September 13, 2018 at 2:47 pmAndreaEnidSubscriber
I want to assign a base acceleration at the base of a wall that have a rotational base constraint. I used a revolute joint to assing its stiffness.
The base acceleration allows me to put the base acceleration only at fixed and displacements supports. I will appreciate any help.
September 13, 2018 at 3:21 pmpeteroznewmanSubscriber
Base acceleration is used to simulate the input a structure might see in an earthquake or when sitting on a vibrating rigid surface like an engine block or a shaker table top.
Can you provide an image of the structure you are working on. I don't understand your "rotational base constraint". Do you mean you have a revolute joint that you added a spring to add rotational stiffness?
September 13, 2018 at 3:37 pmAndreaEnidSubscriber
The wall is the element at the left. The other big element is fixed at the base. The assigned revolute joint at the base of the wall is the one that appears in the tree at the left, below of Connection. I want to put an earthquake at the base of the wall and the other element. ANSYS allows me to put the base acceleration only to the fixed base, but I want to put the acceleration at the base of the wall too.
September 13, 2018 at 3:39 pm
September 13, 2018 at 3:52 pmpeteroznewmanSubscriber
Is the yellow wall bonded to the large block?
If so, then just include the bottom of the wall as a Fixed Support. There is such a large mass and a long contact area that the revolute joint on the short edge on the bottom of the wall is going to be insignificant. Suppress the Revolute and add that edge to the Fixed Support.
September 13, 2018 at 4:11 pmAndreaEnidSubscriber
Oh ok. Yes, the yellow wall is bonded to the large block. The problem is that I want to model the wall with a rotational constraint with a stiffness (I have the value), that is a important part of the model. And I need to put the acceleration at the base of the large block (soil) and the wall, but the program allowed me to put it only in the fixed one.
September 13, 2018 at 7:33 pmpeteroznewmanSubscriber
Create a stand alone Transient Structural analysis system (not connected to Modal) and you can have your rotational joint and spring and apply the earthquake acceleration to all the mass in the model using an acceleration-time history load.
If the wall is supporting a block of soil, I'm not sure that Bonded Contact is appropriate. Wouldn't frictional contact be more appropriate?
September 18, 2018 at 1:29 amAndreaEnidSubscriber
I already did that too, but in reality the amplitude of the earthquake is not the same in all the soil. I need to assign the acceleration as a base acceleration.
I am comparing different cases, and one of those cases is considering a Bonded Contact.
September 18, 2018 at 2:42 pmpeteroznewmanSubscriber
You could create a third rectangular block under the soil and the wall. Make that a rigid body and use either bonded or frictional contact to the soil. The rotational joint with its mobile side scoped to the base of the wall will now have its reference side scoped to the rigid body. Add a translational joint between the rigid body and ground and add an acceleration load to that new joint. Now you have base acceleration on the soil and the wall.
September 24, 2018 at 3:09 amAndreaEnidSubscriber
How can I assign acceleration at the translational joint? I am trying to do that but for base accelerations the program allows me to assign it on fixed support or on a displacement boundary condition.
September 24, 2018 at 3:41 ampeteroznewmanSubscriber
If you don't have a Modal analysis solution feeding into the setup of a Transient Structural analysis, then you can assign an acceleration to the translational joint.
If you do have a Modal analysis solution feeding into the setup of a Transient Structural analysis, then suppress or delete the Translational joint and load and use a Fixed Support on the bottom of the third rectangular block. Then you can use base accelerations.
September 24, 2018 at 4:24 amAndreaEnidSubscriber
I did the second option. When I choose the bottom of the third rectangular block to be fixed, it did not want to assign it. The image shows what happen when I want to assign the bottom to be fixed.
I tried also the first option, but in that case the acceleration will be in all the bodies and I do not want that case.
September 24, 2018 at 2:08 pmpeteroznewmanSubscriber
In the first option, when you apply an acceleration load to a translational joint, that is applying the acceleration to the linear translation of the joint. It is a motion input, not an inertial acceleration load that acts on all mass at the same time, but acts only to displace the joint. If the soil acts like a very soft elastic body and is sitting on a rigid platform that suddenly accelerates upward, the bottom of the soil will move with the rigid rectangle in the first instant, while the soil at the top will have no motion. That is very different than applying an inertial acceleration load where all the soil will experience the acceleration in the first instant.
In the second option, I forgot that you can't assign a Fixed Support to a Rigid body. Just keep the joint but change it to a Fixed joint.
October 1, 2018 at 1:28 amAndreaEnidSubscriber
Hi peteroznewman. I tried the option of assigning a translational joint at the bottom of the rigid element and a fixed joint between the soil and rigid element. Then, I applied the acceleration load at the translational joint. When I click solve, several minutes later the program stop with the next message.
I also tried using the fixed joint at the base of the rigid element, but using that option ANSYS does not allow me to apply the acceleration as an acceleration load to the joint and neither as a base acceleration.
October 1, 2018 at 3:17 amAndreaEnidSubscriber
When I assign a translational joint - ground to surface body, the joint in that is in 'the ground' is considered fixed right? If that is true, can I assign to that 'fixed joint' an acceleration? I think the answer is no but I am curious anyway.
October 2, 2018 at 12:59 ampeteroznewmanSubscriber
A Joint consists of two Coordinate Systems with equations that limit the motion between them. When the Joint is between a Body and Ground, the second coordinate system is fixed to ground. If you don't want a body to move, you can define a Fixed Joint. When you want a body to move along one axis, that is a Translational Joint.
I tried the option of assigning a translational joint at the bottom of the rigid element and a fixed joint between the soil and rigid element. Then, I applied the acceleration load at the translational joint. When I click solve, several minutes later the program stop with the next message.
There are lots of reasons why the solver can generate an unknown error. If you create a Workbench Project Archive .wbpz file, you can attach that to a post, then I can take a look at it.
October 8, 2018 at 9:54 pmAndreaEnidSubscriber
Hi! I am very thankul with your help. Next is a link sharing the model.
Thank you again!!
October 8, 2018 at 10:13 pmpeteroznewmanSubscriber
What version of ANSYS are you using, 19.1 or some other version?
October 8, 2018 at 10:22 pmAndreaEnidSubscriber
Yes, the version I am using is 19.1.
- 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.