October 7, 2018 at 4:39 pmNiranjanRameshSubscriberI been working on concrete filled steel tube. I want to get the ultimate load from the model, Is there any possibilities of doing that in ansys workbench?, kindly help me out. Thanks in advance.
October 7, 2018 at 8:44 pmpeteroznewmanSubscriber
You can predict the ultimate load of a concrete filled steel tube in ANSYS.
Please review this relevant discussion.
How is your steel tube loaded?
October 8, 2018 at 2:16 amNiranjanRameshSubscriberThank you Mr.Peter for your response, the model I've designed is a column with fixed support at the bottom and a compressive load on the top, with various eccentricity.
October 17, 2018 at 7:10 amNiranjanRameshSubscriber
i have attached my model with this, as i am new to ansys kindly ignore the mistakes if there is any. I been Ansys workbench 18.1 for the modelling, Please respond. Thank You
October 18, 2018 at 12:16 pmpeteroznewmanSubscriber
Wow! For a beginner with ANSYS, you have made a lot of progress, well done.
Here are a list of changes I recommend.
The two solids are assigned to be Structural Steel. Create a Concrete material and assign that to the inner solid. The material has to have some failure mechanism added because all you have is a linear material and that never fails. For the concrete, the Microplane method is recommended. For the steel, you have to add Plasticity. A simple model is Bilinear Isotropic Hardening. In that model you just need the Yields Strength and the Tangent Modulus.
There is bonded contact between the faces that touch. Delete the bonded contact between the bodies, that is unnecessary.
The mesh has only one element through the thickness of the steel. At least four elements are required.
Delete the Contact Match Group, that is not required.
You can also add a mesh control called Inflation to make smaller elements near the outside of the inner core.
It is recommended to change from force to displacement to plot the ultimate load capacity of the column. Add a Reaction Force to the Solution results to plot the force vs displacement curve.
Under Analysis Settings, turn Auto Time Stepping On and use Initial Substeps, Minimum Substeps to be 20 or higher to get 20 points plotted on your curve. The Maximum Substeps can be 200. Turn on Large Deflection.
In the chart, you Omit Time.
I may have missed something, so implement those changes and see what you get.
October 18, 2018 at 1:57 pmNiranjanRameshSubscriber
Thank You for your response.
August 24, 2019 at 8:44 pmFraolSubscriber
Niranjan Ramesh, where is the model that you attached. I cant seem to find it.
Peteroznewman, Can i model the column using an incremental load that will be controlled using a displacement control? (say like 0.2mm/min rate)
August 24, 2019 at 10:44 pmpeteroznewmanSubscriber
Yes, you can use displacement control. Rather than a rate of 0.2 mm/min, time in a Static Structural model is arbitrary. You can have a total deformation, that occurs over a nominal 1 s, be divided into 100 substeps.
September 30, 2019 at 4:31 pmDiegoandree1311Subscriber
Hello greetings to all, and excuse the invasion of this post (I hope NiranjanRamesh has managed to answer your question).
I am trying to model a slab in Ansys and my goal is to achieve the calibration of it and compare it with a real model made by different researchers, in short I am having problems because I worked almost 4 months with solid65 for the concrete but then 1 or 2 weeks ago I changed to solid185 with the theory of the microplane, the problem is that I don't know how to calculate the ultimate load and the graph of Load vs. deformation, I am solving as I can but I am not sure if the way I am doing it is correct
I used commands for the materials because I didn't know how to make concrete and steel tubing a compound effect, since the concrete was always deformed but the steel was static, use the mycoplanar and BISO commands for steel with their respective data
to determine the load, place a deformation reaction with the following values, and the result of stress (in the column) I multiply it by the transverse area, and so I determine the last load but I don't know if this is the way everyone mentions do a deformation controlled test
I would greatly appreciate your help, regards
September 30, 2019 at 5:29 pmDiegoandree1311Subscriber
This is the link of the model I am making
September 30, 2019 at 7:06 pmpeteroznewmanSubscriber
Diego, it is better for you to start a New Discussion. When you do, you get an email notification when any replies are posted. Also, this discussion is marked as Solved, which means some members will not read the discussion.
You can include a link to this discussion in your New Discussion post.
October 24, 2019 at 10:08 pmfkezada5Subscriber
I been working on concrete filled steel tube. I want to get the ultimate load from the model, Is there any possibilities of doing that in ansys workbench?, kindly help me out. Thanks in advance.
dear niranjan. i 've been working on a CFT column too, well, actually an I beam - CFT column connection. i dont know how to model de concrete inside de column.
could you help me with that? i really really need some helps, please. i got a code, but it doesnt work
October 24, 2019 at 10:08 pmfkezada5Subscriber
October 24, 2019 at 10:09 pmfkezada5Subscriber
hi diego, do you speak spanish?
December 30, 2019 at 7:08 pmDiegoandree1311Subscriber
Si señor, y se me dificulta un poco pedir ayuda por acá por lo mismo. saludos
- 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.
- 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
- Colors and Mesh Display
- How to calculate the residual stress on a coating by Vickers indentation?
- 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
© 2023 Copyright ANSYS, Inc. All rights reserved.