July 19, 2023 at 2:00 amVanessa PatinoSubscriber
Hello, I posted about a different version of my problem in the past but the the water was static there.
I would now like to simulate the flow of water throughout a glass chamber with a silicon wafer placed inside as the heat source (a transient thermal analysis). I understand you're not meant to mesh the container normally for fluent problems however I would like to see the chambers temperature change after the water heats up from the silicon wafer. Is it possible to do so and is it too overly complicated that I should just focus on the temperature change of the water (and not mesh the container)? Let me know if this description makes sense.
I've been learning purely from YouTube tutorials and online forums but I feel like my knowledge is still lacking. The videos that I've been using a lot for this areand &t=914s. Whlie these vodeos are very helpful they don't showcase all the things I need for my analysis. A 3D Multiphase VOF model and Conjugate heat transfer from a heat source. I'm sturggling to see the convective heat transfer between the silicon wafer and the wafer.
I understand my questions are broad and I apologize there is just so much that I feel needs to be thought through for this analysis to work. I want to see the temperature change of the wafer, chamber, and the water. I would like to see how the particles move in the chamber. Is there something I need to think of for this problem that isn't obvious in the problems of the videos I provided?
July 19, 2023 at 8:03 amNickFLSubscriber
When building a model, it is always important to identify what you know. Then we can try to identify what physics need to be included in the model. Based upon the comments above, this is what I gathered:
- You have a volume that is filled with water. Do we know the temperature and flow rate of the incoming water?
- Inside we are cooling a silicon wafer (or heating some water if you want to take that perspective). Do we know the surface temperature of the wafer (this might be the information you are trying to get from the model)? Or are we going to give it a certain heat generation? What do we know here?
- What is a rough estimate of the maximum temperature of the fluid? Yes this will be output of the model. But if the temperature never exceeds the boiling temprature, we can avoid using a costly VOF model.
For your questions:
- I understand you're not meant to mesh the container normally for fluent problems however I would like to see the chambers temperature change after the water heats up from the silicon wafer.
Do you mean the glass container which holds water? Do you expect there to be significant heat transfer into this body? If you want to see the temperature inside this solid body, then we will have to model it. But if we are interested in what is the temperature of the water and the primary heat sink is water leaving the domain, then we can leave it out.
- Is it possible to do so and is it too overly complicated that I should just focus on the temperature change of the water (and not mesh the container)?
We can model a lot with ANSYS. Deciding on how to build a model begins by identifying what we know, the relevant physics and the desired outputs of the model. Then we have to take into account the computational resources we have and the deadline we have to complete the project. We are still gathering so we cannot say.
- I'm sturggling to see the convective heat transfer between the silicon wafer and the wafer.
Fluent does not differentiate between convective & conductive (well except when we are specifying the boundary conditions). It is solving the energy equation. What output are you using to see the convective heat transfer?
July 19, 2023 at 7:17 pmVanessa PatinoSubscriber
Thanks so much for responding!
Do we know the temperature and flow rate of the incoming water?
Yes, both of these are known and I included them in my setup.
Do we know the surface temperature of the wafer (this might be the information you are trying to get from the model)? Or are we going to give it a certain heat generation? What do we know here?
Ah yes, sorry about that I forgot to mention it. Yes the wafer is set to 65 C, in one of the videos they patched the temperature for their heat source while I've just been setting it 65 C in the boundary conditions... I'm guessing the former is actually correct?
What is a rough estimate of the maximum temperature of the fluid? Yes this will be output of the model. But if the temperature never exceeds the boiling temprature, we can avoid using a costly VOF model.
I believe the water reaches around 80-90 C so just before boiling, does this mean I shouldn't use VOF? What am I using then? Do you mean its not longer a multiphase problem?
Do you mean the glass container which holds water? Do you expect there to be significant heat transfer into this body?
Yes the glass container that holds the water, there is also a glass 'top' that dips into the container taking up a considerable amount of space. The bottom portion of the top sits right above the wafer inside the container. Like a container inside the container but the inner one is actually connected to a top that sits on top of the container... (I hope this makes sense). I do expected there to be a significant amount of heat transfer since a portion of the top sits right about the wafer, I am also intersted in the heat transfer of the inside walls of the container.
What output are you using to see the convective heat transfer?
Could you elaborate a little more on this. Do you mean how am I looking at the results? If so I'm looking at the temperature contours and volume fraction of the water phase.
July 19, 2023 at 7:34 pmNickFLSubscriber
- Why do you expect the water to be 80-90C if the wafer is 65C? Are there other sources?
- Are there multiple phase or fluids where we need to keep track of the interface between them? That is what the VOF model is good for. If not, and we have just liquid water, then we do not need VOF.
- If you want the temperature distribution in the glass, then you will need to include it in the model. The solid will not have to have such a fine mesh as the fluid domain as it is only solving conduction here.
- In your first post you mentioned that you were not seeing convection. My question was related to how you were judging that. To me, the first place I would look would be the temperature field.
EDIT: I would really recommend that you work through the exhaust manifold tutorial. Don't focus on the meshing part (unless you plan on using Fluent meshing), but understand the basics of setting up the model and the theory behind why we chose what we chose.
July 19, 2023 at 8:13 pmVanessa PatinoSubscriber
Why do you expect the water to be 80-90C if the wafer is 65C?
Well there are in person experiments going on but the conditions are different the heat source is not the wafer but an external light. Giving it an actual second thought my temperature range of 80-90C is an overestimate, it would probably be closer to 50C maybe... I wrote a longer explanation but the page reloaded and it was deleted so let me know if this is fine.
Are there multiple phase or fluids where we need to keep track of the interface between them?
The container itself is not filled to the top with water. It'll be about 65% water and the rest air. I would like to see the convective heat transfer between the water and air.
The solid will not have to have such a fine mesh as the fluid domain as it is only solving conduction here.
Makes sense but is it that important that the fineness of the mesh is different between solid and fluid bodies or is it just for processing sake?
To me, the first place I would look would be the temperature field.
So the temperature field is different than the temperature contours?
work through the exhaust manifold tutorial. Don't focus on the meshing part (unless you plan on using Fluent meshing), but understand the basics of setting up the model and the theory behind why we chose what we chose.
Will do, I'm glad you guys go over the theory lots of tutorials don't actually explain why they chose x option. I actually only ever mesh in Fluent meshing, it seems the easiest since it's the next cell after geometry.
July 20, 2023 at 6:40 amNickFLSubscriber
Like Rob said below, start will small simple models and then slowly add the complexity. You also need to do some hand calculations to see where the thermal energy is going. That will give us an indication of how much heat is transferred at the water outlet, into the solid glass and into the air. Our first model should include only the important parts, so the hand calculations will help us identify which ones are important. (Plus we spent a lot of time learning all this in the University, we should probably use it.)
It sounds like you are using Workbench. The meshing can be in the Fluent application (Fluid Flow with fluent meshing) or in ANSYS meshing (Fluid flow Fluent) depending on the Analysis System you selected on the project page. If you use the former, the tutorial meshing step would also be helpful.
Tutorial is here: https://ansyshelp.ansys.com/account/secured?returnurl=/Views/Secured/corp/v232/en/flu_tg/flu_tg_exhaust_manifold_cht.html
July 19, 2023 at 8:10 amRobAnsys Employee
Break the problem down into pieces. There won't be a tutorial covering every model combination as we'd run out of space to store them.... It's also (usually) easier to troubleshoot problems with less physics - there are less options to try and understand.
Get rid of the VOF and solve the single phase conjugate heat transfer problem. How are you setting the initial wafer temperature? Does that heat transfer to the fluid? I assume you did split the wafer volume out of the larger domain & then share topology?
Do a couple of VOF tutorials to see how that works. Decide how you want the boundary conditions to apply to your wafer box.
Once you're happy with both of these models turn them both on. How hot is the wafer relative to the liquid boiling point?
July 19, 2023 at 7:35 pmVanessa PatinoSubscriber
Hi Rob, thanks for your reply!
So this is not a VOF problem or are you saying I should break it down to not be a VOF problem.
How are you setting the initial wafer temperature?
I'm setting the intial wafer temperature in the boundary conditons, I created a named selection for the surface of the wafer and named it heat source and there I applied the temperature to the wall adjacent to the solid domain. From what I saw in one of the videos though, patching your heat source temperature is the correct way?
Does that heat transfer to the fluid?
Have I seen that heat transfer to the fluid? No. But I would like to.
I assume you did split the wafer volume out of the larger domain & then share topology?
Short answer is no. When I import the model into DM there are 3 bodies 3 parts: the Si wafer, container body, and top. I created a fluid domain by creating surfaces at the inlet and outlet and using the Fill tool. I now have 4 bodies 4 parts, I wasn't exactly sure if I should keep the fluid domain its own part and make the rest one part or if it should all be 1 part but 4 bodies. The videos I watched did different things at this point. I decided to just make 1 part with 4 bodies. What should be its own part, everything? I thought this was just to help ansys do the interfaces for you.
Once you're happy with both of these models turn them both on. How hot is the wafer relative to the liquid boiling point?
By both of these models you mean do a single phase conjugate heat transfer model and a VOF model but don't include the heat transfer?
Thanks again for the reply, you are all very helpful!
July 20, 2023 at 7:46 amRobAnsys Employee
For the solid, you can either ignore it and set a heat flux or temperature on the surface to the water. Or, include the solid and set a heat source to that zone. Both are valid, but you need to understand what each does.
At the temperature you're saying, you can neglect boiling. Just keep an eye on the temperatures.
Echoing Nick's comment. Whilst you want to see the air flow, run the first case full of water to see what's going on. It'll be steady state and run in an few hours (mesh & cpu dependent). VOF will be transient, and could take several days to give a stable-ish result.
You noted a lack of buoyancy. Did you set the density to be temperature dependent? Is gravity on? The steady model is a really good way to find all your problems, omissions and any mistakes as it'll go wrong/show silly values very quickly. You don't want to be waiting days to find you missed, or didn't think of, something.
July 21, 2023 at 8:44 pmVanessa PatinoSubscriber
Do I need to create a UDF to set density to be temperature dependent? Or is it much easier than that and I'm missing it in the physics set up somewhere? Yes gravity is on.
So just do multiple steady state calculations, okay makes sense. Thank you.
July 23, 2023 at 3:36 pmNickFLSubscriber
The density can be set under the materials in the tree. Move down to the material used in your simulation and double-click to open the properties of the material. For water, this is set to a constant by default. You could simply change this to be a function of temperature.
The density changes from room temperature water to 100°C only change by 4% or so. Think about your model. If you have forced convection, is it necessary to include this small change in the density? If there is no externally forced motion, then this density change is more important. In the first stages of building the model, we try and keep only the most important parts. The secondary effects we can include in later versions of the model.
- 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.