April 21, 2019 at 4:17 pmmutianzi1Subscriber
Hi. I was performing a transient analysis of a structure. Below is the time history of displacement of the structure. Due to the abrupt application of the load, there is a transient effect at the beginning of the time history (very large fluctuations).
To reduce the transient effects. I conducted a static analysis before the transient analysis, and the load for the static analysis is the same as the load in the first time step in the transient analysis. Below is the setup in Workbench. But I got the same results as the case that I only conducted transient analysis. Does anyone know how does this happen? Anything wrong with the setup?
Thanks in advance. Any help is appreciated.
April 21, 2019 at 5:51 pm
April 21, 2019 at 7:20 pmmutianzi1Subscriber
I guess not. I used bilinear material, and the large deflection is turned on.
April 22, 2019 at 7:13 amjj77Subscriber
Pre stress creates an initial stress that is translated to an equivalent stiffness matrix -Thus it does not initiate a solution (e.g., a transient one)
Read through the help manual and the section of Transient Structural Analysis and subsection about initiating and initial conditions.
Basically one needs to have two steps - first step where the initiation/initial conditions are established (no dynamic effects are considered thus using no time integration in first step), and then the other one (2nd step with dynamic effects) that continues from that state with the transient analysis. Typically in structure analysis gravity only is applied in that first step, and then any other transient loads are applied after that in the second step.
Below is an image of a cantilever beam that has gravity (1st step going up to 1 s), and then after 1 s a gradually increasing transient force is applied as can be seen in the second step.
See the help manual for more info
April 23, 2019 at 2:02 ampeteroznewmanSubscriber
jj77 is correct that the Static Structural to pre-stress a MSUP transient does not cause any initial stress or deformation.
I read the online help as jj77 suggested and learned that a 3 step Transient solution is probably the best option.
For a simple example, say the static load is standard earth gravity (9.8 m/s^2) which causes a displacement of 0.1 m.
Here is what happens in a 2 step solve.
- Step 1 ramps the gravity load on from 0 to 0.001 s with Time Integration Off.
- Step 2 is the beginning of the transient load, with Time Integration On, but the model has been given a 0.1/0.001 = 100 m/s initial velocity at the end of step 1.
This causes as big or bigger problem with the beginning of the transient simulation as the sudden appearance of a gravity load. The problem could be mitigated by ramping on the load over 1 second, which would take a long time to compute, but the model would still have a 0.1 m/s initial velocity at the beginning of step 2. The 2 step solve is actually the method used to create an initial velocity in those problems where this is what is wanted.
The preferred way to accomplish an initial load with zero initial velocity is to have 3 steps.
- Step 1 is the same as above.
- Step 2 also has Time Integration Off and ends at 0.002 s. Since there were no changes in load from step 1 to step 2, nothing moved, which means the velocity at the end of step 2 is zero.
- Step 3 has Time Integration On and begins with the initial deflection and stress, but with a zero velocity.
Attached is an ANSYS 19.2 archive that shows a 3 step transient structural. The Static Structural analysis is just there for comparison and is not required for the Transient Structural to do its initial deformation.
April 25, 2019 at 3:39 pmmutianzi1Subscriber
Thank you for the suggestion! I will try now.
April 29, 2020 at 12:55 pmsma4tSubscriber
mutianzi1, could you please add some relevant tags to this topic? I find the discussion very useful and I'm sure others who concern with transient analysis will find it useful, too.
Here's some suggestion for the tags:
April 29, 2020 at 2:38 pmpeteroznewmanSubscriber
I added two tags, but the discussion is already in the structural mechanics category.
May 22, 2020 at 7:14 amArj1995SubscriberI have a problem of a 3D part consisting of hyperlelastic material along with metal parts. I need to find the natural frequency.I have currently used the prestress modal analysis tool. Also given non linear adaptive meshing. Still there is distorted elements and convergence. Please help.
- 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
- 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
- Defining rigid body and contact
- Colors and Mesh Display
- A solver pivot warning or error has been detected
© 2023 Copyright ANSYS, Inc. All rights reserved.