Explicit analysis of single point cutting tool

  • 90 Views
  • Last Post 5 weeks ago
vaibhav jain posted this 09 February 2019

Hi, I want to do the structural analysis of single point cutting tool through ansys explicit. I am using aisi 1006 material. input parameters are speed, feed and depth of cut.how to calculate the stresses generated on the tool due to machining operation. Please guide me how to start the simulation. Thanks

Order By: Standard | Newest | Votes
SandeepMedikonda posted this 10 February 2019

Relevant Discussion 1

Relevant Discussion 2

  • Liked by
  • vaibhav jain
vaibhav jain posted this 11 February 2019

Thanks sir for your reply. Now I am getting stress values on workpiece but I am getting 0 value of stress and deformation on the tool and also my tool is not cutting the workpiece. It remains stationary and whether to give velocity to the tool or displacement to the tool. i am confused in it. what to do?

jj77 posted this 11 February 2019

If you attach your model then we can have a look for you.

  • Liked by
  • vaibhav jain
vaibhav jain posted this 11 February 2019

i am uploading the file. is it necessary that material selected for workpiece and tool should be from explicit material library. if we have to create a new material than what are the parameters required other than those parameters specified for static materials.

Attached Files

jj77 posted this 11 February 2019

I think the mesh on the large part that is being cut needs to be fine in order to see the erosion of the mesh (it is a bit coarse).

 If it is zero it is because we have an enforced velocity on all the body (makes it very rigid). Try to use an enforced displacement like the one you suppresses only on the back face of the tool, but not on all faces. I just used normal steel that you have (took away all the explicit mat. stell 4340, and used only linear isotropic), and one can see the stresses on the tool, with an enforced displ. on the back and top face only.

  • Liked by
  • vaibhav jain
vaibhav jain posted this 11 February 2019

thanks for he reply. can you please do the simple simulation so that i  can understand how the things work. i started learning explicit recently.

vaibhav jain posted this 11 February 2019

if i am using general material then stress values coming are more than 10000. what to do?

jj77 posted this 11 February 2019

well I am not a pro either (~10 years ago I used explicit).

 

As for the material I think it is just linear elastic thus stresses can go up and up (it will never yield).

 

I think that you should be able to use Bilnear Isotropic Hardening (add that to the steel prop.) in explicit, and that should make it yield.

  • Liked by
  • vaibhav jain
vaibhav jain posted this 20 February 2019

I am using the angular velocity of 30 rad/sec. The chips are not coming out and instead high values of stress come on the tool. I am uploading the file please tell what to do

Attached Files

vaibhav jain posted this 20 February 2019

@Peteroznewman sir please reply

SandeepMedikonda posted this 20 February 2019

Vaibhav, 

I am unable to look at your file but I agree with jj7, you need to have some kind of elasto-plastic behavior for chip formation. As a test, use the AL 1100-O material from the explicit materials library. See if you are observing any difference or the behavior you are expecting? If yes, then it tells me that the setup is correct and the correct material behavior is not being specified.

Regards,
Sandeep

  • Liked by
  • vaibhav jain
peteroznewman posted this 20 February 2019

On the top face, you impose a velocity.  There should be no BC on the face that is being cut!
Checking your Initial Conditions, the body is given an initial rotational velocity of 15 rad/s, but this BC is for 30 rad/s.
Why the mismatch?

The boundary conditions are in conflict. On the bottom face you are fixing the nodes to not move. With the top condition you are just winding up the tube.  You want the previous BC to be applied to the bottom face.

Your simulation time is 0.001 s. At a radius of 20 mm, at a rotational velocity of 30 rad/s, the material on the outer edge of the workpiece moves 0.6 mm around the circumference, but you have moved the tool radially 1.25 mm in the same time.  This is more like a broach than a rotational cut, except you have a radius on the tool instead of an edge. You have the wrong ratio of rotational velocity to tool tip advance speed.

You have left a Bonded Contact in the model. Delete that.

The mesh in the workpiece (lower right) is too coarse.

The mesh shown below might have a better chance of being cut by the tool. I haven't tried it. It will take a lot longer to solve.

Why do you have a 0.5 mm gap between the tool and the workpiece?

You are just wasting computation spinning the piece and advancing the tool while no cutting is taking place. Reposition the tool to be tangent to the workpiece.

  • Liked by
  • vaibhav jain
  • Jackely
vaibhav jain posted this 21 February 2019

Will you please send me the file with corrrect boundary condition. I will solve on my own. Angular velocity is 30 rad/sec. Depth of cut is .5mm

peteroznewman posted this 5 weeks ago

I haven't created a file with the correct boundary conditions, I just inserted images of the ones you had defined that were incorrect. You can make the changes I suggest above on your own.

I am leaving for a week of vacation so I will not be on this site from now till Feb 27. Good luck!

vaibhav jain posted this 5 weeks ago

i am using the materials from explicit material library but  the main thing is that i dont know how to calculate end time for simulation

peteroznewman posted this 5 weeks ago

How many rotations of the workpiece do you want to simulate? You set rot. vel. to 30 rad/s so divide by 2pi to get rotations/s and take the inverse to get s/rotation. Multiply that by the desired # of rotations and that is the end time.

Note that you used a displacement on the tool so that value will be achieved at the end time.

  • Liked by
  • vaibhav jain
Close