When you say, you made the material harder, just how "hard" are we talking about? Artificially stiffening the surface can result in contact problems.

I have some questions to get you started:

-Which one is the master and which is the slave?

-Do you get the correct amount of contact force (300N) in the second case? (create a history output)

-How rigid are the materials?

-What are your units?

+some ideas

-You should consider making a rectangular section in the middle of the tappet where it is in contact and only refine those elements. Your contact patch right now is very small and badly resolved, you won't see the pressure distribution when you only have 2 elements across.

-Hard to tell as the images are small, but these elements look like C3D10... horrible choice for a contact problem. This simple geometry can be meshed with C3D8 elements and they would give you a lot better resolution for fraction of the computing time.

There are my initial thoughts,

Following

Please share your Abaqus model (*.inp).

Thank you all for your attention and David for the useful reply.

· Cam is the master and Tappet is the slave.

· The contact force equals to the reaction force and I assume it is right.

· Young’s modulus of cam is 400e9 Pa and tappet is 200e9 Pa.

· I used SI units (m, N, Pa).

I changed the element type of the tappet in the contact area to Hex, but it is not possible to use this element type on the cam. The result is almost better but I compared it with the Hertzian stress still the Hertzian stress is 10 times of the maximum CPRESS. Additionally, the contact pressure affected area got better and is distributed to more points, but still it is not in the form of continuous and line contact. Details can be found in the attachments. I am interested to know your viewpoint if the model is valid and why still the Hertzian stress is 10 times the maximum CPRESS.

Mohammadmahdi Davoudi thanks for the detailed explanation, I think its a lot clearer now.

I've spent a lot of time playing around with contact mechanics, and my final conclusion is that a detailed fine mesh is the key of getting good results. In your case I think it is still possible to hex mesh the cam, you can section the part, make the outer surface with a small thickness as a "ring" like volume, which you should be able to mesh with hex elements. Then if you want, you can tie it to the core, which can be C3D10, and higher element sizes. The stiffness would be correct, and where it matters you should have the fine regular hex elements.

The other "trick" you can use is a "balanced master-slave" contact, essentially setting up 2 contacts, and switching the master-slave roles in the second. It's a recommended technique when you want really fine contact resolution, and all the usual steps fail to improve the result. In this case you just need to be careful when you check the contact force, as the total will be divided between the 2 slaves.

I think the resolution is still not OK, as the CNORMF is not smooth at all, there shouldn't be so much noise in the results when you capture the contact correctly.

Regading the number of elements, essentially you want to recreate a theoretical parabolic contact stress distribution with linear segments. As a rule of thumb you need about 6 elements across the contact patch to accurately do so. Your model seems to have a lot less. It is hard work designing a good mesh for contact, but fortunately now you have preliminary results, so you know exactly where to place the elements. Make everything else coarse to save on computation time, I bet this runs for a long time anyway.

Do you have contact friction by any chance? If so, switch it off and develop the model, then put it back.

Hope this advice helps

Thank you very much for the points, David. I used them and found all very effective. The problem of the contact area is solved by using a more organized mesh on the surfaces and the contact area is like a bar rather than a stain.

However, still maximum analytic Hertzian stress (1.4e8 Pa) is 10 times of FEM CPRESS (2.5e7 Pa).

What can be the reason?

Also I didn't use friction, although the works with it.

Well a cylinder to plane contact is not a line in reality it also has some width to it. You can estimate the contact patch size with for example: https://amesweb.info/HertzianContact/HertzianContact.aspx

I've guessed the dimensions of your parts, (I estimated 50mm cylinder and 30mm contact length), and I would get 0.092 mm contact patch width. That is tiny, however you need to have the appropriate amount (6 recommended absolute minimum) of elements to get a good resolution. I do understand this can make the analysis prohibitively expensive, so its not modelled like this.

Regarding the peak stress if the patch is not resolved correctly, you won't get the peak right either. In my opinion your best bet is to get the CFORCE and CAREA history outputs and divide them, to get an average stress, that you can compare with theory. (Or multiply it, there is a constant 4/pi theoretical factor between peak and average for Hertzian stress, then you can compare to the max pressure). Check if this agrees with the theory, I'm pretty sure it will.

Best regards,

David

Thanks for the attention.

The material, geometry and loading conditions are as follow:

E1=200 GPa, E2= 400Gpa

nu1=0.3, nu2=0.3

R1=10m, R2=17e-3m

F=100 N, L=0.015m

FEM result shows (as summed in the attachment ):

CNORMF= 104 N

CNAREA= 4.5×10^(-6) m^2

P_m=CNORMF/CNAREA= 2.2×10^7 Pa

From the analytical solution:

P_m=P_0×π/4

P_m= 1.35×10^8×π/4

P_m=1×10^8 Pa

Still the gap is as big as before. Why?

Ok, well if you check, your contact area is 4.5 mm^2. If you do the handcalcs (I get slightly different max pressure to you, but it doesn't matter), your patch width is 0.045mm, while the length is 15mm. So that patch area (approx rectangle) is 0.675 mm^2.

That is a difference of 6.67x. If you multiply your mean pressure from Abaqus by this number: 2.2E7 * 6.66 = 146.66 MPa. 146.66 MPa mean * 4/pi = 186.7 MPa, the calculator I linked you estimates 195 MPa, so I would say good agreement (I couldn't set the 10m radius on the tappet, I approximated it with a plane, but with such a high radius it is OK).

So what's the problem then? When Abaqus calculates contact, as soon as there is any CPRESS on an element, it gets included in the CNAREA with its full surface area, even if the contact pressure drops to 0 partway through the element. So your area is a lot bigger than the actual/theoretical contact patch.

So going back to the first comment, the problem is coming from inadequate contact patch resolution. Even if you have the recommended 6 elements across the patch, this issue will arise, but its extent will be a lot less. Obviously if you have 50 elements or more across, then the problem practically disappears... but you will struggle with runtimes. The forces are fine, because the solver works based on force balance, but pressure and contact areas are derived quantities.

Try running the analysis at a single cam angle with a significantly refined mesh at the contact patch and check what I'm saying is right. Modelling contact in FEA is hard work if you are after the specifics, not just the overall "effect" of the contact.

Right, this analytic-FEM gap issue is mostly related to the element size. When the element size is smaller, Abaqus can detect the CNAREA more accurately. Good mesh is the element size as you said 1/6th of the contact patch width (1/6*7.68e-6m = 1.28e-6m). Even if I choose the element size equal to the patch width, it is really time-consuming to run the analysis just for a simple angle. Consequently, for one rotation of cam (360 deg) is almost impossible. I need a strategy to run the analysis (or obtain the result) for one rotation of the cam in a reasonable time with appropriate accuracy.

I am glad that you agree. Regarding the approach, I can only repeat myself, make a block section of the solid where the contact patch is on the tappet (slave), a little bit wider than where you see the contact currently, and about 5-6 elements deep. This area should be meshed it with the very fine mesh. You can even make it as a separate part and tie it in to the rest of the tappet. The rest should be as coarse as possible.

On the Cam, I would section a ring-like volume where the contact is, and mesh it witch similar refinement as you have now, again 4-5 elements deep. The material is more rigid, so the other side supposed to deform more (which is the slave anyway), you could probably get away with it. Apart from the "ring", the rest should be super coarse as well.

So essentially only put many elements where you care about it. Refining the whole model is pointless, just eats up your computing resources. I don't expect this to run fast, but you can probably get it down to a reasonable run time. Other tip to speed up analysis is to not output everything. You don't need anything in the non-contact elements really, also you might be able to get just the results on the surfaces, of course depending on what is the aim of the simulation. Turn of everything you don't need. Also, when the tappet is on the cylindrical part of the cam, you probably don't need to output as frequently as when it is on the lobe. Writing to disk for a big model takes a lot of time!

Also, I don't see your whole model properly, but from the pictures I think you should be able to cut it in half as it looks symmetric, that would be a massive saving. Of course you know it better if this is not the case.