Thermal aspects during Turning operation
MAMIN219
Member Posts: 42
@peteroznewman Sir I have searched so many times for accepted answer but I didn't get it. once again sorry for that I have also tried @Rob sir's approach but still not finding yet. May be I have started with new discussion so may be this is not occurring now, I am trying here my doubt as Ask a Question according to @Kremella sir's guidance.
@peteroznewman Sir i have tried with 12 mm tool travel nut still my tool is not travelling
and actually distance between that two vertex is 6.8 mm which you have mentioned in last discussion.
here i am also attaching my ANSYS 2019 file.
please guide me why this things is happening
if you find any mistake please change it and send with me for better understanding.
Please answer as soon possible.
Give regards
Mihir Amin
Best Answers
-
peteroznewman
Member Posts: 11,073
@MAMIN219 The tool did travel 2 mm.
I already answered this question in your other post. Look at the last post I made on Page 1.
The problem is the tool is 6,802.3 mm wide in Mechanical. That is 1,000 times larger than it is in SolidWorks. Clearly there is a scale error in importing the geometry, so moving 2 mm is not easy to see.
@Kp_9079 The size of the element is enormous compared with 2 mm so there is not enough penetration to remove any material.
You can measure the distance between vertices and the measurement shows up on the bottom of the window.
-
peteroznewman
Member Posts: 11,073
@MAMIN219 I can't run your model in ANSYS 19.2 because it exceeds the Student License limit.
I'm about to start running your model in ANSYS 2020 R1. I would then see how it looks after 24 hours.
The zip file was attached two days ago. Please reply with your results after 48 hours of compute time.
You ask how to get the results as fast as possible. I told you before to check Characteristic Length. Did you plot the Characteristic Length for your mesh?
The minimum Characteristic Length is 0.025 mm
The most of the elements you will be cutting initially have a CL of about 0.125 mm.
Can you see how it would be possible to make a mesh where the minimum CL was 0.125 mm instead of 0.025 mm? That would mean the maximum time step could be 5 times larger, cutting the solution time by a factor of 5.
Under Analysis Settings, Output Controls, you set Result Number of Points to 20. That number is too small to see a good animation of the model. Set it to 2000.
-
peteroznewman
Member Posts: 11,073
By modifying the geometry, I can increase the minimum CL length to 0.1 mm, which is 4 times faster than what you had.
One mistake in your model is that the Angular Velocity and the Remote Displacement rotation are both positive, but the correct direction of the tool is to have these be negative.
One problem with your model is the workpiece material is a linear elastic material. If you don't use an Explicit Dynamics material with some failure criteria, then you should add a Plasticity material model so the material can flow and fail by meeting the Total Strain criterion.
-
peteroznewman
Member Posts: 11,073
You intended to rotate the workpiece in the blue direction and that is what you did in your model.
All the metal turning literature I have read shows cutting by rotation of the workpiece in the orange direction against the flat face with a small rake angle. I don't believe you have the correct understanding of metal turning practices.
I don't have access to a cloud facility to run this model, just a simple 4-core computer.
I'm not finished with my simulation yet, and I may not be happy with the result, so don't wait for anything from me, because I won't attach any archive I am not completely satisfied with. I can't change it after I attach it. I advise you to make your own mesh with a larger CL.
-
peteroznewman
Member Posts: 11,073
Completed the test with the tube on a global axis, the elements were eroded by excessive shear strain. Something is very wrong with the model. I only expect a small amount of strain due to the centripetal forces, which are not very large because the diameter is small and the rotational velocity is small. I think a New Question is worth posting on this topic and I will do that soon.
Answers
@peteroznewman Sir
i saw @MAMIN219 file , in that if the tool was moving then why there is no removal of material from the workpiece ( chip formation) ?
@MAMIN219 The tool did travel 2 mm.
I already answered this question in your other post. Look at the last post I made on Page 1.
The problem is the tool is 6,802.3 mm wide in Mechanical. That is 1,000 times larger than it is in SolidWorks. Clearly there is a scale error in importing the geometry, so moving 2 mm is not easy to see.
@Kp_9079 The size of the element is enormous compared with 2 mm so there is not enough penetration to remove any material.
You can measure the distance between vertices and the measurement shows up on the bottom of the window.
Respected sir @peteroznewman
Well , sorry for disturbing you number of times ,
However I am trying these simulation from the past 1 month and following your proper guidance , still i am not able to achieve the movement of the tool , and consequently chip formation .
So sir please can you guide me where I am making mistake , so that i can successfully achieve my target.
I have also performed this data in ANSYS 2020 R2 but Here I am sending ANSYS 2019 file so please check this file and send feedback with us so we can get clear idea about it and also this simulation is too much time taking so what can i do for reduce time .
I have applied automatic mass scaling option 'Yes"
please guide me and simulate this file if any mistake . so that I can understand where i am mistaking in My simulation. Once again Thank you @peteroznewman Sir
for always replying my post with clear clarification.
Give regards,
Mihir Amin
@peteroznewman Respected sir ,
Please Give answer,
What can I do to simulate this result as fast as possible
Refer my previous file and Question and please answer me as soon as possible
Give regards,
Mihir Amin
@MAMIN219 I can't run your model in ANSYS 19.2 because it exceeds the Student License limit.
I'm about to start running your model in ANSYS 2020 R1. I would then see how it looks after 24 hours.
The zip file was attached two days ago. Please reply with your results after 48 hours of compute time.
You ask how to get the results as fast as possible. I told you before to check Characteristic Length. Did you plot the Characteristic Length for your mesh?
The minimum Characteristic Length is 0.025 mm
The most of the elements you will be cutting initially have a CL of about 0.125 mm.
Can you see how it would be possible to make a mesh where the minimum CL was 0.125 mm instead of 0.025 mm? That would mean the maximum time step could be 5 times larger, cutting the solution time by a factor of 5.
Under Analysis Settings, Output Controls, you set Result Number of Points to 20. That number is too small to see a good animation of the model. Set it to 2000.
By modifying the geometry, I can increase the minimum CL length to 0.1 mm, which is 4 times faster than what you had.
One mistake in your model is that the Angular Velocity and the Remote Displacement rotation are both positive, but the correct direction of the tool is to have these be negative.
One problem with your model is the workpiece material is a linear elastic material. If you don't use an Explicit Dynamics material with some failure criteria, then you should add a Plasticity material model so the material can flow and fail by meeting the Total Strain criterion.
Thank you so much @peteroznewman for perfect clarification of my doubt.
I am really thankful for your valuable comments and feedback as well as motivation with projects by giving Valuable answer.
I have also tried plot but didn't understand properly that's why I have asked regarding that. Now I have clear clarifications on that.
Right now I didn't have any research license or cloud facility so
Can you please send file after 7 days if possible.
Or send me that updated file then I will try to simulate any other place.
Please explain logic behind opposite direction of angular velocity and remote displacement. I didn't understand that yet so please elaborate for better understand
And please send that simulated file if possible
Once again Thank you so much for always giving great feedback and helping us.
Give Regards,
Mihir Amin
@MAMIN219
Which direction do you understand the workpiece rotates, the blue arrow or the orange arrow?
@peteroznewman In your above picture
Arrow with blue colour which is direction of workpiece. Tool travel is -z direction according to coordinate system.
If any wrong concept please highlight this and give your feedback with reason for better understand.
If you have cloud facility with you and possible then run this simulation so that i can understand properly temperatures effect in this simulation which main aim of my simulation.
Otherwise send me your updated file for better understand which will take very less time consumption. So that i will try to simulate as soon as possible.
@MAMIN219
You intended to rotate the workpiece in the blue direction and that is what you did in your model.
All the metal turning literature I have read shows cutting by rotation of the workpiece in the orange direction against the flat face with a small rake angle. I don't believe you have the correct understanding of metal turning practices.
I don't have access to a cloud facility to run this model, just a simple 4-core computer.
I'm not finished with my simulation yet, and I may not be happy with the result, so don't wait for anything from me, because I won't attach any archive I am not completely satisfied with. I can't change it after I attach it. I advise you to make your own mesh with a larger CL.
@peteroznewman Thank you so much for your brief explanation and clarification of all doubt.
I will check CL and all things related to direction which you have guided me me and also I will change explicit material with failure criteria.
With Regards,
Mihir Amin
@MAMIN219
I suppressed the tool and had only a cylindrical tube with an initial rotational velocity in rad/s, and a remote displacement scoped to the ID with an angular displacement in degrees. When I divide the angle by the end time, it is equal to the initial rotational velocity. I ran that simulation just to see the workpiece rotate at about 350 RPM.
I was disappointed to see the workpiece develop a huge strain over the simulation until elements were eroded away as they reached the 50% strain value I had set.
This is an unexpected result.
I wonder if it has anything to do with the fact that the axis of the cylinder is a large distance from a global axis. I intend to edit the geometry and move the cylinder to be on a global axis and see if I get a different result.
Completed the test with the tube on a global axis, the elements were eroded by excessive shear strain. Something is very wrong with the model. I only expect a small amount of strain due to the centripetal forces, which are not very large because the diameter is small and the rotational velocity is small. I think a New Question is worth posting on this topic and I will do that soon.
@peteroznewman yes sir sure. Thank you for always giving your valuable feedback and motivate us😊