May 21, 2020 at 5:38 pmLuanaSubscriber
My question is is there any option to give a maximum limit in the displacement tool?
I use ansys workbench 19.1 and run an analysis for a truss. I applied constant force at the purlins. I also want to apply increasing thermal condition, and observe the effect of the degradation of the Yield strength and Young's modulus. I use line elements edited in spaceclaim.
When it reaches the plasticity, I have convergence issues, and the calculation stops. At the partial results do not shows the results grafically, just the some of the tabular datas.
I want to control the maximum displacement, because of the convergence issues. Is there any options to give a maximum displacement of the nods while I use constant tabular force in the nods of a truss, while I increase the thermal condition in 30 steps?
I have already tried the displacement tool, but my problem is I do not want do give the BC in a certain displacement, I want to use the Force tool, I just want to avoid the convergence issues when the displacement jump from 20mm to 20000mm suddenly.
(I have already tried finer mesh, and increase the Initial and maximum substeps)
Thank you in advance.
May 21, 2020 at 6:46 pmpeteroznewmanSubscriber
As you can see, it is much better for convergence to use a Displacement than a Force boundary condition. Why don't you want to use Displacement? You can recover the Force using a Reaction Force Probe in the results to show how much force was applied at each increment of displacement.
May 21, 2020 at 7:17 pmLuanaSubscriber
Thanks for your fast reply. I want to use the Force tool, because the displacement is changing in every steps. The force is the constant during the whole analysis. I increase the thermal condition. At first, the the truss start to expand in every direction because of the thermal expansion --> the deflection decrease
After when the the temperature of the steel reach 500°C-600°C, the yield strength and the Young modulus start to degrade in the function of the temperature
--> so the deflection start to increase again. The temperature changes I want to use: 20°C-700°C
So the displacement is changing in every steps. And this is what I want to observe, how does it changes, and that is why I don't want to give it as a BC.
But here is my problem, I have no limit in displacement as a solution, so it stops, give me error messages, and get an amorf truss with 2000mm deflection.
But it would be OK, if I could get the partial results, but it do not show anything just stops. I have already did the same analysis, where I had the partial results I could use, and I wanted to do it again with the same truss, same modell, same force, just with different temperature, but now it doesn't work.
Can it cause a problem that I saved the original modell in an other file?
May 21, 2020 at 8:51 pmpeteroznewmanSubscriber
Turn on Auto Time Stepping. Set the Initial, Minimum Substeps to 100, Maximum to 200.
Turn on Large Deflection.
Do you get some partial results now?
It would help if you inserted some images to explain what you have.
May 21, 2020 at 9:51 pmLuanaSubscriber
The large deflection and the auto Time stepping was already on, I used them in this way at the previous analysis as well. Before I writote here, the minimum substeps was 40 and the maximum was 500. Now I run again, Now I have partial results, but just tabular data, and it do not show grafically on the truss.
I use this material: Structural steel NL from the data base, /Bilinear/ comleted with the following
And here is my truss with the constant force and the thermal condition:
The Displacement B is free at direction X
The displacement C is in all vertex where the forces are, and free to X and Z direction, and ramped in Y direction, perpendicular to the plain of the truss
Here is the Thermal condition of the steel, I added it in 30 steps, till 1800 sec=30min
May 21, 2020 at 10:07 pmLuanaSubscriber
I forgot to mention that I also applied initial imperfection with the eigenvalue buckling.
The truss is 10m long, 1,8m high, and the mesh in the line body is 1mm
And here are my results:
Do not show any of them grafically
Directional deformation tabular data in X axis are comlpetely missing:
But I have the tabular data in Total deformation, Directional deformation in Y and Z, and the beam tool-stress results. Unfortunately despite the fact I have these tabular data, it do not shown grafically in any steps.
And here are the last tabular results of the Y displacement.
Although the analysis is 1800 sec, it stops at 1440, sec, and that is what I exactly wanted. The temperature is the highest at this point, and I used the punctual force when the buckling happen in this temperature. I calculated it in MathCad, and it fits.
So know my only problem, that I can't see more results between 1435,6 and 1440, and I can't see the tabular results grafically, and the directional deformation in X neither.
May 22, 2020 at 3:16 amMahesh11Subscriber
In static analysis, if you are trying force driven boundary condition. Most of the time you will face this issues.
If you want solution with same boundary condition try in Transient analysis. It will work but don't forgot to off the time integration.
May 22, 2020 at 6:59 amLuanaSubscriber
It absolutely work, thank you for help, it saved my life This was a really good advice
Here are my results:
And the displacement in Y direction in the function of the temperature:
I guess it is an acceptable partial result, the calculation stopped at 1440 sec, and the buckling occur at 1440 sec, when the temperature is the highest, as I wanted.
- 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.
- Colors and Mesh Display
- User manual
- material damping and modal analysis
© 2023 Copyright ANSYS, Inc. All rights reserved.