applying strain obtained to next analysis

  • 252 Views
  • Last Post 14 December 2019
  • Topic Is Solved
Gijoys4v posted this 04 December 2019

Please help!

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. 

Order By: Standard | Newest | Votes
peteroznewman posted this 04 December 2019

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.

  • Liked by
  • Gijoys4v
Gijoys4v posted this 05 December 2019

Thank 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)

peteroznewman posted this 05 December 2019

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.

  • Liked by
  • Gijoys4v
Gijoys4v posted this 05 December 2019

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? 

peteroznewman posted this 05 December 2019

You don't make the part dead, you just make the Contact dead. It is called Contact Step Control. I gave you the details above. To find it, open Mechanical on the Model and click on the Static Structural branch. On the Conditions pulldown is Contact Step Control.

  • Liked by
  • Gijoys4v
Gijoys4v posted this 05 December 2019

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.

Gijoys4v posted this 05 December 2019

or else do you know the command for this?

Gijoys4v posted this 07 December 2019

Hallo peteroznewman

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

Gijoys4v posted this 07 December 2019

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)

peteroznewman posted this 07 December 2019

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.

  • Liked by
  • Gijoys4v
Gijoys4v posted this 08 December 2019

thank you for your valuable and timely reply. it really helped me a lot

Gijoys4v posted this 08 December 2019

I obtained a surface plot like this while calculating the strain. Is there is any option to take the volume average of the result. Actually I need the average value

peteroznewman posted this 08 December 2019

 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.

  • Liked by
  • Gijoys4v
Gijoys4v posted this 09 December 2019

Thank you.... I will do

Gijoys4v posted this 09 December 2019

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)?

peteroznewman posted this 09 December 2019

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.

  • Liked by
  • Gijoys4v
Gijoys4v posted this 12 December 2019

Thank you, it worked 

Gijoys4v posted this 13 December 2019

which solution will be correct? with large feflection ON? or large deflection OFF? in the analysis settings

Gijoys4v posted this 13 December 2019

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

Gijoys4v posted this 13 December 2019

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!!!!

Gijoys4v posted this 13 December 2019

I tried to solve a problem , but end up with some issues ; please help me to proceed. figure below shows what i have done

 

peteroznewman posted this 13 December 2019

a

peteroznewman posted this 13 December 2019

 

  • Liked by
  • Gijoys4v
peteroznewman posted this 13 December 2019

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?

Gijoys4v posted this 14 December 2019

sorry

Close