July 27, 2023 at 6:30 amM UsmanSubscriber
Hey Everyone, I am working on a problem in which a hot body having temperature 200-300 degree celcius is getting cooled by the air which is flowing over the body having 0.5 mach speed. I want to know the time it takes for the body to attain normal temperature or alternatively for specific time period likle 2s, 3s or 5s, what is the temperature drop in body. I have tried normal steady state approach and Conjugate Heat transdfer approach using stead state and transient mode as well. But results are same as the temperature contours which initially developed on the body remain same and the iterations on further converge those results like wven in trainsient, I am unable to control the time for which the air is flowing over the body. And when I do the FSI, the analysis time it shows is 1 second which I am assuming is flow time of air over the body. Transient analysis gives the same results only soure time changes if I try to change the flow time.
Help needed from the experts.
July 27, 2023 at 10:51 amRobAnsys Employee
What does the FSI bit do?
If you're not seeing any cool down of the solid, how are you defining the surface between the fluid & solid?
July 30, 2023 at 5:23 amM UsmanSubscriber
I am seeing solid cool down but the analysis time is 1 second which I am unable to change.I want to see how much body gets cooled down at diferent times like in 3 seconds, 5 seconds etc. And for that I want to know which approach should I use.
July 30, 2023 at 6:30 amNickFLSubscriber
It sounds like you are using ANSYS mechanical for a thermal analysis and not Fluent or CFX. This is the fluid board, and you may want to post over there to get a better answer. These fluid packages could solve for the thermal temperatures in the body and the flow field. Obviously, if you just need the temperature in the body this is a bit of an overkill. What are the boundary condition you actually have?
There is a nice Mechanical thermal analysis example in one of the Innovation courses (it involves radiation, but the model building is the same). I recommended you look at that. Keep in mind that if you are modeling the air domain in your model, you won't actually see any fluid moving.
But to answer your question directly, click on Analysis Settings in the tree. In the details panel change the end step time. You can also specify the interval you want to solve at.
July 30, 2023 at 6:50 amM UsmanSubscriber
I am actually using CFD fluent to do the analysis (Conjugate Heat Transfer Analysis) and only using FSI to see the temperature changes on the solid body. The problem I am talking about is to set different flow times in ansys fluent to see the temperature changes in the body. For example in the image below the body temperature changes from 300 degree to lower temperature when air with 27 degree celcius temperature flows with 0.5 mach speed. Now here analysis time is 1 second written which I beleive is air flow time ovewr the body. I want to variate this time to see when does the body reaches a normal temperature. But even in transient analysis, when I change the flow time and import the results to the body using FSI, only the source time changes while analysis time remains the same.
July 31, 2023 at 4:48 amNickFLSubscriber
Based upon what I see, you are importing the body temperature. Then you really are giving Mechanical nothing to solve as you are telling it what the solution is.
Think back to your heat transfer class. What type of heat transfer do we have here? And when solving convection problems, what was the one term we were constantly having to find using correlations? That is the quantity you want to be taking from Fluent and mapping onto the surface of your Mechanical model. Then you can set up this transient analysis with an initial temperature of 300° in the body and then the software will calculate the temperature field in the body.
Keep in mind with the heat transfer coefficient you also need to define the free stream air temperature.
July 31, 2023 at 9:30 amM UsmanSubscriber
I am only using mechanical to see body temperatures as fluent shows static and total temperatures which are different from body actual temperatures. My all working or approach relies on ansys fluent. I just want to vary analysis time or air flow time to see body temperatures after time periods of 2s , 3s or 5s etc. Ansys fluent automatically gives me the cooling of body to certain temperatures as shown above after time period of 1 second. That is my concern here.
July 31, 2023 at 10:20 amRobAnsys Employee
Please can you explain what you mean by body temperature?
July 31, 2023 at 11:27 amM UsmanSubscriber
Actually there is a hot solid body having 300 degree celcius temperature and is being cooled by air flowing over it with 0.5 mach speed and 27 degrees temperature. I want to see how much it cools the body over the period of time which can vary or I can control. For that I did Conjugate Heat Transfer analysis with air as fluid and rod as solid body. Body gets cooled from 300 degree celcius as shown above but it is for specific period of time. I want to cool it to room temperature but I am unable to do that as I am unable to change the time for which air flows over the body. The more is the air flow time, the cooler the body will be.
July 31, 2023 at 12:49 pmNickFLSubscriber
You want to be mapping the heat transfer coefficient on the outer surface not the temperature of the body.
July 31, 2023 at 12:15 pmRobAnsys Employee
You can set the number of time steps and time step size in Fluent to simulate a certain amount of time.
July 31, 2023 at 12:33 pmM UsmanSubscriber
Yes I have done that on Ansys Fluent assuming that it would work but the temperature contours developed on the body remains the same irrespective of the number of seconds I set as flow time. And when I import those temperatures on the body in mechanical, only the source times changes while amnalysis time remains the same. This is the reason I am stuck on this simple problem from many days. Below is the first image of steady state analysis, and second image is of transient analysis in which I set the flow time to 2 second. You can see the temperatures on the body are same.
July 31, 2023 at 12:47 pmRobAnsys Employee
How many time steps did you use to get to 2s?
July 31, 2023 at 12:59 pm
July 31, 2023 at 4:41 pmNickFLSubscriber
- Are you solving for the temperature distribution within the solid body in Fluent, correct?
- You are mapping this temperature onto the body in ANSYS mechanical, correct? If so, what time step are you using?
- Again, the approach I would take is to be mapping the heat transfer coefficient from the steady state model onto the outer surface of a transient thermal mechanical model. Then you can simply run for whatever length of time until the body reaches the temperature you want.
July 31, 2023 at 2:58 pmRobAnsys Employee
And did each time step converge?
August 1, 2023 at 7:16 amM UsmanSubscriber
In actual I want to simulate how the cooling of Fighter Jet Gun firing at 3400-3600 rounds per minute and Jet moving at 0.5 mach speed through air gets cooled by the convective heat transfer due to air flow. The concered area is gun barrel in which heat is generated and its wall reaches 200-300 degree celcius temperature. So to first just set the right approach, I am using a solid rod having a temperature of 300 degree celcius gets cooled by air. So yes i am solving for the temperature distribution on the solid body and I am using mechanical only to import temperature loads on the body to see the temperatures on the body. Not running ay solution in Mechanical. Now the only difficulty I am facing is to vary the air flow time and get diferent temperature contours.
August 1, 2023 at 7:59 amRobAnsys Employee
To echo Nick's comments. There's no need for Mechanical here.
Flow around the cylinder is done in Fluent, and have a look at the NACA wing for some ideas about compressible flow. The cooling will also come from that, but you will need to decide on your initial conditions. Ie do you cool from a stationary point or assume it's at Mach 0.5 and then cools?
August 1, 2023 at 10:27 amM UsmanSubscriber
Boundary Conditions: At inlet, the fluid (air) is flowing at 0.5 mach speed with 27 degree Celcius as its temperature. On rod boundary walls, the temperature is 300 degree celcius. The meshing is done in such a way that Conjugate Heat Transfer Occurs and body gets cooled downn by air flow. But results become constant 1 second air flow time and no matter how much time I set as air flow time in transient analysis, the results remain the same.
August 1, 2023 at 10:36 amRobAnsys Employee
Please post a contour from Fluent showing the temperature field of the air flow & solid: a plane down the centre is sufficient. On the same surface also plot velocity and Mach Number, post those too.
August 1, 2023 at 12:46 pm
August 2, 2023 at 5:07 amNickFLSubscriber
Are you running this simulation with constant properties? If so, you can save yourself a bundle of time by removing the flow equations from the transient solve. Here would be a possible approach:
- Conduct a steady-state flow analysis. (& save!)
- Set-up the model as a transient solve.
- Patch the temperature of 300° onto the solid body. (Patch is under the Initialization panel in the Tree. Be sure to patch ONLY the temperature as if you do anything else you will destroy the flow field you already solved for and are continuing to use.)
- Turn off the flow and turbulence equations and solve only for the energy. This can be set in the Tree under Solution->Controls->Equations
- Set up an Monitor points on the body, .cxa animations or other quantities before you run.
- Save the case file to a new name (indicate that it is transient)
- Run, and enjoy a good cup of coffee while the computer does its thing!
I would also recommend that you do a free-slip wall condition on the upper and lower surfaces of your tunnel. It won't change the results much but be more aesthetically pleasing.
August 1, 2023 at 1:07 pmRobAnsys Employee
OK, and if you run on for some time steps? How did you set the temperature in the solid?
August 2, 2023 at 5:23 amM UsmanSubscriber
August 2, 2023 at 5:28 amNickFLSubscriber
On closer look (sorry, I am editing what I wrote earlier) you have a problem with the interface. What you have in the above panel is say there is a fixed temperature at the surface of the body. Keep this set as coupled that allows the heat transfer thru the interface from solid to fluid. This is why there is no cooling to your body because you are setting the wall temperature as 300. You only want to set the initial temperature to be 300. The easiest way is using the patch command in intialization tab.
My recommendation is to go back and look at the example of conjugate heat transfer in tutorials.
August 2, 2023 at 12:39 pmM UsmanSubscriber
My simulation is working now correctly. Thanks alot for your 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.
- Floating point exception in Fluent
- What are the differences between CFX and Fluent?
- Heat transfer coefficient
- Difference between K-epsilon and K-omega Turbulence Model
- Getting graph and tabular data from result in workbench mechanical
- The solver failed with a non-zero exit code of : 2
- Suppress Fluent to open with GUI while performing in journal file
- Mesh Interfaces in ANSYS FLUENT
- Time Step Size and Courant Number
- error: Received signal SIGSEGV
© 2023 Copyright ANSYS, Inc. All rights reserved.