February 9, 2022 at 3:18 pmphanicmsfSubscriber
What doe the error messages mean in ansys solution information.?
I am able to solve the problem setup using Structural steel material for both geometries. But when I applied different materials Sic_Pores and Sic_Sic for each geometry I got the fallowing error.February 9, 2022 at 9:17 pmpeteroznewmanSubscriberIt looks like you are simulating the thermal strain created by cooling down a composite material from 1326 C to 20 C.
I assume the two materials have zero thermal strain at the beginning of the simulation, and the thermal strain develops as the materials cool down.
To accomplish that, you need to set the Environment temperature to 1326 C since that is the zero thermal strain temperature for all the bodies.
What you have done by leaving the Environment temperature at 20 C is that is the temperature where there is zero thermal strain, then in step 1, the temperature increases to 1326 C, causing massive amounts of thermal strain, which turns elements inside out.
Under Analysis Settings, turn on Large Deflection.
February 10, 2022 at 9:15 amphanicmsfSubscriberThank you for your explanation.
Does the 'Zero-Thermal-Strain Reference Temperature' in the Engineering data of the material and the 'Environment Temperature' in the menu detais of static structural should be same ?
Is it correct defining 'Zero-Thermal-Strain Reference Temperature' and'Environment Temperature' as 1326 ?
February 10, 2022 at 10:42 amphanicmsfSubscriber
a) SOLVING THE ANALYSIS WITHOUT APPLYING MECHANICAL LOADS. ONLY THERMAL CONDITIONS ARE APPLIED --> Cooling the body from 1326 to 20 C.
(After solving for the case a) After simulating the thermal strain created by cooling down a composite material from 1326 C to 20 C. I would like to apply mechanical loads
case :1 ) Compresive unit loads
case:2) Tensile unit loads
and want look for the stresses distribution.
b) Shall I need to apply mechanical loads in the same analysis where I specified Cooling Thermal conditions ? Shown in the tree below
Thermal condition---> has cooling curve with time
Displacement--> has symmetry zero displacements in each of respective plane.
Force ---> Unit load acting on each face of the outer cube (Compressive unit loads)
In this case the resulst I got is same like solving the analysis without mechanical loads.
When there are mechanical loads in addition to uniformly cooling two different materials having different CTE(as a function of temperature) the stresses I would expect should be higher then the stresses got in the simulation without mechanical loads.
Can anyone explain why I am getting the same results in both cases? Is there any mistake in model setup ?
February 10, 2022 at 1:32 pmpeteroznewmanSubscriberIs it correct defining 'Zero-Thermal-Strain Reference Temperature' and 'Environment Temperature' as 1326 ? Yes.
Run a model with no change in temperature and apply the mechanical load, what is the stress? Compare that stress with the stress from the temperature change. What is the ratio between the two stresses?
If the stress from mechanical load only is 1000000 times smaller than the thermal stress, and you only show 5 digits in the stress result, it will seem as if you get the same result in both cases.
To apply a mechanical load after the cool down, simply add another step, keep the temperature constant at 20 C and change the load from 0 in step 1 (or more) to the load value you want in the last step.
February 10, 2022 at 1:38 pmphanicmsfSubscriberThank you.
Viewing 5 reply threads
Ansys Innovation Space
- 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.Trending discussions
- 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
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.