showed you in the other thread, you may get a smoother curve since you won't have elements contacting the square edge.
Also, how would you get the stress along different paths?
For example, if I wanted to plot the distance along path vs displacement graphs from the indentation corner to the indentation centre??
Thanks for this
You insert Construction Geometry and define a Path or Surface, then you can plot the stress along that path or surface at each time step.
Create a Stress Result, but scope it to a Path instead of Geometry.
In this example below, I set it to T=2 so this is the residual stress in the coating from the center of the indenter along a direction that is "normal" to the face of the indenter (not the path on the edge of the indenter).
Also, is there a way to partially bond the substrate to the coating as now the bond in perfect?
How would you partially make it imperfect??
You would go into SpaceClaim and draw small circles on a face, you have several small circular faces and one large face with holes in it. The contact definition is only to the large face. That will simulate an imperfect bond.
P.S. don't forget to Like the posts that are helpful.
Actually, is there a function on ansys that can say set a percentage of bonding adhesion instead of estimating the improper bonding by drawing circles?
Are you interested in simulating the failure of the adhesion bond when the stress becomes too high? There are four material models.
Here are the inputs for one of them:
Yes, but i was wondering if I would be able to have a like a ratio of bonding?
It's either bonded or not. I don't know of a way to distribute flaws other than by separate faces.
Thanks for that. I will make circles and from the area of the circle I will take away the total area and this should be a correct way, right?
Also would you be able to explain how to apply hexagonal meshing to this model? I did not completely understand it last time...
Yes, just draw circles in SpaceClaim. There should be a way to do this in DesignModeler, but not as easily.
It's simple to get a hexagonal mesh, just make a hexagonal body. You don't need the cylindrical shape on the outside, it is so far away that it has no effect on the answer. Make the body brick shaped.
You can slice your geometry until it is brick shaped. Then you can put a mesh method called Sweep on the body. You can put a mesh control called Face Meshing to make a square face have quad elements on that face that will sweep out into hex elements. Sometimes, the default mesh with no controls will be a hex mesh if the body is brick shaped.
I actually made this geometry on solidworks and exported it to ANSYS. Is there no way of selecting a hex mesh on this geometry without modelling it on ANSYS?
Geometry from SolidWorks is fine and should generate a hex mesh. It doesn't have to come from ANSYS.
One reason to open geometry from SolidWorks in DesignModeler is to group multiple bodies into a Multibody part so you can use Shared Topology instead of having to use Bonded Contact to glue two different materials together.
Is there any tutorials or step by step process i would be able to follow to mesh the last achieve file as a hex mesh?
I think this (hex mesh) should produce more accurate results, is that right?
Okay libin, here is a 15 minute video for you to follow the process of getting a nice hex mesh on your indenter and a solution that only takes 200 seconds on my 4 core laptop. I have probably cut the boundary too close, but if you double the dimensions, it will be plenty large enough.
Wow! This is fantastic! I will try this for my first deliverable. However, my second deliverable is to measure the stresses when the coating is not a 100% bonded to the substrate and for that
Also, the pressure applied to the side of the coating was to simulate the presence of compressive and tensile residual stress in the coating and then compare the load vs displacement curve of both to show the difference. This means that I don't need to do the 2nd time step as I just need the data for loading.
Is there a need for the displacement 2 and displacement 3 in the model, as the fixed support ensures that it does not move, right?
I'm glad you Like it. Here is a brief video update.
When you cut away material to reduce the size of your model by taking advantage of symmetry, you must replace the material with a BC such as displacement 2 and 3 to represent the material that is missing. The missing material would prevent material in the cut plane from moving out of plane. Without those BCs, the material can move out of the plane, so those BCs are essential to get the proper results.
Pressure on the side is not a good way to create a residual stress and won't work on a symmetry model since there is a displacement BC that will stop the pressure from affecting the material.
One way to induce residual stress is to have the coating and substrate have different thermal expansion coefficients and apply a temperature load in step 1 then move the indenter in step 2.
What if the pressure is applied on the original curved surface like shown below? Because I have seen published articles that have done it this way, but the one I saw was a 2D model with a force added to the coating from both directions.
Also, is there not a way to add a hex mesh to a curved surface like seen above, or does it just work on brick shaped models?
Or something like this? But from what you have done in the video, I still had to keep the edge as I have to plot the stresses that go through that edge.
- All Categories
- Community Rules, Guidelines, and Tips
- News & Announcements
- Student Products
- Pre and Post Processing
- Physics Simulation
- Tutorials, Articles and Textbooks
- Installation and Licensing
- Student Competition Teams
- Site Feedback