[CFXer]

Hello.

I'm attempting conjugate heat transfer simulation using porous domain in CFX.

The domains are consisted with hot fluid plate / solid plate / cold fluid plate.

----------------------------
hot fluid plate
-----------------------------
solid plate
----------------------------
cold fluid plate
----------------------------

So, I think the heat is transferred from hot to cold plate through solid plate.

And I used porous domain in hot and cold fluid plate to reduce computing cost.


Hot fluid : CO2 / 8MPa, Tin = 349K
Cold fluid : Water / 0.2MPa, Tin = 298K
Solid plate : SUS316


When I used single pair of these plates, I could get Ideal Temperature variance result as you can see in figure 1.

But when I used multiple pair of plates with total model of heat exchanger (as you can see in figure 2), the temperature result is too weird.(figure 3)

I think this result is impossible because it means it has very high heat transfer rate in inlet section.

So, I beg you an opinion of this simulation.

I used completely same domain setting and heat transfer coefficient, porosity setting with single plate and total model of heat exchanger.

Thank you in advance.

[ghorrocks]

How does modelling this with a porous model reduce computing cost? Why not just model it with normal CHT fluid and solid domains? The error you are seeing is likely to be interface conditions at he porous boundary.

So I recommend you just model this with normal solid and fluid domains, and no porous domain.

[CFXer]

Originally Posted by ghorrocks

How does modelling this with a porous model reduce computing cost? Why not just model it with normal CHT fluid and solid domains? The error you are seeing is likely to be interface conditions at he porous boundary.

So I recommend you just model this with normal solid and fluid domains, and no porous domain.

To use fluid domain, I need over than 1 million nodes to get a reliability.

So, by using the porous domain, I can calculate the pressure drop as a correlation with less node number.

So I can reduce the computing cost.

I cannot simulate fluid/solid simulation because of computing cost..

[ghorrocks]

One million nodes is quite a small simulation and easily manageable in CFX. I regularly do simulations many times bigger than that. Sounds like you should consider doing the full fluid/solid model.

Can you show an image which shows how you are modelling these plates with a porous domain?

Regarding your question: If you look under the porous model (I think there is an advanced solver option for it in the solver tab) there are options to adjust the porous domain numerics. You might need to adjust this to reduce that strange glitch at the start of the porous domain.

[CFXer]

Originally Posted by ghorrocks

One million nodes is quite a small simulation and easily manageable in CFX. I regularly do simulations many times bigger than that. Sounds like you should consider doing the full fluid/solid model.

Can you show an image which shows how you are modelling these plates with a porous domain?

Regarding your question: If you look under the porous model (I think there is an advanced solver option for it in the solver tab) there are options to adjust the porous domain numerics. You might need to adjust this to reduce that strange glitch at the start of the porous domain.

I'm sorry I miswrite the number, not a million actually over 100 million.

I uploaded a figure of how I consisted mesh in the porous domain.

And as you said that, I did step by step calculation start with only porous domain.

The result is, the problem is header side.

As you can see in the original post's figure, there are semicircular shape header, and it is a fluid domain in CFX.

When I made a mesh of this, I firstly made half of its shape, and make a symmetry shape to make a full semicircular header.

Could it have a problem with a symmetry step? I cannot understand..

[ghorrocks]

In your first post you show lots of plates in one of your images. Can you show how these plates are arranged? What is a porous domain, what is fluid and what is solid?

[CFXer]

Originally Posted by ghorrocks

In your first post you show lots of plates in one of your images. Can you show how these plates are arranged? What is a porous domain, what is fluid and what is solid?

It is consisted of

solid
hot porous
solid
cold porous
... x7

like this

[ghorrocks]

How does modelling the fluid domains as porous mean you can use a coarser mesh?

[CFXer]

Originally Posted by ghorrocks

How does modelling the fluid domains as porous mean you can use a coarser mesh?

Yes it is.

Porous domain uses friction factor correlation to calculate pressure drop.

So, even it is consisted of fewer meshes, it can calculate the pressure drop with lower number of nodes.

I already tested it with experimental result, in case of isothermal condition.

So, the remain problem is only about heat transfer condition.

[ghorrocks]

So you are using the porous resistance to represent the pressure loss due to the boundary layer in the fluid?

But isn't the heat transfer from the fluid to the plate controlled by the boundary layer? So if you are not modelling a boundary layer isn't your heat transfer completely wrong?

[CFXer]

Originally Posted by ghorrocks

So you are using the porous resistance to represent the pressure loss due to the boundary layer in the fluid?

But isn't the heat transfer from the fluid to the plate controlled by the boundary layer? So if you are not modelling a boundary layer isn't your heat transfer completely wrong?

Maybe it could possible..!

Although the porous domain has a "heat transfer area density" and "heat transfer coefficient" setting, It is just about the correlation.

Plus, when I tested the single plate, the inlet velocity is completely normal to inlet boundary.

But when the inlet header exist, the velocity component in porous domain should be various.

When the inlet header exist, the wall setting is automatically changed to no slip wall, this case shows very good result in heat transfer but not in pressure drop.

So, to consider thermal boundary layer, can I add thin material option between porous and solid domain interface?

I think the zero-thermal boundary layer makes its heat transfer rate too high, so I think the thin material option could be help.

How do you think about it?

[ghorrocks]

If you could accurately predict the pressure loss and heat transfer using a simple correlation then why would anybody bother with CFD? You cannot do it, and that is why CFD uses fine meshes to resolve this sort of thing.

There is no simple function you can define which will accurately model heat transfer in your case. It is a complex function of velocity, development length, surface condition, temperature gradient and many other factors. The only way you are going to accurately model this is to actually model it with the physics which is there.

But before you model this with the correct physics (the fluid modelled as a fluid domain and the solid modelled as a solid domain) - can you tell us why you are doing this model? What are you trying to learn? If we know the purpose of the work then we can make informed suggestions.

[CFXer]

Originally Posted by ghorrocks

If you could accurately predict the pressure loss and heat transfer using a simple correlation then why would anybody bother with CFD? You cannot do it, and that is why CFD uses fine meshes to resolve this sort of thing.

There is no simple function you can define which will accurately model heat transfer in your case. It is a complex function of velocity, development length, surface condition, temperature gradient and many other factors. The only way you are going to accurately model this is to actually model it with the physics which is there.

But before you model this with the correct physics (the fluid modelled as a fluid domain and the solid modelled as a solid domain) - can you tell us why you are doing this model? What are you trying to learn? If we know the purpose of the work then we can make informed suggestions.

Understood.

I'm trying to simulate "Printed Circuit Heat Exchanger(PCHE)" with large scale.

PCHE is consisted of plate with millimeter-scale channels, and large scale PCHE is consisted with over 40,000 channels.

Almost every PCHE simulation papers used periodic condition and calculate single pair of hot/cold channel, because they cannot use fluid domain in large scale.

So, to calculate the large scale PCHE, I'm using porous domain to calculate dP and heat transfer performance effectively.

Porous domain is consisted with
volume porosity : calculate inner velocity
Loss model : flow direction setting
Resistance Loss Coefficient : pressure drop correlation (Friction factor)
Fluid Solid Area Density : Surface area setting (Heat Transfer)
Fluid Solid Heat Transfer : Heat Transfer Coeffieicnt setting (Nusselt number input)

Until this time, I confirmed the isothermal condition shows great result.

But the isothermal condition is not an actual condition, so I have to simulate heat transfer condition.

[ghorrocks]

You have not told us why you are doing this model. Are you trying to optimise the design? Or test a new design concept? Or find why some device is not working as expected?

What flow domain is in the channels? Is it fully developed laminar flow, laminar boundary layer, transitional flow or fully turbulent flow?

What porous domain model are you using?

[CFXer]

Originally Posted by ghorrocks

You have not told us why you are doing this model. Are you trying to optimise the design? Or test a new design concept? Or find why some device is not working as expected?

What flow domain is in the channels? Is it fully developed laminar flow, laminar boundary layer, transitional flow or fully turbulent flow?

What porous domain model are you using?

I'm doing this model to test real scale heat exchanger.

To do that, I firstly doing small scale (lab-scale) model, so in this scale I doesn't optimise a design because to test a real model.

In channel, they are consisted of plate, and the flow Reynolds number is about 18000, fully turbulent flow.

Because of above reasons, now I'm trying to calculate the full domain.

[ghorrocks]

Do I read that you are doing the full-scale model now, which has fully turbulent flow in the channels? Are you modelling this with the porous domain, or with a normal fluid domain?

[CFXer]

Originally Posted by ghorrocks

Do I read that you are doing the full-scale model now, which has fully turbulent flow in the channels? Are you modelling this with the porous domain, or with a normal fluid domain?

Sorry for your confusion.

There are totally 3 domain parts.

Inlet header is fluid domain
Inner core is porous domain,
and Outlet header is fluid domain.

Actually core part has fully turbulent flow, but in porous model it shows same velocity as the real fluid.

But it doesn't show thermal or momentum boundary layer because it uses free slip wall condition.

[ghorrocks]

OK, so we circle around to the point I made before. How are you going to model the heat transfer accurately when the approach you are using does not generate a boundary layer?

The boundary layer is critical to the heat transfer, so you need an accurate boundary layer model if you are going to get the heat transfer correct. Therefore you need to use a fluid domain for the fluid, with a mesh adequate to get the boundary layer accurate enough.

This may well make your simulation too big to be viable. Your options are then:
1) Get a bigger computer - try AWS
2) Network more computers together and run distributed parallel
3) Run it anyway and let it run for days - my longest CFD run took 6 weeks to complete
4) Tell you supervisor the simulation is not possible with available resources
5) replace the problematic section with a simplified model which contains all necessary physics but is simpler than CFD (note: all necessary physics, not just some of it) - this approach requires good knowledge of physics and numerical methods.

[CFXer]

Originally Posted by ghorrocks

OK, so we circle around to the point I made before. How are you going to model the heat transfer accurately when the approach you are using does not generate a boundary layer?

The boundary layer is critical to the heat transfer, so you need an accurate boundary layer model if you are going to get the heat transfer correct. Therefore you need to use a fluid domain for the fluid, with a mesh adequate to get the boundary layer accurate enough.

This may well make your simulation too big to be viable. Your options are then:
1) Get a bigger computer - try AWS
2) Network more computers together and run distributed parallel
3) Run it anyway and let it run for days - my longest CFD run took 6 weeks to complete
4) Tell you supervisor the simulation is not possible with available resources
5) replace the problematic section with a simplified model which contains all necessary physics but is simpler than CFD (note: all necessary physics, not just some of it) - this approach requires good knowledge of physics and numerical methods.

I'm using heat transfer correlation like Gnielinski or Dittus-Boelter correlation.

I think they are modelled including thermal boundary layer of the pipe.

So I thought it is okay to use heat transfer correlation with porous domain even if it doesn't have thermal boundary layer.

[ghorrocks]

Both of those correlations are for flow in tubes, not flat plates. You should be careful about whether they are applicable to flat plates.

Also, for the interface conditions between your fluid and solid domains in CFX, the heat transfer model options you have are conservative interface flux, thermal contact resistance or thin material. You could also put a source term on the interface. How are you proposing to use the Nusselt Number given by those correlations with the available CFX heat transfer interface models? There is no option where you can select Nusselt Number or heat transfer coefficient. (Hint, if you have not worked it out already: the thermal resistance of the interface is 1/h, so you could use the thermal resistance option)