December 4, 2019 at 11:56 amGijoys4vSubscriber
I applied temperature load (from 1000K to 500K) on a geometry and obtained the strain. Next I want to apply the temperature load (500K to 200K) on the same geometry in which the strain obtained previously should be there. How can I do this ansys? When I tried to couple the first solution to the next structural analysis; it is not working. It shows that the next structural analysis became the submodel of the previous one. In short; I want to apply a residual stress in the model.
December 4, 2019 at 8:52 pmpeteroznewmanSubscriber
Is the only thermal load Temperature? Is it applied to the entire body? In that case, the temperature is uniform over the whole body and you can apply that load directly into a Static Structural model using Thermal Condition and there is no need for a Thermal model.
If you have to solve for the non-uniform distribution of temperature due to other boundary conditions, then you need the linked analysis systems. In the Thermal analysis that changed the temperature from 1000K to 500K, under Analysis Settings, where it says Number Of Steps 1, make it 2.Then in the Temperature load, there will be a second row where you can type 200K for step 2. Create 2 steps in the Static Structural system. On the Imported Body Temperature, make the settings shown below.
December 5, 2019 at 1:50 amGijoys4vSubscriberThank you for your reply. Iam applying only thermal load and your reply helped me. But a problem arises when I tried the same in a new geometry. The situation is as follows:
I have two plates bonded each other which is at a temperature of 1000K. Then I have to cool the plates to a temperature to 500K. So a strain arises in these plates. Next at temperature 500K, I have to bond two more plates over the previous two and then I have to cool all these to 200K. So when I followed the method you said earlier upto 500K(when there only two plates) there was no problems. But when I added the two plates, ansys says the solution has to be cleared for adding the extra plates. How can I add those two plates at 500K on the two plates without clearing the solution (means I need the residual strain on the first two plate, when I am adding the two new plates on top of those previous)
December 5, 2019 at 4:12 ampeteroznewmanSubscriber
I have two plates of the same material made to have the same length at 1000 K.
In Step 1, the right part stays at 1000 K, while the left part is cooled to 500 K.
In Step 2, the bonded contact, which was Dead during step 1 is made Alive in step 2.
In Step 3, the temperature of the right part is cooled to 500 K and the strain bends the part.
You can build this out in subsequent steps to make alive another bond to another layer and cool it to 200 K.
December 5, 2019 at 5:13 amGijoys4vSubscriber
Thank you, your timely reply giving me a lot of help and relaxation. But I don't know how to make a part dead and alive in steps. From where I can find that option to make a part dead or alive?
December 5, 2019 at 12:32 pm
December 5, 2019 at 2:13 pmGijoys4vSubscriber
Thank you for your reply. very sad to inform you that I was trying to do the analysis with Ansys 18.1 which is not having this provision. I will try Ansys 19 and inform the progress and contact you soon.
December 5, 2019 at 2:14 pmGijoys4vSubscriber
or else do you know the command for this?
December 7, 2019 at 9:35 amGijoys4vSubscriber
Now I have Ansys 19. In the above explained example by you. How you maintained one part at 1000K and the other cooling to 500K. Expecting your reply. Thank you
December 7, 2019 at 9:46 amGijoys4vSubscriber
Also whether we can do the same example like this. while making the contact alive whether we can cool the second part to 500K. whether it is required that the making the contact alive should be made in a single step(means whether a step should be separetely assigned for making the contact alive)
December 7, 2019 at 12:23 pmpeteroznewmanSubscriber
The Thermal Condition load in Static Structural allows me to assign a Temperature load to a body. In this case, I have two bodies and the each has an independent Temperature load on the body. This is a 3-step analysis and the Environment temperature, which sets the temperature of all bodies at the start of the simulation, is set to 1000K. In step 1, I change the Temperature of one of the bodies to 500K and leave the temperature in the other Temperature load at 1000K.
In step 2, the contact comes alive. That means a hot body is being bonded to a cool body.
In step 3, the temperature of the hot body is changed to 500K and the cool body remains at 500K. This is when the strain develops that bends the beams.
December 8, 2019 at 5:37 amGijoys4vSubscriber
thank you for your valuable and timely reply. it really helped me a lot
December 8, 2019 at 5:42 am
December 8, 2019 at 3:32 pmpeteroznewmanSubscriber
Please learn how to make a screen snapshot that does not have a huge white border.
You can right mouse click on a result and Export the nodal data to a CSV file, then perform the volume average in Excel or matlab.
December 9, 2019 at 1:24 pmGijoys4vSubscriber
Thank you.... I will do
December 9, 2019 at 1:26 pmGijoys4vSubscriber
Is there any provision in ansys sothat we can make a fixed support (or other similar supports) active after a particular load step(say after 2 steps)?
December 9, 2019 at 1:43 pmpeteroznewmanSubscriber
Not Fixed Support, but Displacement can be set to Deactivate, or Activate by load step. In the Tabular data panel where it shows the displacement setting, which can be 0, you right mouse click on a row and select Deactivate. Contact objects can be set to activate or deactivate by load step also.
December 12, 2019 at 4:55 amGijoys4vSubscriber
Thank you, it worked
December 13, 2019 at 10:37 amGijoys4vSubscriber
which solution will be correct? with large feflection ON? or large deflection OFF? in the analysis settings
December 13, 2019 at 12:26 pmGijoys4vSubscriber
while I solved a structural problem using workbench in 1step(analysis setting 1 step is given with 10 substep), I could obtain the stress at each substep. But when I solved the same problem in 2 time step(in the 1st time step I made one side of the beam fixed and the next time step a displacement is given), in the second time step I can find only the final answer, the substep I given havent seen. Please help me to resolve the problem
December 13, 2019 at 12:27 pmGijoys4vSubscriber
for finding ut the reaction force after structural analysis in workbench, I have seen different location methods in the details window like boundary condition, beam , spring, surface etc. which one I have to choose. how can I understand which one I have to choose for a particular problem. what is the meaning of each one?. Please help!!!!
December 13, 2019 at 3:49 pm
December 13, 2019 at 6:52 pmpeteroznewmanSubscriber
December 13, 2019 at 6:54 pm
December 13, 2019 at 8:06 pmpeteroznewmanSubscriber
Your last question was answered in this post.
Can you see how you can waste our time if you are asking the same question in more than one discussion?
December 14, 2019 at 4:29 amGijoys4vSubscriber
December 14, 2019 at 4:42 pmpeteroznewmanSubscriber
- 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.
- Solver Pivot Warning in Beam Element Model
- Saving & sharing of Working project files in .wbpz format
- 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
- User manual
- 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
- material damping and modal analysis
- Colors and Mesh Display
© 2023 Copyright ANSYS, Inc. All rights reserved.