July 8, 2019 at 2:10 pmericpflorSubscriber
Hi, I'm trying to model construction sequence (staged construction) on ANSYS 19. By now, I have a simple model with two columns, modelled as link/truss, connected by a common node (2 elements, 3 nodes total). In the first load step, there's only the bottom column and the axial load applied to it. In the second step (by using birth and death control) the upper column comes alive as long as the load applied to it. My problem is: I need the upper node on the upper column to be in original position (disconsidering the deflection inherited from the bottom column from the first load step) when it comes alive. Is there any way to automatize this consideration after each load step? I intend on increase the number of columns/load steps. Any help would be appreciated.
July 8, 2019 at 2:18 pmpeteroznewmanSubscriber
It would be helpful if you include an image of your structure and annotate it with the sequence of the elements coming alive.
July 8, 2019 at 2:36 pmjj77Subscriber
This is very strange - you add a second column to the bottom one of course you are going to have the top of the top one being lower than the original position.
Stage construction models reality, what type of scenarios is this (just playing with this or)?
In any case if you do not want the top node of the top column to move just fix that vertex.
July 9, 2019 at 1:22 pmericpflorSubscriber
Hi, thanks in advance for your responses. This is actually for my masters dissertation.
I attached a picture to illustrate my case.
The reality in this case is to simulate the fact that at every concrete cast stage the deflection on the upper nodes os the structure are 'zeroed out'. Otherwise, the analysis would lead to unreal (large) displacements, specially on the upper nodes of the structure, as you can see in the 2nd scheme on the picture. This is very useful in the analysis of tall buildings, for example.
Here's my intention:
Stage 1-1 - a load (P) is applied, equivalent to 1 displacement.
Stage 2-0 - the upper column comes alive with upper node on the original position
Stage 2-1 - the load on the upper node is applied, leading to 1 displacement at the first column node and 2 displacemnts on the 2nd column node (1 displacement from its own deformations and 1 inherited from the bottom)
Stage 3-0 - a third column is applied and there it goes...
I tried the use 'part transform', apply a displacement on the opposite direction, element birth and death, but no success so far...
July 9, 2019 at 1:38 pmjj77Subscriber
We said fix some degrees of freedom on the top of the column that you do not want it to move.
An example: 2 columns (1 and 2). 4 Steps/stages.
1 stage: Only the bottom column (1) is active which has an axial load and a bottom fixed support; 2: Both columns active with the top vertex of the top column fixed as well (all 3 dof -translations - see displacement support in the tree); 3: The same as two so nothing happens here, just a dummy stage; 4: The top restrain on the vertex of the top column is released/deactivated (free), and an axial load is applied on the top column (2 which became active in stage 2), thus the top vertex should move down.
This can be seen below (green-line shows the top vertex, does not go anywhere until stage 4 - red line is on the top of the first column or if you want at the bottom of the second top column):
(One can do hand calcs. and get the same result so it is OK)
July 10, 2019 at 3:06 pmericpflorSubscriber
It worked perfectly, thank you so much!
By curiosity: Is stage 3 ("dummy stage") necessary for this consideration?
July 10, 2019 at 3:21 pmjj77Subscriber
Not really it was just for me to check.
- 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.
- User manual
- Colors and Mesh Display
- material damping and modal analysis
© 2023 Copyright ANSYS, Inc. All rights reserved.