Regarding Drilling operation in ansys explicit dynamic ( Validation of research paper)

Hello sir I am attaching one research paper along with my ansys 19.2 drilling operation file. Problem : after simulating results my answer can't match with that thesis. How can I validate that research paper for better understand of drilling operation in ansys explicit dynamic

https://drive.google.com/file/d/1DM8EUbsYP0DI2R4b1pMq-PQTcRYN29Jh/view?usp=sharing

Tagged:

Comments

  • peteroznewmanpeteroznewman Member
    edited September 13

    Validation occurs when you compare your simulation result to an experimental measurement.

    You are not doing validation. The research paper did no validation.

    Your model is wrong because you used a Fixed Support on all six faces of the work piece. You should only fix the four edge faces.

    Your model is wrong because you have zero friction in the Body Interaction. You need a non-zero friction to create heat.

    Your model is wrong because you used a Remote Displacement on all seven faces of the tool. You should only use the top flat circular face.

    Your model did not change the Erosion Controls from Strain to Material Failure. If you do those things, this is what you will get...

    I don't think the research paper produced a result that would match any experimental data. The mesh is too coarse and they only used 2 elements through the thickness of the work piece.

  • Respected sir, Thank you for your kind reply. According to your guidance I have tried simulation once again but There is huge difference in value Or Equivalent Stress ( von-mises) I am getting close answer for only total deformation. Can you please guide us for other parameter so that we can get very close in our answer according that paper.


    Also can you please tell me Erosion Controls from Strain to Material Failure in brief for better understand.

    And also How can I find temperature profile for tool and workpiece

  • peteroznewmanpeteroznewman Member
    edited September 13

    My advice is to not spend time trying to get your model results to match the results from that paper, which did not do a mesh refinement study. I don't find any scientific value in that paper. I recommend you find a research paper with a simulation result validated against actual experimental measurements including statistics on the variation about the mean.

    The default Erosion control in Explicit Dynamics is the element fails when the strain reaches 150%, which is an arbitrary value used for any material. That is not at all relevant. You have a material model that has a failure criterion built-in that has been validated against experimental measurements. That is much more relevant.

  • What about user defined Function in explicit dynamic. Like if I am trying to perform this whole drilling operation and after simulation I am Adding UDF with TemperatureAll command. Is this correct way to find out temperature profile for this operation Or are there any other approach for finding suitable temperature for drilling and other operation.

    Thank you

    Mihir Amin

  • It is called a User Defined Result and you type the name TEMPERATUREALL as you said.

  • @peteroznewman respected sir, I have applied all things with your guidance. I have doubt in analytical end time calculation for drilling operation .Can you please tell explicate

    dynamics end time calculations for 285 RPM Spindle sped .

    I am also attaching my ANSYS file in which time step error is there because I have doubt in end time calculations.

    Also how can I find thrust force in this drilling operation.


  • Hi @MAMIN219 , I am working on the cutting simulation. My experience is before the parametric study, we should do mesh sensitivity analysis first. When the mesh siez effect is ruled out, the subsequent parametric study could be reliable.

  • @peteroznewman respected sir, Please give your valuable feedback on my file and please tell how can I find end time for drilling process.


    with regards,

    Mihir Amin

Sign In or Register to comment.