May 25, 2021 at 5:12 pmdodonn4Subscriber
I am working on a simulation in which a blood bag is removed from a cooler and placed in ambient air. The goal is to determine the temperature on the outside of the blood bag when the center of the blood reaches a certain temperature.
I am trying to model free convection in Fluent, but keep struggling with the boundary conditions. Other examples I have found online involved a hot solid object cooling off in air, but my system involves a cold liquid warming up in air through free convection and conduction through the plastic bag wall.
I have tried a few different models that essentially all have a large enclosure around the blood bag to represent the warmer ambient air, but had no luck. The boundary conditions applied included pressure inlets on every side of the enclosure except the top, which is a pressure outlet, and then wall boundary conditions with shell conduction applied to the plastic bag wall.
Could anyone recommend a different approach to this problem, or possibly share some helpful references/documentation to guide me?
Thanks in advance!May 25, 2021 at 6:58 pmmichael.hanchakSubscriberCouple of ideas:
1) use "outflow" boundary condition for the top and pressure-inlt for the sides (and bottom). You could also try "wall" for the sides.
2) if the blood is cold and thick, model that as a solid with the right density, k, and Cp. In other words, first ignore convection in the blood.
I always try to simplify the problem as much as possible. Ignoring blood convection and using standard HTC for convection, what does the hand calculation predict?
Hope this helps, Mike
May 26, 2021 at 3:21 amdodonn4SubscriberThank you! I tried your first idea and it seemed to work fairly well. However, there is no convection happening inside the bag, and I cannot figure out how to solve that. After running the simulation the temperature gradient of the blood inside the bag is a constant value, When reading the documentation, it states that one of the thermal boundary conditions I can apply at the wall is a convective boundary, but I cannot seem to find that anywhere when setting my boundary conditions. In the thermal tab of my wall boundary condition, the only options for "thermal conditions" are: Heat Flux, Temperature, and Coupled.
The closest way I could find for setting convection is by making the blood volume a radiator type boundary condition and inputting the heat transfer coefficient there, but I do not think the radiator condition is accurate.
Any advice for be greatly appreciated!
May 26, 2021 at 12:53 pmmichael.hanchakSubscriberGlad it helped! A couple of ideas:
Make sure gravity is turned on.
The interfaces between air-to-bag, and bag-to-blood should be of type "coupled." The convection will be determined by the flow solver (conduction plus advection)
Do you have temperature dependent density for the blood? If not, at least the Boussinesq approximation value? Without density changes or Boussinesq there will be no thermal convection in the blood.
May 26, 2021 at 2:18 pmdodonn4SubscriberI think my problem is with the interfaces. When making the named selections, I create an interface between the faces for air-to-bag interface, then I make another for the faces for bag-to-blood interface and they end up being the same exact interface. I get an error stating there are overlapping named selections, and when I highlight each individual named selection they are the same thing. For example, if I hide the geometry for the blood inside the bag and then highlight the named selection for the bag-to-blood interface, it shows the faces from the air-to-bag interface. Essentially, it seems to be acting like the bag is not there.
Could this be an error in my geometry setup? I created the bag by copy-and-pasting the faces of the blood volume and giving those surfaces a shell thickness during meshing. I can highlight and see there are different surfaces for the bag and the blood, but when I try to apply a named selection it seems to mess things up.
May 26, 2021 at 2:55 pmRobAnsys EmployeeIf you did the share topology step the surface between the blood and air should be a wall and wall:shadow pair. Heat will pass through the surface (you can set a thickness too for heat transfer) and you can inflate both sides to get a good near wall mesh.
May 26, 2021 at 4:46 pmdodonn4SubscriberThanks for the suggestion, Rob!
Yes, I did do the share topology step, and there is the wall and wall:shadow pair for that surface. I set the thickness and turned on shell conduction.
However, I am still stuck figuring out the convection. My previous fluent model corrupted so I had to start over, but now I can't seem to get the blood or ambient air volume to load into fluent. All of my other named selections loaded fine, and there are internal boundary conditions named "interior-blood_domain" and "interior-air_domain" present, but when I select them an error appears: "Surface for zone interior-blood_domain doesn't exist. It must have been deleted. It can be created using "Zone Surface panel".
I did not have this issue is my previous (corrupted) model, and I used the same named selection choices/methods, so I am confused on how this happened, and how to resolve it.
Just to see, I ran the transient simulation anyway, and within a few iterations the internal temperature of the blood was equivalent to the ambient temperature of the air. From my time step settings, this temperature change occurred over a few minutes, so I know something is incorrect.
May 27, 2021 at 9:14 amRobAnsys EmployeeYou set the fluids on the cell zones. Face zones (boundary conditions) are for walls etc.
Viewing 7 reply threads
Ansys Innovation Space
- You must be logged in to reply to this topic.
Simulation World 2022
Check out more than 70 different sessions now available on demand. Get inspired as you hear from visionary companies, leading researchers and educators from around the globe on a variety of topics from life-saving improvements in healthcare, to bold new realities of space travel. Take a leap of certainty and check out a session today here.
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.Trending discussions
- Suppress Fluent to open with GUI while performing in journal file
- Heat transfer coefficient
- What are the differences between CFX and Fluent?
- Floating point exception in Fluent
- Time Step Size and Courant Number
- Difference between K-epsilon and K-omega Turbulence Model
- The solver failed with a non-zero exit code of : 2
- Floating point exception
- Exporting Data Results
Top Rated Tags