TAGGED: ansysmechanical, mesh, mesh-size
April 9, 2023 at 6:22 amDmArcherSubscriber
I am doing a 3D thermal simulation with Ansys Mechanical. I noticed that the fineness of the mesh has some big effects on my model. I assume that the smaller the mesh is, the simulation result will be more close to the actual result. However, if I decrease the mesh size too much, I will get an error saying that the academic license does not support this many calculations (Or something similar to that. Basically, it is saying I cannot have this many grids to have this large amount of calculation under my current license.)
The thing I realized is that under Mesh -> Sizing, there is only Element Size that I could adjust the size of the mesh. And Ansys Mechanical is trying to have the mesh shape close to a cube, which means that the mesh length, width, and height are close to each other if possible. But in my case, my structure is kind of flat. So I actually only need the grid size on the height (z direction) to be small. However, by decreasing the value of Element Size, the gird scales on the x and y directions are also decreased which leads to lots of unnecessary nodes.
So I am wondering is there a way to decrease the mesh size by only decreasing the length of the grid in one direction, not every direction?
April 9, 2023 at 12:35 pmpeteroznewmanSubscriber
It would help to know the boundary conditions. I assume the heat transfer you are interested in is vertical. If the BCs on the four sides are identical and the loads on the top and bottom faces are symmetric, then you could slice the geometry with 2 planes and discard 3/4 of the geometry by applying a Symmetry BC on the cut faces. That will free up a lot of nodes! If the BC on the four sides is insulated and the top and bottom BCs are uniform across the face, this 3D problem collapses to a 1D problem and you only need one element in the plane!
I see that Bonded Contact is being used to connect the four layers together. If you don’t need Contact to add an extra thermal resistance, you would be better off using Shared Topology to have the elements on each side of the interface grab the same nodes. In SpaceClaim, on the Workbench tab, click the Share button. Then in Mechanical, delete all the contacts.
Once you have shared topology, all the layers will have the same element density in the plane. Add a Sizing mesh control and have the Geometry filter set to Edges. Pick the 4 vertical edges in one layer and set the control to Number of Elements. Repeat for the other three layers. Now you can control the number of elements in each layer.
April 9, 2023 at 2:35 pmDmArcherSubscriber
Yes, the heat transfer I am interested in are in all directions (x, y, z).
In Ansys Discovery, the modle looks like this:
Different colors represent different material, which means different thermal conductivity. Except the yellow and the red part are the same material but the red part does self heat generation.
I am not sure what you meant by 'BC'.
All different mateirals (lays) are contact tightly to each other. I am doing steady state themal simulation with Ansys Mechanical, which I believe is using Finite Element method to solve the problem. Therefore, thermal resistance is not typically involved. So I am not very sure what you meant. Will really appreciate if you could explain with more details. Also please correct me if I am wrong. I thought thermal resistance is used while the thermal model is approached through a way using thermal RC netowork.
April 9, 2023 at 3:13 pmpeteroznewmanSubscriber
BC means Boundary Condition, sorry I wasn't clear on that abbreviation.
Bonded contact can be used to represent thermal resistance at the surface without needing to explicitly make a body with a different material to represent that surface layer. For example, a layer of oxide on the surface of a metal that has a different thermal conductance than the parent metal. You can represent that layer in the Bonded Contact definition itself. If you don't need to do that then you are better off without any contact elements.
If you look top down on a wireframe of the assembly, are there any planes of symmetry in the geometry, materials, loads and BCs? If so, you can cut down the model size by using a Symmetry BC. If all those items are not symmetric then you need a full model.
Please describe the BCs on all faces of the model. If you don't define a BC on the face of the model, it is automatically considered to be insulated (zero heat flux).
April 9, 2023 at 7:25 pmDmArcherSubscriber
The boundary condition I have here is that all surfaces have the same temperature. So I was trying to see the teamperature difference inside the structure. Such as the temperature of a path that goes from bottom to top through the center of the self heat generation part Or the temperature distribution of a cross section that contain the cross section of the self heat generation part like shown in the images below.
April 9, 2023 at 8:22 pmpeteroznewmanSubscriber
There is one plane of symmetry you could use to cut the model size in half. It is the plane that cuts the image above in half with a horizontal line through the center of the heat generating block. The top half of that image is a mirror image of the bottom half of that image.
- 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.