Hi all,
Actually I was wondering if anyone could help me by modeling zero-thickness walls in ANSYS Fluent (CFD). My model is a wall with a cavity inside, and I need to mesh the air-gap inside (to evaluate the heat convection). I already modeled the geometry in SOLIDWORKS (with walls coming with thickness) and do not know how to model this problem.
Please help me what you think.
Sincerely,
As ANSYS employee, we can not download the attachments. Can you please insert some images.
You may want to look at following video
Hi Moda,
I looked at your iges file. It looks like you have all the solid bodies shown in the left image that has two glass panes and a set of insulators and the air that is enclosed in this space in the image on the right.
I believe this is sufficient to build a FLUENT model.
Regards,
Peter
Dear Peter,
Thank you so much for verifying my model. However, the problem is that I'm not able to mesh the air-gap! I know clearly that I should define the air-gap, but don't know how to do it. Basically, in the setup mode, I'm not able to define it as air wall (as ANSYS just accept solids as walls). In other words, I'm not sure how to model the air-gap as an air domain; while the material drop list is just including solid materials(attached)!
Also, I was wondering if you could do me another favor and show me how to generate any wall as a zero-thickness wall. When I modeled my geometry in Solidworks, there was no way to draw the walls as zero-thickness walls, and I assume it should be a way to define them as zero-thickness ones (either in geometry/mesh).
I really appreciate your help in advance.
Sincerely-bc.jpg?width=690&upscale=false)
,
Dear Moda,
I don't understand what you mean by an air-gap. Please create an image that points to it with an arrow, and Insert that image in your reply. Please also describe the Boundary Conditions for this problem. It looks in the image above that you want to apply a temperature to one face of the glass. I expected you would define Convection instead.
In the image I provided on the right, that solid body is the air. It exists in the "gap" between the panes of glass and the solid insulators. I can mesh the air solid body in Meshing, then in Fluent, I can define the domain to be a fluid called air, which is available in the library.
When you first open the iges file in SpaceClaim, you should set the assembly to use Shared Topology. That will simplify the appearance of the model in Fluent because in Meshing, it will not need Contacts that show up as Interfaces in Fluent. Instead, nodes will be shared at common faces between bodies.
Regards,
Peter
Dear Peter,
Thank you so much for your explanation. I followed your instruction in adding a photo with more details on. Basically, two of my glass plates have constant temperature BC, while in the middle, I've cavity (air-gap) -showed by red arrows- with convection BC.
Can you please explain to me how did you define the air domain to be a fluid called air, as it only shows me solids materials in my BCs (attached)!
Thank you so much for letting me know about Shared Topology. It was really super helpful to me, helped me to get rid of so many useless BCs.
I really appreciate all your time, help, support, and consideration.
Sincerely,
.jpg?width=690&upscale=false)
-bc-li.jpg?width=690&upscale=false)
Dear peter,
I tried Shared Topology in SpaceClaim (attached). However, still suffering TOO MANY BCs (attached), including interiors, shadows, and contact regions! Would you please give me a hint? I really appreciate it!
Sincerely
For defining air, you need to use cell zone condition.
With contact region, it looks like sharetopology is not applied correctly in spaceclaim.
Check following video
Or you can do sharetopo in DM.
Dear Peter,
I', still in trouble to mesh the air cavity. I tried to simplify my model as much as possible. This is why I created a geometry of a hollow box, included with a cavity (attached). Now, I was wondering if you could do me a favor by helping me with the following:
I really appreciate all your help.
Sincerely,
Dear Moda,
If you don't want to model the temperature change through the glass thickness and want to just assume that it is constant, then Exclude from Physics the glass solid bodies. That means you just apply the constant temperature to the face of the body that is the air directly.
You have explained all your BCs except for the faces on the Insulators. If they are perfect insulators, then Exclude from Physics all of those bodies as well. All you will have left is the air body. Any face that does not have an explicit BC defined is automatically adiabatic (I think). Certainly every face of a fluid domain is automatically a wall unless an explicit BC is defined.
In Meshing, you should create Named Selections for each face that you want to apply a BC to such as FrontTemp, BackTemp, LeftConv, RightConv. Those names will be available in Fluent to make creating the BCs a little easier.
I would be happy to look at your geometry if you attach a Workbench Project Archive .wbpz file to your reply.
Regards,
Peter
Dear Peter,
I really like to attach my geometry. But supposedly, there is no way to attach a file anymore. Can you please let me know how to attach a file? Is there anyway to chat online?
Thanks
After you post, the Attach button appears. Take a look at the post you just made and attach the .wbpz file to that. Note, it's not the .wbpj file.
Thanks. Would you please let me know how to get the .wbpz file? ANSYS saves as .wbpj!
Sincerely,
BTW, I'm still struggling how to define different surfaces in my model?!! It just shows me an entire box! I really get stuck stuck into this problem geometry/meshing!
Moda, please click on the text in blue. It is a link to instructions on .wbpz file creation. Basically, File, Archive...
Also, please say what film coefficient and ambient temperature for the convection surfaces and the temperature for the constant temp surfaces.
Hi Moda,
I opened the 30.iges file from your first post. I had to repair it by using Sew in SpaceClaim.
Mechanical might automatically create Contacts in the Connections folder. Just go in and suppress them.
Here is a first attempt at a mesh. It needs a lot more work to get high quality elements, but this mesh is swept from one end to the other.
Since the five wedges on the right don't have any common area where they touch their neighbors, and since the three faces are: one constant temperature and two adiabatic, I don't see any value in making them have any shared topology or interface conditions. Aren't they just independent air wedges that have no influence on the large air cavity to the left? In that case, there is no need for Shared Topology. Solve one wedge and you have the solution for them all.
Regards,
Peter
A better mesh...
I had to do another repair, this time Simplify. I see how fragile the import process is.
Regards,
Peter
Here is the mesh in Fluent.
Attached is an ANSYS 19.1 Workbench Project Archive. Use File, Restore Archive.
Regards,
Peter
I want to know what is needed to solve this model correctly. I expect gravity has to be turned on and the temperature dependent density of air has to be present in the model. I don't know if that is there already or has to be added. Those are questions I hope the CFD experts can answer. I ran out of time to edit the video to take out the waiting time.
Regards,
Peter
Normally you'll want gravity (remember to set the vector to down!) and in Fluent I'd suggest incompressible ideal gas for density. There are also some considerations for the external boundaries to stop the air "falling" through the domain. Where does the heat come from? I may have missed that in the thread.
Thank you so much for your clarification. Basically, there is a heat source- that makes the internal wall getting warm. As a result, I assumed that surface is constant temperature- which is accurate enough for my test.
Dear Peter,
First of all, please accept my sincere appreciation for all your time and consideration. Honestly, it was much beyond than my expectation and really super awesome! Thanks!
However, I still have a question on heat convection that occurs inside the wall. Please let me clarify: what you did for external convection (as convective BC) was totally correct. BTW, we still must model the convection that happens inside the wall (between two glass walls, and also inside each of those 5 wedges- at least the main air domain inside the wall (not those wedges)), as it really matters for my research. Any idea about this part?
Also, I was wondering if you could let me know about those repairs that you made it by using Sew in SpaceClaim?
Thanks again for all your support.
Sincerely,
@rwoolhou, this is a closed box, though the images above didn't show that. Using an ideal gas, as the temperature increases, the pressure will increase in the fixed volume. Does a fixed volume change your suggestion for using incompressible ideal gas for density? Is Pressure-Based solver appropriate, or would the Density-Based solver be better? I'm guessing Density, but correct me if I am wrong.
Dear Moda,
The body called air is meshed as a fluid for the Fluent solver, which means that each cell has a temperature, pressure and velocity vector computed as part of the solution. As I suggested, and rwoolhou has confirmed, gravity must be turned on.
With gravity turned on, natural convection will develop in the solution by heat transfer to the air near the wall, reducing its density. Gravity will pull the colder, heavier air in the center down, which pushes the warmer, lighter air near the wall upward. That means you have to edit air and change density from a constant, to ideal-gas or something else as suggested by the experts.
So in the steady state solution you can plot the upward velocity of air near the wall, while there would be a downward velocity in the center creating a big swirl pattern. With the above settings, it will take more than 1000 iterations to converge.
Here is a slice at x=40mm through the volume plotting the Y velocity component in cm/s
I would be interested to run a Transient solution and see the still air begin to flow to better visualize the convection, but that takes longer to compute than the steady-state solution.
Regarding the 5 wedges, since they have no connection to each other or to the main air cavity, they all will behave identically, so you can just mesh one wedge to see what happens in any wedge.
You can show your appreciation by clicking Like below the posts that are helpful. If your original question on zero thickness walls has been answered, you can click Is Solution on the post that best answered the question. Open a New Discussion to ask about computing Natural Convection. You can use a link in that new post to point back to this for background.
Regards,
Peter
Dear Peter,
I went through all your assumptions. It was really helpful to me. Thanks! How you modeled the air domain was perfect. Thanks!
Meanwhile, I'm going to model wedges as well as insulators. I don't think disregarding the insulators/wedges would be a very accurate idea- as insulators are not perfect insulation (small heat flux). Also, if I suppress the physics of wedges, it will cause heat escape! Also, my advisor asked me to evaluate two glass plates (still constant temperature, but different temperature on each side- as we consider conduction), in order to evaluate impacts of replacing the glass walls with other materials.
Now, I was wondering if you could help me by the 2 following questions:
I warmly appreciate all your considerations.
Sincerely,
Dear Moda,
What conductivity are you assigning to the insulators? What interface resistance are you assigning to the contact between the insulators? If you don't have any extra resistance between the insulators, you should just unite the six solids into a single body. That will get rid of a lot of extra contacts in the model.
You defined RightConv (and LeftConv), but you didn't pick all the faces that are exposed to the convective cooling on that end.
Inflation is useful when there is a high gradient, usually in velocity, but in this model, in temperature. I suggest you only put inflation on the air faces that touch the glass. If you are sweeping, then you can use a sweep bias to put smaller elements near the convective surfaces.
The wedge could use smaller elements than the large cavity.
I noticed you upgraded to ANYS 19.2 since your first post. Attached is my changes.
Please start a New Discussion for new questions as this topic is solved.
Regards,
Peter
Thanks. I created a new discussion as
Here is the link: https://studentcommunity.ansys.com/thread/how-to-define-boundary-conditions-for-my-complex-model/?postbadges=true
Thanks,
abenhadj
112
peteroznewman
106
rwoolhou
93
kkanade
52
FlaviaGelatti
40
jj77
32
tsiriaks
25
EngineerMech
24
Max4
22
SandeepMedikonda
14
