[briangoesindie]

Hello All, I'm really new to CFD and have been working on it for a class I am taking. The professor gave us a project where we have to work on turbulent convection and we have to use a CFD package. I have never used fluent until this class and the example he did in class was steady so I am struggling to figure out how to do this.

So let me lay out my project quickly and I'll tell you where my problem is.

I am doing a study of convective air flow over a cylinder. It is a problem of cooling the cylinder which has been heated over a short period of time and I want to get data on how much i can cool the cylinder based on air speed in 1 minute.

I have made my meshes in pointwise. Ifirst did a mesh where I have the center circle wall and the fluid flow around it. When I load it into Fluent R16.1 I set the simulation to k-epsilon and the flow speed and temperature and can run the simulation, but I am missing some key data.

So, first, I am unclear how I can set an initial temperature to the cylinder surface. I have seen many posts talking about doing a patch, but I have been unable to figure out how to do this and searching this forum and google(which is how i found this forum) I can't find anything that explains what it is or how to do it. All I have been able to do so far is set a constant temperature which is not what I want in order to see the cooling effect of the flow.

Second, I have been looking around and it seems I can have a 2 part mesh, one for the fluid and one for the cylinder. This seems like more of what I am trying to do.

Can anyone address these two issues? Maybe tell me whether I am right or whether I am going in the wrong direction competely. My professor will not give much assistance whenever I ask him so I am looking outside of class and the tutorials I have been doing for the last few weeks as my project due date is getting closer and I need to get some data for my report. THanks to anyone who can give me a hand.

[LuckyTran]

You need to do a two part mesh (the air flow around the cylinder, and the solid cylinder) if you want to see how the cylinder cools when the air moves over it.

The patch option is in the initialization pane where you setup the initial conditions. It is simply a utility that lets you overwrite specific variables in specific regions.

Create an interface for the solid-fluid interface (the surface of the cylinder).

Setup all materials for the fluid & solid zones. Setup all your boundary conditions and initial conditions. For the solid-fluid interface, use the no-slip condition for velocity and coupled condition for the thermal boundary condition.

Eventually you can start iterating. There are some tricks you can do to solve the problem faster. For example, if you have constant properties everywhere and your velocity field doesn't depend on temperature, then you can solve for the velocity field and then freeze it (by disabling the flow equations). The you can crunch only the heat transfer problem by solving only the energy equation, which can be done very quickly. Do not worry about this part until you've mastered the earlier parts.

[briangoesindie]

Thanks for responding!

I have a two part mesh that I did after doing some reading. Do I create the interface in the meshing software? I made connectors so I have the wall boundary set up at the cylinder surface. Is that sufficient? How do I create the interface?

I doubt I will master any of this before the project is due, but I'm trying.

[LuckyTran]

Originally Posted by briangoesindie

Thanks for responding!

I have a two part mesh that I did after doing some reading. Do I create the interface in the meshing software? I made connectors so I have the wall boundary set up at the cylinder surface. Is that sufficient? How do I create the interface?

I doubt I will master any of this before the project is due, but I'm trying.

Do it in the meshing software. An easy way is to set properties, solid and fluid to each region. Then when you import the mesh into Fluent, the interpreter will figure out there need to be an interface and generate one automatically. It should appear as a wall & shadow-wall combination. If you get the wall & shadow-wall pair then you've done it correctly.

I haven't used pointwise in almost a decade so sorry I can't give immediate help.

[briangoesindie]

Originally Posted by LuckyTran

Do it in the meshing software. An easy way is to set properties, solid and fluid to each region. Then when you import the mesh into Fluent, the interpreter will figure out there need to be an interface and generate one automatically. It should appear as a wall & shadow-wall combination. If you get the wall & shadow-wall pair then you've done it correctly.

I haven't used pointwise in almost a decade so sorry I can't give immediate help.

I set it up like you said right after i replied (Yay! I kinda have an idea of what I should be doing) so I was happy to see I did something right. I set the solid and fluid in pointwise then exported. I didn't see this wall shadow wall unless you are refering to the repeated boundary, which I assume is basically the boundary for the solid and the boundary for the fluid(not sure about the shadow thing you mentioned). I am running a test case based on the little advice I could get out of my professor which was to set the initial temp in the solution initialization screen. I set it to calculate from my solid boundary wall. I am running it for 2500 iterations which will give me .5 seconds to review if it is doing what it is supposed to. I'll let you know...

Let me know if this sounds like I'm doing something wrong.

[briangoesindie]

Originally Posted by LuckyTran

You need to do a two part mesh (the air flow around the cylinder, and the solid cylinder) if you want to see how the cylinder cools when the air moves over it.

The patch option is in the initialization pane where you setup the initial conditions. It is simply a utility that lets you overwrite specific variables in specific regions.

Create an interface for the solid-fluid interface (the surface of the cylinder).

Setup all materials for the fluid & solid zones. Setup all your boundary conditions and initial conditions. For the solid-fluid interface, use the no-slip condition for velocity and coupled condition for the thermal boundary condition.

Eventually you can start iterating. There are some tricks you can do to solve the problem faster. For example, if you have constant properties everywhere and your velocity field doesn't depend on temperature, then you can solve for the velocity field and then freeze it (by disabling the flow equations). The you can crunch only the heat transfer problem by solving only the energy equation, which can be done very quickly. Do not worry about this part until you've mastered the earlier parts.

So I went back and looked at your first response since my case didn't seem to work. I have a solid at one temp and a fluid at another. I can't find this coupled condition you are talking about. Can you expand on this part? The motion part of the case seems to work so far. I am seeing the begining of the Von Karman effect.

[LuckyTran]

If you have two boundaries then you have two isolated regions and they cannot communicate with one another. That means your mesh wasn't done "properly." You can salvage this in Fluent if you can't figure it out in the mesher. But I think you should be able to just specify one zone as solid, the other as fluid, and specify the interface as a "wall" type. Don't specify it as an interface in pointwise.

To salvage it in Fluent. What you can do, is set both zones to the same type (both fluid or both solid). Then merge the surfaces that are redundant so there is only 1 surface for the surface of the cylinder. Then change one of the zone types (from fluid to solid or solid to fluid) so that the zone types are now different. Fluent will then build your coupled wall and generate the shadow-wall.

Once you have this wall and shadow-wall pair. Go to boundary conditions, select your wall, go to the thermal tab and you'll see:

Thermal Conditions
heat flux
temperature
coupled

You want the coupled condition (for both the wall and the shadow-wall).

[briangoesindie]

Well, that's bad. I have emailed my mesh to my teacher and basically begged for some assistance. I really don't understand pointwise, so I'm basically screwed. I tried merging, but it wouldn't do it, so hopefully he can provide some help or I'm probably going to fail. THank you for your help, keep your fingers crossed for me...

[briangoesindie]

Originally Posted by LuckyTran

If you have two boundaries then you have two isolated regions and they cannot communicate with one another. That means your mesh wasn't done "properly." You can salvage this in Fluent if you can't figure it out in the mesher. But I think you should be able to just specify one zone as solid, the other as fluid, and specify the interface as a "wall" type. Don't specify it as an interface in pointwise.

To salvage it in Fluent. What you can do, is set both zones to the same type (both fluid or both solid). Then merge the surfaces that are redundant so there is only 1 surface for the surface of the cylinder. Then change one of the zone types (from fluid to solid or solid to fluid) so that the zone types are now different. Fluent will then build your coupled wall and generate the shadow-wall.

Once you have this wall and shadow-wall pair. Go to boundary conditions, select your wall, go to the thermal tab and you'll see:

Thermal Conditions
heat flux
temperature
coupled

You want the coupled condition (for both the wall and the shadow-wall).

I finally figured out how to make this work. I have the wall and shadow wall. How do I utilize the coupled BC? Do I just leave it blank and set the initial temp in the solution initialization tab?