Have you first tried a by-hand calculation to get a first estimate of the stresses in the beam? Secondly, note that a concentrated load at one node will give you a local stress singularity (meaningless) which may significantly alter the color scale of your output. Try with a threshold to see the stress distribution in the beam

You could make a small block/surface and you can push it to the edge and let Abaqus resolve the contact stresses. That would help with the concentrated force singularity problem.

I think no, if contact is on one node only you still have singularity (but now a much higher numerical complexity because of contact)

Denis Benasciutti and David Sziroczak Thank you both for taking the time from your day to answer my question. I will try to do that right now.

Currently I am applying the same force that a journal paper applied on the chip area. I believe that the meshing i am using is fine. I have attached two images of my forces being applied on the nodes that cover the contact area

I have broken my chip-tool contact area to 22 nodes.

I have a total of

530 N in the X direction So... 530/22 = 25N/node

1330 N in the Y Direction

265 in the Z Direction

I have attached an image of the force values for a 75 degrees cutting edge angle. I have also attached my current mesh

All the above is CLEARLY NOT WORKING... So I will do the following below.

1. I will apply a pressure on the by hand calculated chip area ( the chip that generates the forces on the tool) instead of nodes and if that doesn't work.

2. I will make my area very fine and distribute the force there.

The paper i am referring too is " Finite element analysis of bending occurring while cutting with high speed steel lath cutting tools" published in " Material & Design"-Elsevier in 2005

applying a pressure instead of nodal forces will not improve very much your solution, as a pressure on the side of a finite element will authomatically be converted into consistent (equivalent) nodal forces via the Principle of Virtual Displacements. You may check your solution with analytical solution (for example, bending and torsion stress) at a section far away from the point where loads are applied

Hello Denis Benasciutti thank you again for quick responses.

I have made my chip area much finer ( went from 26 nodes to 199 nodes). I distributed the forces equally between the nodes.

I attached Four images

The tool meshing,

The forces being applied & The values I am using to apply the forces from the paper

The results I got

The results the author got

I have followed the limited information that the author of the paper provided, and the author compared an analytical model results with FE results of ANSYS ( not ABAQUS) .

My maximum deflection was :0.04065 mm

The author maximum deflection was : 0.2158 mm

From your experience in ABAQUS, is there a type of constrain or any possible tool that can make the the program know that this applied force is going to impact the chip area but in the same time the whole beam (tool) should be impacted... I am looking at it from a deflection stand point. Because I know the tool has to act like a cantilever beam but its not doing that. Btw i have fixed the back end like i mentioned earlier.

I am new to ABAQUS , and i watched countless videos online / tried to read the manual but until i haven't been able to duplicate the results.

Yes your are right, there is an issue with edge contact, however the aim of the contact is to allow for compliance and redistribution of the load as your result as opposed to idealising a single node load, which is a lot less realistic. Using a couple of nodes in contact with a rigid surface is unlikely to result in excessively high computational demands.

David Sziroczak From your ABAQUS experience do you have suggestions ?

Thank you.

Well I would go through the following questions 1 by 1, most of them are pretty obvious, but just to be certain. After that we can see:

1) Are all the materials defined correctly, and you have a consistent unit system?

2) You don't have plasticity or any additional behaviour applied over the base linear elasticity, do you?

3) Does the reference model you are replicating have any other features, fillets/chamfers?

4) What elements are you using? You should try changing to something else, like a C3D20R at least on the tip. It might just be that the tip element reacts poorly to the applied loads. Check the energy totals in the history to see if the applied work matches the elastic strain energy, if not, then at least we can see what takes up the energy.

5) If you want to improve the mesh you can always cut out a tiny block near the edge, make a super fine mesh on it and then tie it back to a coarser mesh. I don't think mesh resolution would be the problem here, but just an advice

The deformation you see is scaled by a scaling factor, so the actual deformation you have is much smaller.

You probably need to switch on NLGEOM (which then sets this factor to 1) depending on what exactly you are trying to do.

David Sziroczak Thank you for your useful comments.

Martin Baeker, thank you for your useful comments. Also, having NLGEOM on definitely helped with overall "looks "of the results. I have attached an image of it.

I am looking at the "Deflection" on the tool ( treated like a cantilever beam) Unfortunately the result I got in ABAQUS is much higher than the results that was in the journal paper that I am trying to duplicate.

My ABAQUs Deflection = 0.6684 mm ( for the tool of a cutting edge of 75 degrees) I terminated the job, because the deflection was way off and there was no point of continuing to run it.

Journal Paper ANSYS Deflection = 0.04065 mm ( for the tool of a cutting edge of 75 degrees)

Please let me know if I am making a mistake or if you have any suggestions

The below are the steps I have taken to get the results I got in ABAQUS

The steps:

1. I designed my tool in SolidWorks and imported in into ABAQUS

2. I have created the mesh for the tool ( the area where the load is applied is much finer than the rest of the body . There is a total of 103812 nodes and 96551 elements

3. I imported my material properties ( straight from the journal paper)

4. I turned On the Nlgeom option

5. For the chip area, I created a set of 105 nodes where where the load is applied equally over each node

6. I fixed the back end of the tool, to treated as a cantilever beam

7. I applied the force ( the same values as the paper).For example. 530 Newton is applied in the x-direction so per node the force is (530/105 N/each node) in the x-direction, the same procedure was followed for the y and z direction in terms of force application

Btw my results and the paper's results are in mm

I have attached images for the following

- meshed tool

-force nodes

-edit step where Nlgeom is ON

-forces being applied on the nodes

-where the tool is fixed

-the paper's results

-my results which is clearly off

I you have any suggestions/comments for my ABAQUS usage procedure. Because the results I am getting is way off. Anything is much appreciated.

Thank you.

Can't see anything wrong, but I would recommend to change the application of the force: Partition the surface to define a region where you apply the force, then apply the force as surface/pressure load. That way, there is no need to change anything when you change your mesh.

And critically look at your material definition - is it purely elastic? Have a look at stresses. And check your element type.

This paper contains some hints on how to check a model:

Preprint How to get meaningful and correct results from your finite e...

Martin Baeker

Thank you.I will definitely give the paper a read.

Also, regarding the material properties I just inputted the density, Young's Modulus, Poisson's ratio, the yield stress, and the plastic strain.

Note plastic strain = 0 when yield stress = 850 MPa. is that what you meant when you asked me to make sure my material is purely elastic ?

Also, I have created a partition where I applied the force. I assumed only the vertical force in the Y- direction so the pressure was

Pressure = Force/Area -> Pressure = 1330/(2mm*0.2mm) = 3325 N.

Below I have attached two images

1. of the partition and the force being applied

2. Of my results which are still off from the paper

I also attached my "Inp" files

labeled "tool_75_job103" is the inp file where i applied the force

labeled "NoUse1" is the inp file where i applied the pressure

I would really appreciate it if you can take a look at it and give me your opinion.

Thank you.

This was one of the questions, are you looking at purely elastic behaviour? Judging from your input file:

*Plastic

850.,0.

You are not. This line means that your material starts to yield along a flat line once you reach yield stress, effectively the material flows away. This can lead to convergence issues and its non-physical as well. Remove the plastic behaviour first to debug your model, that is a general advice by the way.

If you want to use plastic behaviour and you want "real" results, then it is a good start to have real plastic curves.

David Sziroczak, thank you for your reply. Most likely i thought i understood u the first time but due to my lack of experience with the software i assumed that I didn't have issues in that point.

I will remove the plastic property off my material.

To have real plastic curves I should indicates the stress values at multiple strain values based on the true stress-strain curve correct ?