Ansys of drilling operation

  • Last Post yesterday
  • Topic Is Solved
Krishna posted this 07 April 2018

Hi everyone I need a help regarding a drilling operation simulation in Ansys.

Analysis of Tool life and Tool wear, simulate and show the temperature generated during a drilling operation.

Trying to achieve: Tool life of the drill Temperature created during drilling

  • Liked by
  • Raef.Kobeissi
Order By: Standard | Newest | Votes
Raef.Kobeissi posted this 07 April 2018

I think Peter would help more in this area but the first thing that comes up to my mind is 'Explicit Dynamics' coupled with Thermal and Structural analysis. Peter is this possible?


Raef Kobeissi

  • Liked by
  • Krishna
peteroznewman posted this 07 April 2018

Hello Krishna,

Raef has the right idea. You could either go fully with Explicit Dynamics. This discussion has some examples. More examples. Or you could make a thermal model possibly coupled with a structural model.

ANSYS also has a wear model.

  • Liked by
  • Krishna
Krishna posted this 08 April 2018

Thank you Peter, i will try it with your idea and come back to you. Thank you again.


Krishna posted this 11 April 2018

Hi Peter,

              After a long time. I have start the project and facing some problem in this. First i want to inform you about the size of model which I used.

Work piece - 10 x 10 x 3 mm

Drill - Dia 6 mm, length 5 mm

Queries: 1. Its take long time why?

               2. How I have use a Drill material HSS-M35  ( In Ansys any equivalent material of this category)

               3. in solution which option best for the material removal, temperature generated and tool life.

Thank You

peteroznewman posted this 11 April 2018

Hi Krishna,

Explicit dynamics takes a long time because the solver is based on explicit dynamics equations that require time steps short enough to track a wave passing through an element. The speed of sound in the material depends on its modulus and density. The time to traverse an element depends on its size. If you have small elements, that will cause small time steps.

You can create your own material or use a similar material from the library.

Your tool will create chips that will fly away from the workpiece and remove themselves. Some of the elements will experience "death" when the material failure criteria is exceeded.

If you want to attach a project archive .wbpz file to your post, I will take a look at your mesh.

Krishna posted this 12 April 2018

Thanks peter,

                        I will send you a project file after some time.

Krishna posted this 12 April 2018

Hi Peter,

             Please find the attached file. Can you help me.

Attached Files

Krishna posted this 12 April 2018

File extension not allowed error in attachment.

Krishna posted this 12 April 2018

please check its uploaded


peteroznewman posted this 12 April 2018

Okay, please reply with the version of ANSYS you are using 18.2 19.0 and if you are on Student license or other.

Krishna posted this 12 April 2018

18.2 I have

peteroznewman posted this 12 April 2018

Hi Krishna,

Changes to your model.

Pick a material from the Explicit Dynamics library instead of Aluminum Alloy, which has no Equation of State material model. I picked AL 1100-O.

Applied mesh controls to get smaller elements on workpiece.

Created a Cylindrical Coordinate System at center of drill.

Changed Velocity to use Cylindrical Coordinate System. Now Y velocity is in rad/s. (rotation speed 6000 rpm) Applied to Face, not Body. That will be 10 turns in 0.1 seconds.

Deleted Fixed Support., Changed Displacement to move workpiece toward rotating tool, 5 mm in 0.1 seconds.

Analysis Settings. Erosion Controls, change to On Material Failure, Yes. Output Controls, Result Number of Points, 2000.

Just started it running on 8 cores and it predicts 16.8 hours of run time, but it will take longer once the erosion starts.

Attached Files

peteroznewman posted this 12 April 2018

Hi Krishna, so after about 4 hours, this is the message:

Cycle:  1986450, Time:  1.567E-02s, Time Inc.: 6.710E-10s, Progress:  19.00%, Est. Clock Time Remaining:   19.2 hrs


EXECUTION FROM CYCLE        1 TO  1986450
ELAPSED RUN TIME IN SOLVER =      2.25981E+02 Minutes
TOTAL ELAPSED RUN TIME     =      2.70184E+02 Minutes

Problem terminated .... energy error too large
Problem terminated .... energy error too large


The energy error is set in Analysis settings, but I believe the corrective action is to use smaller elements in the workpiece, which will require even longer run times. Notice that the initial estimate of 16.8 hours increased to 19.2 hours as the drill engaged the workpiece.

I made up the rotational speed and the plunge speed. What values do you want?  It might go better with a faster plunge.




The new mesh has 3 times more elements in each direction in the workpiece and the plunge speed is 10 times faster.

The estimate for this model is it will run for 36 hours on 8 cores.  Maybe it will finish by the weekend.
I was going to cut down the size of the workpiece, but you didn't include the geometry files.

If you want to discuss drilling further, please start a new discussion because this one is marked as Solved.

Attached Files

Krishna posted this 13 April 2018

thank you so much


Krishna posted this 13 April 2018

If I have any queries I will ask you


Mohamed123 posted this 07 December 2018

Dear Friends,

I'm working on a research project where i want to simulate the drilling operation with oil lubrication using Ansys Explicit.

my problem is how to introduce the oil lubrication in the model.


Can any one help me with this issue?

Thank you very much.

peteroznewman posted this 10 December 2018

Mohamed123, please copy the text and open a New Discussion, since you will get email updates when people post to your discussion (if you choose that option). You don't get that when you use some else's discussion. After you have posted a New Discussion, come back to this one and delete your post (and I will delete mine).

felixsuperchao posted this yesterday

Hi peter, sorry for interupt but I am currently doing a drilling simulation using explicit dynamics, however I am struggling to find the thrust force of the drill. I tried to use the contact force solution type and selected the drill within the y direction( which is the direction of the thrust force) however it seems like my results didn’t appear to be right. Do you think I use the right solution type? Thank you so much. Have a nice day