December 18, 2019 at 11:43 amAGATHIYANSUSILRSubscriber
I am trying to simulate orthogonal cutting process in ansys workbench using explicit dynamics. i have used johnson cook model and other physical properties for the tool and workpiece. Workpiece dimensions are 10*4*3 mm and tool has 5 deg rake and clearance angle. I have made both tool and workpiece flexible with lagrangian approach. Tool and workpiece materials and its properties are taken from a science article. Mesh was body sized with element size of 0.1mm.tool and workpiece is modeled in solidworks with fixing depth of cut to 1mm
In explicit settings:
fixed support- 2 faces of workpiece of other side (bottom and left side face)
displacement- displacement was given to tool (8mm) towards the workpiece and keeping the workpiece stationary.
analysis settings - end time is given as 0.001 sec
The problem i face here is that it says the time step is too small so the result is not obtained.
i wanted to calculate the stress and temperature from this simulation
can someone please help me with this (i have attached some of the screen shots)
i coudnt capture the error message but it says ('Time step is too small')
i have also included friction co-efficient of 0.2
December 18, 2019 at 6:57 pmAGATHIYANSUSILRSubscriber
CAN SOMEONE PLEASE HELP ME WITH THAT PROBLEM STATED ABOVE?
December 22, 2019 at 5:55 pmAGATHIYANSUSILRSubscriber
@peteroznewman sir u have blocked my duplicate discussion, i posted that because of curiosity of getting my doubts cleared early. Sorry for that!!
Can u please go through this discussion and help me out!!
Thanks in advance
December 22, 2019 at 8:09 pmpeteroznewmanSubscriber
Posting duplicate discussions can result in two people answering the same question in two different discussions. That is considered a waste of time.
I see from your image attachment that you have left the Minimum Time Step Program Controlled.
Please try entering a value instead of leaving the decision up to the solver.
December 22, 2019 at 8:23 pmAGATHIYANSUSILRSubscriber
Yes Peter sir i have also tried giving 1/10 th of end time as the minimum time step, still the issue is same. How much does the mesh size affect the time step?
And for explicit dynamics is automated mesh with body sizing is enough or anything specific like multizone and sweep should be used?
because in the article i follow they have used some different mesh.
here is a snap of it (see the mesh near the contact)
December 22, 2019 at 8:52 pm
December 22, 2019 at 11:18 pmpeteroznewmanSubscriber
Are you solving a 2D model?
Under Analysis Settings, Output Controls, what did you set the Result Number of Points? It should be 200 or 2000.
If you increase the density by a factor of 100 or 1000 you can get a cartoon like the one below in much less time.
The minimum element size controls the time step. Try to keep all the elements the same size.
December 23, 2019 at 5:31 amAGATHIYANSUSILRSubscriber
Yes Peter sir!!
I am solving a 3D model of same thing simulated in the video.
Sir my input velocity is 10m/s (to the cutting tool) which is actually less but that is the practical one.
now i have changed the points to 2000 and ON the material failure in Erosion controls (as i have given failure criterion to the workpiece (johnson cook failure criteria))
And sir what is that "NO CELL CONTAINING TIME STEP" means (this snap is put in my previous post)
December 23, 2019 at 1:08 pmpeteroznewmanSubscriber
Set the units to mm.
Use CAD to move the tool so it is just touching the workpiece at the vertex. You are not interested in simulating the tool approach the workpiece at a constant velocity.
Does the tool have a Velocity that is equal 10 m/s under the Initial Conditions as well as a Boundary Condition of Velocity?
Delete the Displacement constraint. You only need a Velocity Boundary Condition if it controls X, Y and Z on the top face.
What material did you use for the workpiece and tool?
December 23, 2019 at 2:54 pm
December 23, 2019 at 2:57 pm
December 23, 2019 at 8:57 pmpeteroznewmanSubscriber
Mechanical automatically creates contacts to be "helpful". Delete them. You don't want them.
You have not put an Initial Condition for the velocity of the tool in the model. You only have a velocity Boundary Condition. They are different. Right mouse click on the Initial Conditions folder, Insert Velocity, then pick the tool and enter the data. You will get a velocity initial condition under the folder.
Please show the Engineering Data for your Workpiece material. I want to see the where you included the Johnson-Cook material model.
December 24, 2019 at 3:40 am
December 24, 2019 at 3:44 am
December 24, 2019 at 12:53 pmpeteroznewmanSubscriber
I don't know what NO CELL CONTAINING TIME STEP means exactly, there is no reference in the ANSYS Help. The explicit solver must compute a stable time step for the solution to proceed and if it can't do that, I suppose this is the kind of error it might report.
I don't work for ANSYS and I don't use Explicit Dynamics, I have just played with it a few times. Search this site to find a member who has posted a question about Explicit Dynamics or AutoDYN and ask them for help. You can try things to look for what might change the outcome. I don't know what will help. At this point I am guessing.
It is odd that a large rectangular block was removed. What is the element size? Is that two elements that disappeared or 200?
Try changing to one of the Explicit Materials predefined in Engineering Data. These are known good material models.
One thing that helped my play models run more smoothly was to ramp up the velocity from zero. That reduced the shock waves that bounced around inside the material. You do that by typing an expression such as 100*time then after 0.1 seconds, it will be going at 10 m/s if the units were set to m. If you do this, then delete the Initial Condition of velocity.
Finally, you are using an old version of ANSYS, 15.0. If you attach your Archive .wbpz file, I will try running your model in the latest version of ANSYS and let you know if it runs any better.
December 25, 2019 at 10:09 amAGATHIYANSUSILRSubscriber
Hello peter sir !!
i am not able to upload the wbpz file here as it only accepts the link and images
so can u please send a blank mail to email@example.com , so that i can send it to you and help me
I am also raising this question in other forums but not getting any reply from anyone, thank god atleast you looked it over.
PLease send me a blank mail to the above mentioned and i will share you the files as i am not ale to share here
And yes the element your mentioning about is workpiece size ? its 10*4*3 mm of dimensions with 0.1mm mesh size
Thank you sir
December 25, 2019 at 5:49 pmpeteroznewmanSubscriber
In Workbench, right mouse click on Model and Clear Generated Data. That will delete the mesh. Then do File, Save, then do File, Archive... don't include Results. Then the size of the .wbpz file will be < 120 MB and you can Upload that file to your reply. It is working fine today.
December 25, 2019 at 6:13 pmAGATHIYANSUSILRSubscriber
Sir here it says file extension is not allowed for the wbpj file nor the .rar file, so finding difficult to upload, but i have uploaded the tool IGES file
December 25, 2019 at 6:21 pmAGATHIYANSUSILRSubscriber
This is the link for the files Peter sir. Kindly let me know whether anything more than this is required for the simulation
Sir this is the link for the science article that i am referring for this simulation
Thanks in advance
December 25, 2019 at 8:20 pmpeteroznewmanSubscriber
I think I have said these things before...
1) Attach a .wbpz file not a .wbpj file.
2) Delete the displacement boundary condition.
3) Delete the contacts.
4) Is this the mesh you tried to compute with? It is too coarse.
5) Use 2000 Result Number of Files, you had 20.
6) Don't use Minimum Time Step = Program Controlled. I used 1e-9. Use an Initial Time Step of 1e-8.
7) The Velocity BC should be on the top face of the tool, not the whole body.
I changed the wp material to AL 7039 from the Explicit Dynamics material library, which uses Johnson-Cook and Shock EOS Linear. I changed the Fixed Support to be on the bottom face only. Here are the Erosion Controls I used.
I increased the density of the two materials by a factor of 100 to reduce computation time to make a cartoon in a few minutes. You will have to let the simulation run for hours at a normal density to get physically accurate results.
I believe your material model for wp is inadequate or incorrect. The cells around the contact point just erode away immediately as you have shown above then it gives the no cell controlling time step error after just 14 cycles.
I can't help you with material models for Explicit Dynamics.
December 26, 2019 at 4:25 amAGATHIYANSUSILRSubscriber
Yes peter sir !!
sorry that i misread your last post and sent you the wrong extension file, here i have attached the .wpbz file.
Actually sir why i was changing the mesh and was looking how the time step varies each case, and one such case was the coarse one that you pointed out, and that wasnt the mesh i wanted to implement, but just was checking it
Okay sir i will look into the material models no problem, But the simulation you obtained had the following?
1) Velocity is 10m/sec (tool) ?
2) you included friction body interaction between the tool and workpiece?
3) And what was your mesh size ? (it looks like 0.1mm)
4) Did you keep both tool and workpiece flexible ? or tool rigid and workpiece flexible?
5) Mainly what was the endtime did you provide?
6) Did you have intial condtions for the tool too along with the boundary condition?
7) Also i hope you used the same CAD model i sent you in that link ? (or any changes in the dimensions of the tool or workpiece)
Did you also change the tool material?
I understood your explanation si (about the erosion controls) I am right now simulating it, i will soon post my results if at all i get it
And By increasing the density by factor of 100, you meant about the number of points in the result? or changing the density of materials in the engineering data directly?
And sir please clear these things that i have mentioned, dont think i am pestering you just my curiosity towards learning these
THANKS A LOT SIR
December 26, 2019 at 11:31 ampeteroznewmanSubscriber
1) Velocity is 10m/sec (tool) ? Yes.
2) you included friction body interaction between the tool and workpiece? Yes.
3) And what was your mesh size ? (it looks like 0.1mm) 0.125 mm
4) Did you keep both tool and workpiece flexible ? or tool rigid and workpiece flexible? Both flexible.
5) Mainly what was the endtime did you provide? Unchanged at 0.001 s.
6) Did you have initial conditions for the tool? Initial conditions unchanged at 10 m/s. But I changed the Boundary Condition from the whole body to just the top face of the tool. I also changed the Fixed Support to be just the bottom face of the wp.
7) Also i hope you used the same CAD model i sent you in that link ? Unchanged CAD.
Did you also change the tool material?. No.
To make the simulation solve faster, in Engineering Data, I put two extra zeros on the density of the tool and the AL material. Try putting three zeros and it goes even faster, but it is for making cartoons because it is no longer the same physics. High density material has more inertia than the real material so it moves differently, but it can be helpful to see if things are going to work before you spend an hour (or many hours) waiting to see with the real density of material.
December 26, 2019 at 7:37 pm
December 26, 2019 at 7:42 pmAGATHIYANSUSILRSubscriber
And Peter sir !!
Is there any reason why did you use 1e-8 sec for intial time step and 1e-9 sec for minimum time step (because my actual end time will be 0.1 sec so like is there any specific ratio that describes these values)
If yes then what are the factors that affect this ratio , so that if we play with the factors accordingly the result may vary or be constant with the ratio ?
December 26, 2019 at 9:09 pmpeteroznewmanSubscriber
At higher material density, that error does not occur for the time increments above. When I ran the model at normal density, I had to reduce the minimum time step to 1e-10 then it ran to the end time of 0.001 s.
I choose 1e-8 because the first few time steps before it failed were on the order of 1e-7 s.
December 28, 2019 at 6:30 pmAGATHIYANSUSILRSubscriber
Okay Peter sir i understood the methodology of giving the time step !!
SINCERE THANKS FOR SPENDING TIME FOR ME AND HELPING ME OUT, YOUR GENEIUS
Hope i will also get my future doubts cleared from you here in forum if at all any in ansys workbench
ONCE AGAIN THANK YOU
May 11, 2020 at 6:44 ameedegouthamSubscriber
I have gone through your steps in this conversation. I am trying to perform impact analysis on lattice structure. I am having difficulty solving my problem.
When I use the default default time step and same mesh size (for both impact and impact absorbent material as 0.1 mm), kinetic energy started to decrease and internal energy started to increase and got error an error immediately as- time step too small.
I have modified the following:
I have selected end time as 0.001 s.
Meshing size 0.2 mm for lattice structure and 1 mm for impact material.
Minimum time step as 1e-10 s and maximum as 555,556 s.
Now I got the following graph, please help me.
- You must be logged in to reply to this topic.
Boost Ansys Fluent Simulations with AWS
Computational Fluid Dynamics (CFD) helps engineers design products in which the flow of fluid components is a significant challenge. These different use cases often require large complex models to solve on a traditional workstation. Click here to join this event to learn how to leverage Ansys Fluids on the cloud, thanks to Ansys Gateway powered by AWS.
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.
- Solver Pivot Warning in Beam Element Model
- Saving & sharing of Working project files in .wbpz format
- Understanding Force Convergence Solution Output
- An Unknown error occurred during solution. Check the Solver Output…..
- What is the difference between bonded contact region and fixed joint
- User manual
- The solver engine was unable to converge on a solution for the nonlinear problem as constrained.
- whether have the difference between using contact and target bodies
- material damping and modal analysis
- Colors and Mesh Display
© 2023 Copyright ANSYS, Inc. All rights reserved.