March 12, 2021 at 9:08 pmDevarshSubscriber
I am am running a structural simulation which imports temperature data from a thermal simulation. The geometry is just a cylinder of 15mm (dia) x 5mm (height) (no contact surfaces or gaps or hollow spaces) which is being cooled to -150 C and warmed back to room temperature. The whole simulation is for 10000s. The material has temperature dependent specific heat, viscosity and creep constant 1 for time hardening model. Other properties are constant (I am unable to upload the zip folder for the Ansys project file due to upload size limitations.)
Mesh: The mesh has hex elements of 1mm size. The mesh was generated using GUI for both thermal and structural simulations. There are 3366 elements and 15520 nodes.
Information on PC: I am using Desktop having 40GB RAM and 8 cores intel i-7 processor. The ANSYS 2020R2 is installed on HDD drive of the PC (Windows 10 OS is installed on SSD).
Little bit about the problem: I am trying to find out the stress in a liquid which is cooled from room temperature to very low temperature. As the temp drops, the viscosity increases exponentially and the liquid vitrifies, behaving like an elastic solid. This behavior is called Maxwell fluid model and is simulated using creep strain, where the creep constant depends on the viscosity only. After cooling, as the material is rewarmed, stresses buildup, which I need to find out.
The thermal simulation is performed using Transient thermal module and it takes 2-3 min max. The results are linked to the transient structural module. For structural simulation, there is no external force - thermal load is the only load. I am using load-steps of 10s time with minimum time step of 0.1s.
The structural simulation is very very slow - In more than 36 hours, it solved only 14%. This looks insanely slow for such a simple geometry and relatively coarse mesh. I have used all 8 cores but no improvement on simulation time. The mesh size and time step size were initially kept high, but they caused convergence issues, so were reduced. There is no convergence related error now.
My questions: 1) How can I increase the simulation speed? I believed 40GB RAM and 8cores were more than sufficient. (Only ~10GB RAM is used during simulation).
- IS there any issue with the problem setup (mesh type, size or time settings) which is causing the low speed? If so, what can I change? How can I identify the bottleneck here?
- I understand that being a cylinder, it makes more sense to change the problem into 2D axisymmetric problem. I am running a 3D simulation because, this one is just a trial. Once I get results on this geometry, I will be adding more components in the geometry which cannot be solved using axisymmetry.
- I have run 2D axisymmetric simulations for this problem and got the results in 5-10 min. I want to see if the 3D simulations also give me the same results, based on which I will add more components in the geometry.
2) Will it help if I install the ANSYS on SSD instead of HDD? I installed it on HDD as SSD has limited storage space.
I appreciate your help.
P.S.- I am not very conversant with ANSYS, I started using it only last year.March 13, 2021 at 12:26 amDevarshSubscriberHere is attached the .wbpz file for the problem. Due to size limitation, mesh and solution data for both thermal and structural modules has been cleared.nnMarch 15, 2021 at 11:25 ampeteroznewmanSubscriberMarch 15, 2021 at 3:33 pmDevarshSubscriberHello PeternThank you very much. With my PC configuration and ANSYS research version, it solved within 8.5 minutes!nI have some questions about the changes that you made, though.nWhen I solved the 2D axisymmetric problem for similar geometry (different dimensions), I didn't use any boundary condition (weak springs were also off) and still got the results. Why the same settings didn't work for 3D geometry without adding remote displacement?nWhen I kept max time step size of 25s, it never used that value for time increment, it was always less than 10 sec. I am not sure why it took unto 100s for the changes you made. nWhat is the difference between remote displacement and displacement boundary condition? How can I understand when and where to add remote displacement? As I mentioned that this was just a trial simulation and I will be adding more components in the geometry, I need to understand how the remote displacement works.nFor creep settings, I had learnt that the first load step has to be very very small (~0.000001s) with creep analysis off. Creep analysis needs to be turned on at 2nd load step. Only this way I got results for the 2D axisymmetric model, and it was working for 3D as well (no error related to creep limit ratio), but you have not used the same method. Why is that? (I have attached the .wbpz file of 2D simulation just for reference, in case if needed)nAdding constraint does help the simulation run time, so I had tried fixed support on one edge, which did not work. I also tried frictionless support on the cylindrical surface since I am simulating a fluid, which solved within a few minutes. However, the results were very very different and incorrect. So, in a simulation that is not common structural problem and has no external forces, how can I identify where and what boundary condition do I need.nThe solution you have provided has certainly made my life easier now, but I need to understand why this works.nOne question I have is related to meshing. I have observed that for cylindrical geometry, when I meshed using CFD as physics preference in Mechanical module, the solution speed almost doubled. When I was performing thermal simulation on a cylindrical geometry with more components and contact regions, I used to get errors when used Mechanical as solver preference, but nothing when I changed it to CFD. I was just curious why did this happen.nThank you for your timely help.nnMarch 15, 2021 at 10:16 pmpeteroznewmanSubscribern1. Axisymmetric geometry comes with built-in boundary conditions. There is really only 1 DOF and that is the axial direction, while a body in 3D has 6 DOF.n2. In 3D, with 6 DOF of rigid body motion, the time increment was less than 10 sec because the model was unstable. With one Remote Displacement there are 0 DOF so the stable model allows 100s time increments.n3. What is the difference between remote displacement and displacement boundary condition? Displacement is an essential BC. That value is assigned to that node, no matter what. A deformable Remote Displacement is scoped to several or many nodes and the average motion of those nodes can be controlled to be zero at the Pilot node, which is a new node created at the center of the nodes. That allows a circle of nodes to freely expand or contract during temperature changes.n4. In a Static Structural analysis, loads are ramped on over the duration of the time step. If you want to evaluate creep due to a constant load over 10000 s, you need step 1 to ramp on the load in 1 s with creep off, then turn creep on for step 2. If you have only 1 step, the load is ramping on for 10000 s, which is not what you want. n5. A fixed support on one edge will not work because it prevents free expansion and causes element distortion and artificially high stress. Frictionless support on the cylindrical surface also gives incorrect results because it prevents free expansion of the body.nTo run a Static Structural analysis on a body with no external forces and no constraints, there are three methods that work.n1. Remote Displacement with all 6 DOF set to zero with Deformable behavior.n2. A kinematic mount. That means hold 3 vertices using exactly 6 constraints. There are several valid arrangements. One is called 3-2-1. That means set a zero displacement in X, Y and Z on a first vertex. Set a zero displacement in Y and Z on a second vertex, spaced in X from the first one. Then set a zero displacement in Z on a third vertex, spaced in Y from the first one.n3. Turn on Inertia Relief. Look it up in the ANSYS Help.nThe default mesh for structural models is quadratic elements, which means each element edge has an extra mid-side node. The default mesh for CFD models is linear elements, which has no mid-side node. The reduction in node count can be nearly a factor of two.nViewing 4 reply threads
Ansys Innovation Space
- You must be logged in to reply to this topic.
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.Trending discussions
- Saving & sharing of Working project files in .wbpz format
- An Unknown error occurred during solution. Check the Solver Output…..
- Understanding Force Convergence Solution Output
- Solver Pivot Warning in Beam Element Model
- How to calculate the residual stress on a coating by Vickers indentation?
- Colors and Mesh Display
- whether have the difference between using contact and target bodies
- What is the difference between bonded contact region and fixed joint
- The solver engine was unable to converge on a solution for the nonlinear problem as constrained.
- User manual
Top Rated Tags
© 2023 Copyright ANSYS, Inc. All rights reserved.Ansys does not support the usage of unauthorized Ansys software. Please visit www.ansys.com to obtain an official distribution.