Louvered Fin Incorrect pressure Drop

[ankit.khurana]

I am tring to find the pressure drop as air flows over 1 convulation of louvered fins.
experimentally the pressure drop comes out to be 450Pascals at an inlet velocity of 8m/s
For CFD Simulation, i created an external volume
The inlet side extends to about 1.5 times fin depth and the outlet side extends to 0.8times fin depth.

The boundary conditions applier by me are 
Inlet Velocity : 8m/s

Outlet Pressure: 0Pa (gage)

slip/symmetry conditions were applied to two of the sides of the external volume (the one which is almost parallel to the fin plane, i.e. the one having more width)
Now exmaining the result

pressure at inlet of external volume : 210Pa

pressure at outlet of external volume: 0Pa

This is not in agreement with the experimental Data.Could anyone tell where I am going wrong?
I couldnt upload the CFDfile as the system on which cfdesign is installed has no net connection as it contains propriety patented designs

Eagerly looking forward to some response

[marco.mueller]

I'd change the inlet/outlet dimensions. Also probably the mesh is too coarse and you could try to use SST k-Omega model and ADV5.

[ankit.khurana]

The mesh isn't too course for sure. I refined it considerably. From the
original 3 million elements from auto sizing I refined it to increase the
element count to 12 million. Could try increasing the extremal volume.
One more problem I'm encountering is that the external volume isn't
completion enclosing the fins on the other two sides (not the inlet ,
outlet side). There is a slight gap between the external volume and the fin
due to which free flow is taking place.

[ankit.khurana]

I'm on cfdesign 2011. It doesn't have adv5, I should use adv2 instead, right?
I dont thibk it has the SST k-Omega model as well. What should I use instead of that?

[srhusain]

You might try Adv2 and the eddy viscosity turbulence model with a turb/lam ratio of 10. If the solution is is still unstable, try a ratio of 100.

Hope this helps.

[ankit.khurana]

It didnt help. The pressure is still much lesser than expected

[srhusain]

Is it possible for you to update to the latest version of SIMCFD (V2015)?

[apolo_vanderberg]

The mesh is not about the number of elements.

When you quote 3M or 12M elements, is this from the Mesh Estimator (on the mesh dialog), or fro the Output Bar / Status file?

If the former, this may not be the actual element count, check the output bar or status file for the actual element count.

Now there are models where 3M is very coarse as it is not about the number of elements but where and how those elements are used.

For your model, through the flow passages what does the mesh look like, how many elements do you have across the gap?

Based off your comment, the pressure you are expecting, how is that lab test configured? Does it allow bypass flow as you mentioned you have in the CFD model? If not, you will need to modify the geometry to prevent this

[ankit.khurana]

Well I did refine the mesh further. started having meshing issues so had to fine tune the geometry in CAD then used the edge removal tool in CFDesign to remove edges less that 7degrees(6 in total). I made the mesh fine and also locally controlled the mesh in and around the fin. My results are much more accurate now. A max error of 10% and a standard deviation of 4% whichis really good.
Now I have two problems
1)As the velocity increases, the error is increasing. this is due to free flow occuring.(PIC ATTACHED). how do i modify the geometry to take care of this?It doesnt let me make the external volume any narrower.

the second one I'll post as soon as im able to get a screenshot of what I want to explain

I want to thank you all you have been very helpful. My boss was very impressed with the agreement of the CFD results with experimental data. I also told him about the help I got from here

[ankit.khurana]

hey
i attaching 2 photos of the mesh i had used before which helped me get down the max error to 5%

Now here is my second problem

Now i have to deal with heat transfer

along with the fins, i have attached 2 tubes on each side(Shown in CAD model) (p.s. I will be using only 2 fins and not 4 and will accordingly adjust the CAD model)
the tube are hollow

I have created internal flow volume for the tubes( highlighted in the pic)

I have created an external flow volume also (pic attached)

I will be applying slip/symmetry condition on the side which is highlighted in the above external volume pic. I will also apply slip/symmetry to the side directly opposite to it

Im going to apply aluminum to the fins and tube

Water to the inter volume (through the tube)

Air(fixed) to the external volume

Now the boundary contitions

Inlet Air(external volume) : velocity 8m/s, temperature 45Degrees celsius

Outlet air(external volume): pressure 0Pa(gage)

inlet of the water in tubes (internal volume, total 2 of them 😞 velocity 1m/s, temperature 98 degrees celcius

outlet of the water in tubes (internal volume, 2 of them): Not sure: need help on this

Now i want to calculate the temperature of air at the outlet as gets heated due to the fins.

I also want my analysis to consider the effect of choke

That is, if i reduce my fin pitch (distance between the 2 fins) to an insanely small value, the temperature rise of air should be more (instead of less) as due to closely placed fins, the flow of air is choked (probably due to two boundary layers impringing with each other causing further obstruction to flow). How do I take care of this.

Should i use the same solving conditions, i.e. ADV 2 and eddy viscosity (ratio 10) or anything else

Thank you in advance


p.s. The rest of the pics I Am attaching in another post 

[ankit.khurana]

I have attached the remaining pics.

[ankit.khurana]

Update :
I had created internal volume (inside the tube) and tried to define it as water.
Since this lies in the external volume I created, I got an error that 2 dissimilar fluids are being mixed. I now changed the material of the internal volume from water to aluminium and supressed it. I now selected surace selection mode, selected the outer surface of the tube and assigned a temperature of 98degrees to it. Rest is all same

[ankit.khurana]

Hey
I had done analysis of 17mm fin depth (along direction of air flow)
Today my boss comes up to me and tells me that by mistake he gave me the experimental result of 48mm fin depth instead of 17mm fin depth. He further added that the pressure drop for 17mm fin depth should come out to be around 120Pascals. My answer using adv2 and eddy viscosity (ratio 10) is coming 430Pascals and using the default settings comes out to be around 240 pascals.

Please guide me as to what I should do.

[apolo_vanderberg]

Take a large step back.

How is your test setup configured? What does teh test lab look like, what sized duct is there? Note that Ext. Volume from CFD cannot be co-planar with geometry (this is outlined in the help) so there will always be a leakage path. If this should not be the case, Build your wind tunnel in CAD and import it with the rest of the geometry.

I would be running K-epsilon or SST rather than manually selecting a given Tubr/lam ratio with Eddy Visc.

To match test resutls you need to be sure we are matching constraints and assumptions as to how and where we are taking measurements

[ankit.khurana]

A very large step back indeed. The test is conducted by our technological joint venture company in Japan whereas I'm In India. I havent looked at the test lab but they conduct the test for the entire radiator. A standard size radiator is used which perfectly fits into the duct. I wont be able to model the full hear exchanger due to hardware limitations, that is why I am working on one fin convolution. The properties it exhibit should be similar. I've read research papers on the same in which they have also conducted CFD on one convolution. I could add tubes to the two sides as shown in the picture but that would probably just increase the pressure drop instead of decreasing it.


For modeling the external air flow in CAD, I'll have to develop a negative model, such as that which is used in the car aerdodynamics model?

[ankit.khurana]

Which advection model should i run along with SSTK-epsilon ?

a particular research used periodic boundary conditions but did the analysis in a different software(Pic attached)
I couldnt understand as to how this will help

Neither could i figure out how to implement the same

[apolo_vanderberg]

If this is a small section of a larger radiator then yes:

We would want the air domain to be generated appropriately such that it would split the gap/cut through in a periodic/patterned fashion

The lateral/sides upstream of the radiator would have Slip/Symm conditions as to not introduce extra pressure drop and represent a large segment of air coming in.

The sides at and downstream of the radiator should be set up with Periodic conditions (we discuss how this is done in the Help)

This will allow for flow that leave the "right" side to enter the "left" side as though there was a patterned array of them. By not having this in your current model we are assuming its just the 1 fold in a wind tunnel

[ankit.khurana]

Thanks for the reply 
I am unable to understand which sides should i put up as slip and which as periodic. YOu are refering to the side with more width or less width. Could you clear that a bit please.
Also, should i apply the periodic , slip boundarary condition throughtout the mentioned side of the external volume, (from inlet to outlet) or to only a portion of the side

[ankit.khurana]

I have changed my approach a bit

i have constructed 3 rechangular channels  in CAD (having a wall thickness of 1mm) and have placed them as shown in the pic "Channel"

The left one is the inlet channel

the right one the outlet channel

the middle one is the channel surrounding the fin (lets call it fin channel)

the channels are open on the sides

in using using the void fill tab i have build a surface at the left opening of the inlet channel and at the right opening of the outlet channel

then i have filled the void

now i have assigned Aluminium to the 3 channels, supressed the 3 channels

assigned air (fixed, 45Degrees) to the 'cfdCreated internal volume'

assigned aluminum to the fin, supressed it 

I am only dealing with flow, no heat transfer

reffering to the pic 'FIN flow', i am trying to simulate the pressure drop while air passes over one verticle row of fins

Now I am confused as to apply slip symmetry on which face and periodic condition on which face

i feel i should apply the periodic boundary condition on the flow volume in the fin region, only on  the 2 wider sides (the sides which are almost parallel to the plane of the paper)(the side along the faint green axis seen in the top picture)

should i apply the slip symmetry condition on the inlet aur volume or the outlet air volume also

and on which sides should i apply it?

Thanks in advance