Use this forum cfd.oline it can help you. Good luck.

Thank you..

you mean http://www.cfd-online.com/Forums/

Check the thickness of your specimen in 2D and 3D; in 2D, it is the value given in the section definition; if you did not provide a value, Abaqus assumes 1 in whatever units you are in.

Apart from that, without further information or a look at the models it is difficult to say anything.

Thank you very much for your suggestions. I am checking the result for larger thickness.

In 2D simulation, work piece size is 3μm x 1μm with default thickness. All my units are in Newton, mm, second, degree. that means thickness will be 1 mm as you mentioned.

after running cutting simulation of 100 nm depth of cut, i am getting 0.5-1 Newton force in 2D.

Whereas for 3D simulation, length and height are same as 3μm x 1μm, but thickness is 1μm.

Martin Baeker sir, what modification you suggest for 3D simulation for getting similar result as 2D simulation.???

Are you sure that this software have the mathematics to resolve the size effect?

Martin Baeker sir, you are right... The force value has increased... but..now the problem that I am facing is ----if I take actual width of cut (i.e. thickness) 250μm, the no. of elements will be very very large as I have to take care of 100 nm depth of cut.. 

 in figure I am just considering 100μm thickness.

does any body have solution for it..??

Check your units. I am quite sure that you did not introduce well defined units to software. At first think about on which scale you want to carry out the simulation. For example, if it is in mm then you have to convert all of your input values to mm. It is very important to consider this for example density is a function of length scale you have to change that one too. Etc.

@Ali Sir,

I have converted all my input values such as young's modulus, density, velocity to mm, N, sec.. etc... 

But i am not sure what you meant by last sentence... "It is very important to consider this for example density is a function of length scale you have to change that one too. Etc.",

Can you kindly explain it...

Dear Borad,

When you get 1000 N in 3D and 1 N in 2d or vice versa it means that this is not something happening because of addition of another dimension. For me it means that you didn't insert inputs properly or there is something wrong with geometry. Try to work around these issues to figure out why you are getting such difference. when you are converting SI units to be as mm then you have to  be careful about each input depends on dimension or length. Density is Kg/m3 did you convert that m3 to mm3? Check your calculation.

If still you could not fix the issue then provide pics of your inputs and your 2d/3d models. 

BTW, I am curious why you want to carry out plain strain problem in 3d while you can do it easily in 2d? 

Good luck.

Thank you @Ali sir...

Yes, I did... I have converted all units to similar unit (i.e. mm, N, sec, degree). as you said kg/m3 to tonnes/mm3.. and my model is in mm. 

For your kind information, I am working on machining simulation of Silicon carbide using negative rake angle tool. and analyzing cutting force and thrust force. During 2D simulation, failed element (chips) does not contact with workpiece itself. I know in 3D simulation I can generate element based surface and contact problem can be solved.

As Martin Baeker sir suggested, plain stress/strain thickness was the issue for getting different force values.

Are you using any failure model in the model? Element deletion? 

ductile failure.. 

with element deletion .. 

Ok. That is your problem. Try to simulate chip formation without failure model with pure plastic deformation. It has been a long discussion in FE machining of materials and the use of failure model is not recommended because the material on contact will not attach to the tool and then you have deterioration of results. I understand if you don't use element failure you cannot separate the chip in Lagrangian domain analysis because of element distortion but this is how it works. You have to use more advanced adaptive remeshing techniques such as ALE (Arbitrary Lagrangian Eulerian) technique to simulate chip formation. There are tons of publication with topic of ALE, follow them and do your simulations.

I at least partly disagree with Ali. It is possible to get meaningful results with element deletion in a cutting simulation. You have to make sure that you use general contact with the internal surfaces of the elements included so that even after element deletion there is contact.

However, it is important that your deletion zone is small and that the total volume removed by the deletion is also small.

Nevertheless, there is a large number of publications using this technique successfully.

you can contact me regarding your problem at [email protected]

@ Martin: you are right, but i personally had problems to define general contact in 2D. I always  got error after defining it. At least, it was impossible for me to define this type of contact in 2D. That's why it's very tricky to get the right chip formation in 2D. Another issue that i faced is related to study Temp.disp. along the tool.I used both dynamic-explicit-temp and coupled temp-displ, with the corresponding elements,but none of them worked.