April 7, 2018 at 4:46 amKrishnaSubscriberHi 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
April 7, 2018 at 11:07 amRaef.KobeissiSubscriber
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?
April 7, 2018 at 1:10 pm
April 8, 2018 at 4:31 amKrishnaSubscriber
Thank you Peter, i will try it with your idea and come back to you. Thank you again.
April 11, 2018 at 7:54 pmKrishnaSubscriber
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.
April 11, 2018 at 10:45 pmpeteroznewmanSubscriber
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.
April 12, 2018 at 1:18 amKrishnaSubscriber
I will send you a project file after some time.
April 12, 2018 at 2:21 amKrishnaSubscriber
Please find the attached file. Can you help me.
April 12, 2018 at 2:30 amKrishnaSubscriber
File extension not allowed error in attachment.
April 12, 2018 at 2:34 amKrishnaSubscriber
please check its uploaded
April 12, 2018 at 4:06 ampeteroznewmanSubscriber
Okay, please reply with the version of ANSYS you are using 18.2 19.0 and if you are on Student license or other.
April 12, 2018 at 8:11 amKrishnaSubscriber
18.2 I have
April 12, 2018 at 11:21 ampeteroznewmanSubscriber
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.
April 12, 2018 at 4:18 pmpeteroznewmanSubscriber
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
SIMULATION ELAPSED TIME SUMMARY
EXECUTION FROM CYCLE 1 TO 1986450
ELAPSED RUN TIME IN SOLVER = 2.25981E+02 Minutes
TOTAL ELAPSED RUN TIME = 2.70184E+02 Minutes
JOB RAN OVER 8 SLAVES
JOB RAN USING IBM MPI
JOB RAN USING DECOMPOSITION AUTO
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.
April 13, 2018 at 11:26 amKrishnaSubscriber
thank you so much
April 13, 2018 at 11:27 amKrishnaSubscriber
If I have any queries I will ask you
December 7, 2018 at 11:33 pmMohamed123Subscriber
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.
December 10, 2018 at 5:21 pmpeteroznewmanSubscriber
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).
March 21, 2019 at 8:55 amfelixsuperchaoSubscriber
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
October 28, 2020 at 8:41 amMAMIN219Subscriberdid you get thrust force? n
- You must be logged in to reply to this topic.
Simulation World 2022
Check out more than 70 different sessions now available on demand. Get inspired as you hear from visionary companies, leading researchers and educators from around the globe on a variety of topics from life-saving improvements in healthcare, to bold new realities of space travel. Take a leap of certainty and check out a session today here.
Earth Rescue – An Ansys Online Series
The climate crisis is here. But so is the human ingenuity to fight it. Earth Rescue reveals what visionary companies are doing today to engineer radical new ideas in the fight against climate change. Click here to watch the first episode.
Subscribe to the Ansys Blog to get great new content about the power of simulation delivered right to your email on a weekly basis. With content from Ansys experts, partners and customers you will learn about product development advances, thought leadership and trends and tips to better use Ansys tools. Sign up here.
- How to calculate the residual stress on a coating by Vickers indentation?
- An Unknown error occurred during solution. Check the Solver Output…..
- Saving & sharing of Working project files in .wbpz format
- Solver Pivot Warning in Beam Element Model
- Understanding Force Convergence Solution Output
- whether have the difference between using contact and target bodies
- Colors and Mesh Display
- The solver engine was unable to converge on a solution for the nonlinear problem as constrained.
- Massive amount of memory (RAM) required for solve
- What is the difference between bonded contact region and fixed joint
© 2022 Copyright ANSYS, Inc. All rights reserved.