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?
- 231 Views
- Last Post 2 days ago
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.
Think about the physics of what caused the residual stress. If the coating was applied at an elevated temperature when the bonding occurred, then it was cooled, and the coating and substrate have different coefficients of thermal expansion, that will cause stress in the sample. I took your FINAL model and expanded it to a full circle and made one model with Edge Pressure of 10 MPa and another model where the temperature change causes 10 MPa of tensile stress at the face where the coating is bonded to the substrate. Look at how uniform the stress is at the center of the sample. It only changes as it gets to the free surface on the curve where it can cause some deformation.
Contrast that with 10 MPa of Edge Pressure which is supported by deformation and stress only at the edges with almost no stress at the center. This is the opposite of the thermal model.
What academic paper showed edge pressure? The quality of academic papers varies widely. One way to evaluate the value of a paper is to count how many other authors cited that paper in their own papers.
So how would you know what value of thermal expansion to use to get a required stress?
This is the paper: https://www.sciencedirect.com/science/article/pii/S0921509314009071#f0005
Also, just to get the force vs displacement curve, if I was not considering the symmetry model, would it be possible to apply a pressure to the sides?
Another thing, is the analysis like the one shown in the article only possible through a 2D model?
To find the temperature to create 10 MPa at the center, use an initial temperature change, like 9 C and calculate the stress at the center, Sci, then to get 10 MPa in the center, set the temperature change to Tc = 10*9/Sci
If you want to use a conical indenter, then you can use an axisymmetric model too. If you build an axisymmetric model you don't have to apply a fixed BC to the bottom of the steel, you can use a Y=0 displacement constraint, since the center of the sample is mathematically required to be at X=0 by axisymmetry. This means that when you apply a -10 MPa radial pressure, you can put the entire sample into a state of tensile stress. Since the steel and coating have a different Young's Modulus, this creates a small stress difference at the interface between the steel and the coating. If Young's Modulus was equal, there would be no change in stress across the interface.
Contrast the axisymmetric state of stress above with the 3D edge pressure stress from a -10 MPa pressure. In the plot below, the yellow band contains the entire range of the plot above. The reason for the larger range in the 3D model is the Fixed Support, which cannot expand with the pressure the way the 2D base can. This could be overcome by making the substrate 5 times taller and ignoring the end effects near the fixed support. The deformations below are visually exaggerated by 5000 times.
Below is the section through the thermally induced stress. Note how the same Fixed Support has almost no effect on the stress in the steel because there was no expansion of the steel as the CTE was set to zero. More significantly, there is a large change in stress at the interface between the coating and the steel due to the difference in CTE between the coating and steel. The deformations below are true scale.
For your model, you could use either method, but you might ask yourself, what is the physical cause of the residual stress? Are you interested in how the indentation affects the stress at the interface, or only the stress in the bulk material of the coating? How can you physically apply a negative pressure to the side of the sample only?
If you want to use a pressure load on the side of your sample, you need that to be applied in step 1, with 0 displacement on the indenter. Then in step 2, you can move the indenter down, and finally, in step 3, you can move the indenter back to 0 displacement. The pressure remains a constant in steps 1, 2, and 3.
I'm only interested in creating a model so that I can show the difference in the load displacement graph for no stress, compressive stress and tensile stress. I think it would be easier for me to use the 2D model, right? or would it produce the same results as a 3D model when considering the thermal method? Also, it is not possible to create a model of a Vickers indenter using a 2D model right?
Also, is it possible to do this by instead of applying a pressure, a force could be applied right?
Does axisymmetric mean 2D? Would you be able to archive the 2D model if that is ok?
Axisymmetric means the geometry is a Body of Revolution. There has to be an axis of revolution and all slices through that axis and all loads have to be the same. So, no, you can't do a 4 face Vickers indenter in an Axisymmetric model. A conical indenter, yes.
I understand you don't care about the interface and are only interested in the bulk behavior of the coating. Why do you bother to have a steel substrate, why not just extend the coating a bit deeper and have a support instead of a substrate? That way, there would be no stress discontinuity at the interface due to differences in Young's Modulus.
You can use pressure instead of temperature, but why such a low 10 MPa pressure when the yield strength of the coating is 3,430 MPa?
Here is a much better idea than a Fixed Support. If you use the 1/4 symmetry 3D model, you can replace the fixed support with a Y=0 support instead. The other two displacement BCs on the symmetry faces keep the whole body fixed at the intersection of three planes. That also means there is no stress buildup on that plane when the pressure is applied since the face is free to move radially.
"Here is a much better idea than a Fixed Support. If you use the 1/4 symmetry 3D model, you can replace the fixed support with a Y=0 support instead. The other two displacement BCs on the symmetry faces keep the whole body fixed at the intersection of three planes. That also means there is no stress buildup on that plane when the pressure is applied since the face is free to move radially."
Would this work and does this give a sort of uniform pressure throughout the indenter?
Also, I do care about the substrate as I have to plot graphs for stresses on the substrate.
The loading cycle of load vs displacement give me everything I need to measure residual stress. When there is a compressive residual stress the indenter will need to have a higher load to go through the same displacement in comparison to a tensile residual stress. This is the basis of what I'm doing so, I sort of need a somewhat uniform load so I can compare the values if that makes sense?
I would prefer to stick with the original 3D model with the vickers indenter but I'm not sure now if this is possible.
Coming to the 10 MPa pressure, it was just a random value I choose, I'm planing to vary the values and then compare the difference in the curve for loading for higher and lower values of pressure. Is putting a force load on it just as same as the pressure??
The three displacement BCs instead of the fixed support creates a beautifully uniform stress in the sample due to a pressure load on the side.
Applying pressure on the side of the sample does create stress, but it doesn't create residual stress.
Residual stress is stress that remains in the sample after the load is removed. There is residual stress when the indenter is removed because the material experienced plastic strain.
Even 100 MPa of pressure is too low to create plastic strain, it only creates elastic strain, so when the pressure is removed, there is no residual stress. You would have to apply 3,430 MPa to get past the yield point, but then the sample collapses as the Tangent Modulus is zero.
Applying elastic strain from a pressure load while the indenter goes down is not the same as creating residual strain on the surface of the coating before the indenter goes down.
You may have heard of Shot Peening, which is a method of treating the surface of ductile metals to extend the fatigue life against cracking. It works by shooting small balls of steel or glass at the surface of a metal. The impact of the balls yields the surface and creates a compressive residual stress at the surface that protects the material from fatigue cracks which develops during cyclic tensile stresses.
You have to figure out how to induce a residual stress on the surface of your coating. The load that creates that residual stress has to be higher than the yield stress or there will be no residual stress when the load is removed.
I just wanted to emulate the presence of residual stress on the coating of the model. That is what the journal article has done also I just want the stress on the coating not both the coating and substrate. I also don't want there to be strain as I just wan to see the different loads at the same indentation depth.
Is the model above just the coating of is it both the coating and substrate?
I am not really looking at the removal of the load (Unloading curve) for this study. It is only the loading that matters for the measurement. I am doing an analytical analysis of the residual stress analysis instead of simulating it straight from ANSYS.
Would what you have done above be possible on the fill final model of the indenter substrate and coating? I mean that the same uniform stress can be applied only to the coating in the full model??
The model with coating and substrate, with a 10 MPa side pressure has a distribution of stress that looks like this.
This model is with the pressure added to the substrate as well, I just want the pressure to be added to the coating.
Also, to find the load that is being applied, shod the reaction force in the solution not be applied to the displacement 1 (Top of the indenter)??
As I showed above, pressure on just the side of the coating results in very little stress at the center of the sample, while pressure on both coating and substrate results in near uniform stress on both.
If you don't want any stress on the substrate, then I recommend you use the thermal load to create stress in the coating, and very little stress in the substrate, other than at the interface.
If you don't want stress at the interface, there may be a way to use a displacement BC Y=0 on the coating at the interface during step 1 when the pressure is applied and also have the bonded contact inactive during step 1. Then in step 2, activate the bonded contact, in step 3, deactivate the displacement BC on the coating, then in step 4 move the indenter. This will result in stress in the coating and no stress in the substrate at the beginning of step 4.
Would you be able to explain how to set the temperature load? I didn't really understand the last time, sorry. Would you just click the side and then put in the magnitude of the temperature to something high?
1) In Engineering Data, for Coating material, add Isotropic Coeff of Thermal Expansion.
2) Details for Static Structural, set the initial temperature.
3) Add a Thermal Condition and set the final temperature on two bodies.
Since the Substrate has no Thermal Coefficient of Expansion, it will not move.
I know I have asked about this before but if I was not considering a symmetrical model, would I be able to do this?
It gives me a sort of uniform stress around where the indentation happens:
No! You can't cut your model down to 1/4 size and not add the symmetry BCs on the two cut faces. You don't get the same answer!
Below is the Z direction deformation with the 10 MPa pressure load you have shown on the flat faces of the coating only with no symmetry BCs.
Without the symmetry BC's on the cut faces, those faces are free to deform away from the cut plane, just like they would be allowed to do if you make a physical cut and loaded the wedge piece. But that is not what you want. You want uniform stress in the center of the sample. You get that with a full model. What you have shown is like the full model with a full depth crack from top to bottom and across the full diameter in each direction.
So to get uniform stress in the model that has been shown above, the only solution is to add thermal loading, right??
If I was just wanting to plot the graph using a 1/4 model instead of a full model, would it still not work as the maximum deformation is very low and could this not then be neglected?
Thermal loading is one solution, the 4 step method of (1) deactivating contact, applying pressure, (2) activating contact, (3) deactivating the coating Y=0 BC, then (4) displacing the indenter is another solution.
Yes, BC1 and BC2 are correct.
No, the lack of BC1 and BC2 cannot be neglected since the indenter causes huge deformations and I am sure some of that material will squish in or out past the plane, dramatically changing the stress compared with having BC1 and BC2. Why don't you try it?
Look when I reduced the model size and the fixed support is added without BC1 and 2, I think adding pressure to the side is ok?
There is still some deformation before indentation occurs but the results after indentation does not seem to deform the model like before, ill add the solution to this shortly.
It's your project, so you can do what you want, but if you use 1/4 symmetry geometry and don't add the symmetry BCs, anyone reading your report will have doubt about the validity of the results.
I gave you two options for applying stress to the coating that can coexist with the symmetry BCs (unlike the side pressure). Why don't you use one of those?
"To find the temperature to create 10 MPa at the center, use an initial temperature change, like 9 C and calculate the stress at the center, Sci, then to get 10 MPa in the center, set the temperature change to Tc = 10*9/Sci"
How do I calculate the stress at the centre?? I'm really sorry for bothering you again but ive tried doing this but I'm unclear on the method. What value would you use for the Isotropic Coeff of Thermal Expansion??
Please help, really struggling?
Would you be able to go through how you can exactly specify a certain stress of the model?
In Engineering Data, the Coating has the CTE property of 1e-5 per C.
In Static Structural, the initial temperature is entered. It is 22 C by default. You can type in 9 C.
In the Thermal Condition, you can type in 0 C so the temperature change is 9 C.
Plot the Minimum Principal Stress, probe the section near the center in MPa. Call that value Sci. Say it was 60 MPa but you want 10 MPa.
It is a simple ratio of stress to temperature change, so apply the formula to calculate a new initial temperature to type in under static structural.
Tc = 10*9/Sci
Tc = 90/60 = 1.5 C
Type in 1.5 C instead of 9 and Solve. You will have 10 MPa where you last probed.
Don't worry about the probing part. Just look at the Legend. There will be the most negative value of Minimum Principal Stress, say it shows -60 MPa, that is the 60 you put in the formula above, because the 9 C reduction to 0 C is generates too much compressive stress.
Hi there Peter, I have again had a meeting with the supervisor and he has agreed to let me put the pressure on the substrate as well as the coating! He said it would be a better way of analysis as I can validate it from papers previously. However, it again does not seem to be working as I tried the model that you archived and when the indenter goes down, it does not effect the coating but there is a displacement of y=0 already in place. Also, the boundary conditions were set by you in that model. What would be the reason for it not working??
Please attach you archive to the post above and I will look at it.
It is your own archive that you done for coating and substrate. When I unsuppress the indenter, it does not seem to work.
That archive was created to show you a perfectly uniform stress due to correct BCs and a pressure on the side of both substrate and coating. I suppressed the indenter and the contact between the indenter and the coating. Can you see that? When you unsuppress the contact, you will find one of the faces in the contact pair is not selected. Can you fix that?
I fixed the model but Im really struggling here as the load vs indentation curves look very similar with and without the pressure added! This is wrong and it should show a big difference but however, I am unable to get this difference in load. As there is a compressive pressure added to the substrate and coating the load required to go indent 0.1 mm should be considerably more than without the pressure added and even less with tensile pressure added. What could the reasoning behind this be?? Please help!
10 MPa is a 10 N of force over 1 square mm of area.
The coating stiffness is 1.3E5 MPa or a 130000 N force over 1 square mm of area.
The coating is 13,000 times stiffer than the stress created by the pressure.
10 MPa of stress is not going to make any measurable difference in the indentation load curve.
I have tried 100 MPa and even more but even then there is only like a 3/4 N of change
Okay, when you get to 130,000 MPa, you will have a stress equal to the stiffness of the coating if you are using elastic materials.
Are you still using Plasticity with a zero Tangent Modulus? You will find you can't apply more pressure than the yield strength because then the elements will collapse.
I am playing around with plasticity as I am comparing the curves for both and i was going to use the cure which gives me the best results. It doesn't really matter if its elastic or plastic with 0 tangent modulus. The maximum pressure realistically is going to be around 150 MPa
- All Categories
- News & Announcements
- Student Products
- Pre and Post Processing
- Physics Simulation
- Tutorials, Articles and Textbooks
- Installation and Licensing
- Student Competition Teams