March 20, 2020 at 4:59 pmLivinSubscriber
Dear Ansys Community
I'm currently working on my Bachelor Thesis regarding the distortion of a local heat treatment on a component. One of the aims of my Bachelor Thesis is to understand this kind of distortion with a finite element simulation with ANSYS workbench 2019 R2.
For this reason, I want to simulate in a simple test-case how the temperature- and stress field propagates. First of all I want to understand the boundary conditions in a steady state thermal analysis connected to a structural analysis. How does the stress increase due to a local heating? See attached Picture for the thermal conditions. (Sheet metal dimensions 500x800x1.27mm)
I want to simulate how does a simple structure like that behave under these circumstances.
Heat flux in the middle of the plate to increase the temperature to around 760°C. Free convection of the whole body.
To calculate the stress and strains I have to define the boundary conditions in the structural analysis.
In an experimental setup I would like to lay this plate on the floor without clamping and heat it in the middle to about 760°C. Because of the local heat input and the non-symmetrical geometry, elastic/plastic stresses and deformations build up. How can I reproduce this free support on the floor in a digital environment? I tried it with remote displacement but i'm not sure if this is the right approach. I expected a symmetrical deformation.
March 21, 2020 at 5:18 pmpeteroznewmanSubscriber
This Static Structural model is held by a Remote Displacement at a single vertex at the center.
Try to use smaller elements and try to increment the nonlinear solution more gradually and you can obtain a solution where the plate remains flat.
If you want the temperature load to "potato chip" the sheet, then you need to provide a geometric imperfection or an initial load to bend the part out of plane.
March 21, 2020 at 11:50 pmLivinSubscriber
Thank you for your tip of the vertex BC, it gave me some realistic results:
Load: Heat flux and free convection in addition with earth gravity
BC: Remote displacement on the vertex in the middle + displacement of sheet locked in z-direction due to the gravity.
To achieve the "potato chip" deformation, how should I definie an initial load? I tried it with a point load on the vertex in the middle, same result as above. Or do you mean with the step controls?
I want to depict the real experiment as close as possible. Heating pad on top of the sheetmetal which lays unclamped (free) on the floor -> therefore I guess there will be no "potato chip" deformation. Just an in-plane deformation as shown above.
March 22, 2020 at 1:46 ampeteroznewmanSubscriber
I made a model and used a single vertex that was fixed because it would solve relatively quickly. In that model, if I wanted to induce a "potato chip" deformation, I would use a two step solution, and in step 1, I would put a small force on the ends of the sheet to bow it slightly. This can ramp up as the temperature ramps up. Then in Step 2, the force is ramped down to zero. It might turn out that the sheet remains bowed.
You can create a model where there is a larger surface, let's call it the floor, that is in the same plane as the sheet body that gets the thermal load. The floor would be configured as a Rigid body. You need a Fixed Joint to Ground to hold the floor. You then create a frictional contact between the sheet and the floor. The floor has to be the Target side of the contact pair. You add Standard Earth Gravity to hold the sheet to the floor. The frictional contact will greatly slow down the solution progress.
If you further want to put a heating pad on top of the sheetmetal, that slows the whole process down even further. There will be a lot of struggle to obtain convergence.
Some of that can be alleviated if you do a 1/4 model, and enforce a symmetric deformed shape.
- 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.