July 1, 2020 at 3:10 pmDavid2020FEMSubscriber
Dear ANSYS community;
I am using dynamic explicit analysis for dental implant to simulate chewing so for static analysis it run easily but for the dynamic analysis i do know how to set the time step and I need some help. To make efficient I am applying oblique load at some angle on the crown of the implant system. I have used mESH METHOD OF TETRAHEDRON pATCH CONFORMING, PLEASE ADVICE ME TO RUN IT EFFICIENTLY!
THANK YOU SO MUCH PLEASE HAVE A LOOK THE ATTACHED PICTURE!
July 1, 2020 at 7:39 pmWenlongAnsys Employee
I couldn't see your image, please use this button to insert an image.
Leave the time step controls as program-controlled if you don't know how to define it. Regarding mesh, change the mesh to linear order instead quadratic in explicit dynamics.
The critical time step size will be proportional to the mass density, mesh size, and inversely proportional to Young's modulus. (Ref: https://www.dynasupport.com/tutorial/ls-dyna-users-guide/time-step-size) The time step in your simulation will need to be smaller than the critical time step. The solver will automatically calculate the time step for you so you don't need to worry about it. But the takeaway is your smallest mesh size controls the critical time step and determines how fast your model runs. So assign a relatively uniform mesh if possible.
Another way to improve the speed is to use "mass scaling", but that will be the next thing to try. Let's see your image first.
July 2, 2020 at 2:45 pmDavid2020FEMSubscriber
Thank you for your explanation but still need help yes I tried as you told me may be I missed some points for example I couldn't find the ctical time step undet analysis setting, perhaps you wanna say Initial time step, final time step under time step definition in the analysis setting. can you please see the attahed pictures. even the Kinetic energy is higher than the internal energy during analysis so I didn't see any convergence behaviour in the solution please suggest me techniques that will help me run my analysis in the most efficient way (i.e, also considering the final solution accuracy). Actually my current problem is even to see the program run succeful in this dynamic exlicit analysis.
glad to hear from you!
thanks a lot!
July 2, 2020 at 3:34 pmWenlongAnsys Employee
Thanks for your reply and the images. There are several things I'd like to point out:
1) In Explicit Dynamics, there is no convergence issue. Your model may become "unstable" but it can always converge at each time step since each time step is linear.
2) The fact that the kinetic energy is way higher than internal energy doesn't necessarily mean the simulation is inaccurate or "unstable". As you highlighted in your image, the current simulation time is 1e-4s, which is quite a short duration, and if a high load or displacement is ramped up during such a short period, high kinetic energy may not be surprising.
3) I see that the mesh between the tooth and the block is extremely fine, and this is highly undesired in explicit dynamics analysis. Do these two geometries have shared topology? If so please remove that in order to achieve a more uniform mesh. You can use a bonded body interaction to constrain these two parts together. This will help your model run much faster.
4) Regarding the time steps, yes there is no place to define the critical time step, and it is calculated by the solver in the back scene. You can leave all the settings of the time step as program-controlled.
5) I noticed in your image you have a contact region in your model. Please delete that and use body interaction in Explicit dynamics analysis because the formulation of body interaction is more suitable for explicit dynamics and more efficient.
6) In Analysis settings -> Output settings, you can request more results, so that you can view more output plots even if the solution cannot finish successfully. This is helpful to debug.
Feel free to follow up. I will probably take several iterations to make it run successfully but you will get there
July 2, 2020 at 11:39 pmDavid2020FEMSubscriber
I appreciated for your valuable explanation and time. I followed all your suggestions above and Run the ANSYS yesterday at mid night and go back home. when I returned still running like you see in the picture. I changed the Meshing from very fine to moderate fine. and also I canceled the contacts and left the body interaction and used Bonded instead of friction less which is the default. As well as I increased the End time by two digit I changed it to 5e-2 sec. But when I apply the load it is oblique load. 150N at 45 degree to the occlusal surface of the crown. I applied it on the YZ plane. I want the resolved body with time history.
For your information I have six components here by the way. Crown,Abutment,Screw, Implant, Trabecular Bone and Cortical Bone.
Please what I can do to solve this convergence problem.
Thank you so Much!
July 3, 2020 at 5:28 pmWenlongAnsys Employee
Thanks for sharing the images. If you click on Solution information, then in the details window at the lower left, change the solution output to "solver output", then what is the current time step size? What is the order of the magnitude?
If you plot the deformed shape, what is it like, does it have some crazy deformation?
July 3, 2020 at 6:12 pmDavid2020FEMSubscriber
Thank you so much? This is my PhD work and it really took me longer time can i share my ANSYS file so that you can see it and edit it accordingly. Please bro can you help this so important to me.
can you share me your email.
Thank you so much!
July 3, 2020 at 7:15 pmWenlongAnsys Employee
Sorry, but as I mentioned, Ansys employees are not permitted to take files from the student community. You may share it with other non-Ansys employees but the only way we can communicate is by describing the problem & result then provide suggestions.
Sorry about that.
July 4, 2020 at 9:36 amDavid2020FEMSubscriber
Oh! I understood I didn't know that before sorry. And I will follow your suggestion that is I will share my problem and challenges here and then we will discuss it further.
So as I mentioned before, I followed what ou suggested but why it is running very slow.
This is what I have improved
1. I deleted the contact and leave the body interaction
2. Make uniform mesh and avoid those densely meshed regions with acceptable mesh
3. Increased the time it was too small, I used now 0.5sec as end time
I have followed all your suggestions actually I see some important when it runs like the kinetic energy was decreasing and Internal energy increasing
but very slow.
I do have six assembled component here as i mentioned before.
Wenlong, can you suggest me further tricks to run this simulation and get successful.
Thank you so much!
July 4, 2020 at 3:31 pmWenlongAnsys Employee
Can you share the mesh details (the min size, and the total number of elements, like shown below)?
Also, what shown below can provide you valuable information about the Time increment, and the time remaining to run the simulation. Please attach an image of that as it is very important information to diagnose the model.
- 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.
- Saving & sharing of Working project files in .wbpz format
- Solver Pivot Warning in Beam Element Model
- 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
- whether have the difference between using contact and target bodies
- The solver engine was unable to converge on a solution for the nonlinear problem as constrained.
- User manual
- Colors and Mesh Display
- material damping and modal analysis
© 2023 Copyright ANSYS, Inc. All rights reserved.