Simulation at micro scale

[Vxxxxx]

Hi, I have done simulation on othorgonal cutting of a certain material, and the size of my workpiece is 1x5 mm.

So right now, I have trying to do the same on a microscale level, size of my workpiece is 0.15x0.05mm, but it doesnt converge,takes unreasonable calculation time and shows this common error: "The analysis may need a large number of increments (more than 20,000,000)and it may be affected by round off errors...".

Everything was the same, material properties, interaction properties, etc
Step chosen is dynamic temp-disp explicit.
Mass scaling 5000.

PS: when i switch to dynamic explicit for the microscale model, it worked as normal.

I have never encountered such weird situation, and it would be great if someone could provide some insights. Thank you.

 

[FEA way]

Stable time increment in Abaqus/Explicit analyses heavily depends on element size, among others. You can try reducing mesh density, speeding up the process artificially (by decreasing step time) or using mass scaling.

 

[Vxxxxx]

Hi FEA way, the problem is, the mesh is not even densed, workpiece element no. is 4375, tool element no. is 535, mass scaling 5000.
i even tried step time 0.000001.

I have no idea what is going on.

 

[FEA way]

Check the stable time increment computed by Abaqus for you mesh. Try further increasing the mass scaling factor and make sure that you use all CPUs that your machine has for this simulation.

 

[Vxxxxx]

Okay I will try and come back soon with some results. Thank you.

 

[Mustaine3]

I wouldn't recommend scaling with a factor. Use a target time increment instead. With this only the really needed mass is added and nothing unnecessary.

 

[Vxxxxx]

Okay will try target time increment as well, thank you @Mustaine3

 

[oldNail]

If you are simulating a dynamic process then the large mass scaling will obviously have a large effect on the result. In that case you must coarsen the mesh or Explicit is not suitable.

 

[Vxxxxx]

I realised that mass scaling of 5000 and 30000 has no difference on the simulation time. If I coarsen my mesh which is undesirable, I would encounter problem of mesh extremely distorted, which also stop my simulation from running. Its like an endless cycle, if I wanna reduce simulation time, I have to increase element size; if I want better results/avoid element distortion, I have to decrease element size, but the simulation takes so long like for example, 1 out of 500 output takes 2-3 hours or even longer.

 

[oldNail]

Mass scaling should directly increase your stable time increment and reduce runtime. If that is not happening then something must be wrong with your setup. However, if you are modeling a dynamic process (and I think you are, right?) then all that additional mass will make your results nonsense.

What type of elements are you using? Abaqus 2021 has new distortion controls for C3D10 elements in Explicit. Maybe that will be helpful for you.

 

[Vxxxxx]

yep im doing 3d elliptical vibration machining simulation and im using C3D4T for tool and C3D8RT for workpiece.
I tried using second-order accuracy for my workpiece and at least my simulation is completed and it took 82 hours for step time of 0.0001s. (Dynamic,temp-disp,explicit, general contact)

 

[oldNail]

I'm glad you have a result.
Note the confusing nomenclature that "second order accuracy" mentioned in the element type suboptions is not the same thing as using quadratic C3D10MT elements and that these quadratic elements will have a smaller stable time increment for the same element size.

 

[Vxxxxx]

Noted, Thank you very much. @oldNail