Regarding How to change multiple back rack angle in turning simulation

Respected Sir

Here I am trying to simulate my Turning operation simulation. In which I am intended towards change of back rack angle effect of +10, +5, 0, -5, -10. I am attaching my ansys file in which I have applied all necessary data for turning operation and in this present simulation I have used 0 back rack angle. So can you please help me how can I simulate this four ( +10, +5 , -5, -10 back rack angle) at a single time

Please send your file after changing this data for better understand

Thank you so much sir

Mihir Amin

Tagged:
«1

Comments

  • I think the element size is too large to get useful results from this simulation. Use smaller elements on the workpiece. What are you trying to show as the angle changes?


  • Thank you for your reply.

    I am talking about how to set angle as parameter so that I have run one time simulation and after that only I have change that value of different angle so no need to change multiple times and get effective output in single time simulation

    Here I am also attaching one photograph for your reference


    Another question

    Can you please guide what type to mesh is recommend for this frictional Turning operation for getting effective Temperatures profile on Single point Cutting tool.

  • peteroznewmanpeteroznewman Member
    edited September 20

    @MAMIN219

    Is the tool at some odd angle and off the centerline of the turning axis for a specific reason or is it just because you didn't know how to square it up and center it?

    I moved it to be squared up and on the axis. I also moved the parts to put the axis at the World Origin.

    Here is a 10 degree rake angle

    Here is a -10 degree rake angle

    Do you have access to a Research license? The mesh below has 250,000 nodes.

  • Thank you so much Sir for your reply. Now I will check by implementing This four different back rack angle value as your file in which you have set parameter for that. Yes sir My university has research license for that.

    Thank you so much once again for always giving reply and motivating me to do this type of work 👍

  • peteroznewmanpeteroznewman Member
    edited September 22

    I made the workpiece into a Tube instead of a Rod to get better elements that had a larger characteristic length Mesh Metric than the mesh I made in the previous post.

    To make the simulation take less time to compute, I increased the density of the materials by a factor of 100 which reduces the solution time by a factor of 10.

    I also increased the rotational and translational velocity by a factor of 100 to reduce the end time of the simulation by a factor of 100 for a total reduction in wait time by a factor of 1000.

    Unfortunately, these changes to the physics make material move in a way that it does not when using real density and real velocities and end times. The result was that the centrifugal force on the workpiece caused the material to expand radially and the Poisson's ratio made the length shrink faster than the tool advanced, so the edge of the workpiece moved away from the tool in the first 0.1 milliseconds of the simulation. It didn't help that when changing the end time, the tool advance distance ended up being 5e-3 mm instead of the intended 0.5 mm.

    In the next iteration, I would reduce the velocities by a factor of 10, and increase the end time by 10, but increase the element size to recoup some of the extra simulation time that will entail. I would also insert an Initial Condition of the Velocity of the Tool. I forgot this on the attachment.

  • After about 25 degrees of rotation, the tip is starting to heat up. This ran for a few days on my 4-core computer, so you are going to wait a few weeks for one revolution. You might consider a coarser mesh to speed up the solution. Pay attention to the Mesh Metric Characteristic Length, which is at the bottom of the list. That is what controls the maximum time step.

  • I have so many doubt regarding your answer. So I am writting here this


    1) Why are you select Tube instead of a Rod bcz both have different things after that simulation there are different value of temperature.

    2) right now I am. Selecting material for Single point Cutting tool(HSS ) and Workpiece ( LM 6 which is one of grade for Aluminum alloy).

    You have taken value for 100 multiple for original value for density and alll change the value for velocity for our simulation takes less time

    But i can't understand your last Message which Is start from

    " Unfortunately, these changes to the physics make ..! " Please highlight on that

    Also please tell why are your selecting whole workpiece or whole tool you have select some faces so please tell regarding that


    And can you please brief for reason behind this type of mesh . More highlight on mesh why are you select this particular mesh is there any reason/ physics behind this

  • peteroznewmanpeteroznewman Member
    edited September 25

    1) The only reason to convert the geometry from a rod to a tube was to get elements with a larger Minimum Characteristic Length so that the solution would take less time to compute.

    2) Use whatever materials you want for the two parts.

    If you artificially increase density by a factor of 100, the solution will solve 10 times faster. This changes the physics because everything is heavier, but the stiffness didn't change. So if you are rotating by some angular velocity, the displacement will be 100 times greater.

    I artificially increased the rotation speed and the translation speed to reduce the end time. I overdid this on the first attempt and the part changed shape too much, so I dialed back the artificial increase in speed, but that required the end time to be longer to get one rotation so the solution ended up taking weeks instead of days.

    The time it takes to solve depends on the minimum characteristic length, the density, the modulus, the speeds and the end time.

  • peteroznewmanpeteroznewman Member
    edited September 25

    @MAMIN219

    With larger elements, the simulation made 1/3 of a rotation in 7 hours so expect about 21 hours/rotation. Now you can get one rotation per day. The tip temperature has risen to 783 degrees C, but that is not really useful because the workpiece is rotating 10 times faster than it does in reality, so the temperature in this simulation is probably higher than the true temperature. Unfortunately, if you slow the rotational speed to the real speed, it may take 10 days to do one revolution instead of 1 day, and you probably need many revolutions to get the tool temperature up to a steady state.


  • MAMIN219MAMIN219 Member
    edited September 25


    Thank you for your mail @peteroznewman.

    Respected @peteroznewman Sir,


    I want to clear my fundamental regarding these density for getting simulation rate faster and more knowledge on how can predict for suitable mesh for any Finite Element Analysis. In addition how to get near answer of Temperatures which is conceptual and also possible in reality.

    Also Material Removal Rate is one the key features in Any Machining process so I want to understand MRR for This Turning process which will give some fruitful real in industry level.

    Also my main concern is to learn what's going behind ansys means I want to learn this all things as analytical solutions for better understand like Matlab coding or like hand analytical calculations for understand "Heart of this analysis"

    And for that i have to apply that on my main project .

    So Can You please send me your mail id

    Here I am also sharing my mail id with you so you can share you mail id in that

    [email protected]

    Once again Thank you so much Sir for always continues reply and providing you valuable time with students to motivate and enjoy the better research skill in simulation and CAE field .


    Regards

    Mihir Amin

  • peteroznewmanpeteroznewman Member
    edited September 25

    Dear Mihir Amin,

    Thank you for those kind words. You are sharing your mail id not just with me, but the whole wide world. It's not necessary because we can communicate here @MAMIN219 .

    The MRR is a combination of the Turning Speed and the Feed Rate of the Tool. The Turning Speed depends on the workpiece diameter and the spindle RPM.

    Here is a good discussion to help understand the Maximum Time Step, which has a lot to do with how many hours you will have to wait for the solution to compute.

    Regards,

    Peter

  • peteroznewmanpeteroznewman Member
    edited September 26

    @MAMIN219

    While the larger elements allowed one rotation in one day of simulation, the elements were too large for the single point cutting tool to remove material in a meaningful way as you can see in the attached video.


  • Respected sir @peteroznewman

    Can you please explain like We are doing this simulation in ansys so can we get some nearer value like ex I am getting output of temperatures via thermal camera is 101 degree Celsius and also getting value of ansys temperatures value is like 90 degree or nearest to 105 or 110 degree like nearer to this value.

    Or can we use other moving mesh to getting this results in simple manner.


    I am also intended towards analytical approach for this too. Also please send analytical solution or Analytical Method to exactly how can we write FEM standard in hand with forumula base like whats the things behind ansys for feeling the heart of this results 😊

    In Addition I will send my file with you and my calculations of this end time. You will tell is my calculations for end time and all the things are correct like you

    😊

    Thank you sir

  • peteroznewmanpeteroznewman Member
    edited September 27

    @MAMIN219

    My last attempt was to use more traditional rake angles than what you started with.

    Unfortunately, the elements are still too large to get good material removal.

    The tool tip is starting to erode and with the switch to hex elements on the tool, some hourglass defect has made its way into the mesh.

    I recommend you use Google to search for academic papers on single point cutting and see how researchers did this without using Explicit Dynamics. You can't do a study on Rake Angles if each setup takes a month to solve.

  • Thank you for your suggestions @peteroznewman SIR,

    with your advice I have tried Transient Structure analysis incorporate with APDL command in ANSYS 2020 R2 academic .I have put all the required things according to this attached thesis .I have not much more knowledge about APDL command and CONTA so I am trying this new things. Can you please help me in this. Is this correct approach towards Turning simulations.

    Please highlight more on APDL command and send file with me for better understand,


  • The Transient Structural analysis described in the 2016 Thesis has no material removal. There is only friction between the tool and workpiece generating heat as a function of the speed of rotation.

  • Thank you for your reply sir @peteroznewman ,

    Here I am attaching My ANSYS 2020 R2 file. Also I am putting here me calculations and all specification if there are any mistake please guide me.

    1) I have taken Workpiece (Aluminum alloy LM6 material) and Single point cutting tool(HSS material).

    2) I have defined Frictional contact between SPCT and workpiece and put 0.8 has frictional coefficient. and also go body interaction and put 0.8 as frictional coefficient. I have doubt in this : is there necessary to define frictional contact via manual contact region. or we have assigned body interaction and direct go type and assigned as frictional and put frictional coefficient. Please clarify this doubt and brief discussion this .

    3) then I have used your previous mesh here. if any changes please guide me in details.

    4) here I have taken Feed=0.4 & RPM=350

    L=cutting length per min =feed*spindle speed=0.4*350=140 and so on.

    here I am trying to move my Single point cutting tool as 20 mm

    that's why i have taken displacement and in that for x =(0.0007 Depth of cut) and in z=(0.02 tool travel ) In addition in displacement 2 i have defined cylinder and coordinate geometry so i have taken Y= (17998.9718)

    and i have found 8.5714 as my end time

    i have also mentioned my logic behind value in y which is 17998.9718


    Please give your feedback with explanation and mention any mistake or false procedure on it


    thank you

    Mihir Amin

  • Please review this Wiki article on Feeds and Speeds. https://en.wikipedia.org/wiki/Speeds_and_feeds

    Your document uses the word feed in an equation with RPM, which is wrong. Cutting Speed uses RPM and the diameter of the workpiece in an equation to calculate the tangential surface speed of the material being cut.

    Feed Rate is the velocity that the tool tip has along the axis of the workpiece.

    The depth of cut together with Cutting Speed and Feed Rate determine the Material Removal Rate.

    Different materials have different cutting speeds that work best for them. https://www.cnclathing.com/guide/cutting-speed-chart-for-different-materials-in-turning-drilling-and-more-cnc-machining-processes-cnclathing

  • Greetings,

    @peteroznewman Sorry to crash in on the discussion. I am facing a problem in my 2D simulation and would greatly appreciate your input. In my 2D simulation for Inconel, I am unable to get the temperature distribution on the tool. I have defined the tool with flexible stiffness, thermal property and plasticity model. I added the temperature through the worksheet after the simulation. But it always only gives the temperature distribution on the workpiece. Not the tool. What am i doing wrong? I have also attached images of the material properties and the .wbpz file. Would greatly appreciate your support.


    This is the link to the actual post: https://forum.ansys.com/discussion/15835/missing-tool-temperature-distribution-2d-explicit-dynamics#latest


    Gratitude for the support.


    Regards

    Ibrahim Nouzil

  • @peteroznewman

    Respected sir,

    1)I have defined Frictional contact between SPCT and workpiece and put 0.8 has frictional coefficient. and also go body interaction and put 0.8 as frictional coefficient. I have doubt in this : is there necessary to define frictional contact via manual contact region. or we have assigned body interaction and direct go type and assigned as frictional and put frictional coefficient. Please clarify this doubt and brief discussion this .

    2) I have applied angular velocity as 36.56 (for N=350 RPM) AND velocity as 0.421( using formula pi*D*N/60 AND N=350,DIAMETER 23 MM for cylinder ) and end time i have calculated my last conversion photo and conversion. I am also mentioning regarding link from which i have calculated my end time for 20 mm tool travel length

    3)

    this is your snapshot from your second file .please give me your guidance regarding my parameter so what are those values on remote displacement which i should give to run this file .and also tell which face i should select for this remote displacement.

    Please give your feedback with explanation and mention any mistake or false procedure on it and send your corrected file with me for better understand .

    Thank you .

Sign In or Register to comment.