CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > FloEFD, FloWorks & FloTHERM

Define a Counterflow heat exchanger in FloEFD

Register Blogs Members List Search Today's Posts Mark Forums Read

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   July 18, 2016, 06:58
Question Define a Counterflow heat exchanger in FloEFD
  #1
New Member
 
Anders
Join Date: Jul 2016
Posts: 1
Rep Power: 0
Kylbalsam is on a distinguished road
Hi all,

My goal is to find the correct pressure drop through a counterflow heat exchanger.
It’s supposed to be 101 Pa in each direction of flow over the exchanger. (I’m only looking at one of the directions – see attached images below)
This is the setup in FloEFD with outlet airflow in red and inlet environment pressure as blue - https://i.imgsafe.org/ca62ac9145.png

The volume flow is 720 m³/h and the medium is air.

The way the heat exchanger is constructed, is that the flow can only travel in Z and Y-direction. This is because the “heat transfer plates” are stopping the flow to travel in the X-direction. (these are the coordinates in my model)

To simulate this in FloEFD, I have defined the entire heat exchanger as a “Porous Medium”.
In order to define the direction of travel for the air and not to make it to travel in X-direction, I’m using the “Orthotropic” option under Item Properties in the Engineering Database. See attached image https://i.imgsafe.org/ca40a192ec.png

The pressure drop is known through the heat exchanger from its datasheet, so I really know what it's suppose to be. But I'm doing this just to confirm I get the settings right before I'm going to build further on this, but that's another story. Anyway...

Pressure drop definition is made per axis – see attached images https://i.imgsafe.org/ca416043bb.png, https://i.imgsafe.org/ca416584e8.png and https://i.imgsafe.org/ca41572399.png

X-direction is defined with a very high pressure drop as air flow is not meant to travel that way.

Now to the core of the question:

Definition of length and area!

When defining the length and area according to the geometry of the heat exchanger, the resulting pressure drop and flow pattern are completely incorrect. The flow through the heat exchanger looks abnormal and actually travels in x-direction.
See attached images:

https://i.imgsafe.org/ca431071b9.png

https://i.imgsafe.org/ca4300c92d.png
https://i.imgsafe.org/ca43057a04.png
https://i.imgsafe.org/ca42f16d18.png
https://i.imgsafe.org/ca42f79cda.png


When changing the geometry, like length and area, the flow pattern changes. Sometimes only minor changes in result, sometimes very big ones in result. Both flow pattern and pressure drop.
The flow through the heat exchanger is expected to be more laminar/straight through and not changing direction like it does in the attached images. Inlet and Outlet should also have a more even flow pattern.
It seems like the length and area are both important. It’s not only the definition of pressure drop that is important.

Is there an example in how to use the length and area definitions? And what is it supposed to be really? This would help me defining this heat exchanger.

Hopefully someone can guide me in the right direction.
Thanks!

/Anders

Kylbalsam is offline   Reply With Quote

Old   August 16, 2016, 09:46
Default
  #2
Senior Member
 
Boris Marovic
Join Date: Jul 2009
Posts: 584
Rep Power: 18
Boris_M will become famous soon enough
Hi Anders,

there are several issues in the model definition.

For one I would increase the inlet and outlet length as you suck out the air, there will be some separation due to the corner of the heat exchanger (HX) because the outflow vector is prescribed onto the outlet surface and you can see in the streamline image that the flow paths bent towards a perpendicular outflow as it is forced onto them by the boundary condition.

I cannot tell why it has so odd flow in the xy-plane plot without a closer look onto the model and definitions.

In general the way you want to specify the porous media is correct, but I think one issue might source of the properties. I don't know what your source is and what it references to (the whole HX or the porous media). If it is the whole HX, then the geometry shape and the influence is included in the pressure loss but you model that shape and flow again which will - simply said - double the shape effect.
The correct model would only reference to a section out of the porous media structure you have inside the HX, not its total pressure loss. So cut out a 10x10x10cm cube and get the properties for that and use these dimensions as well as pressure loss data as reference data for the porous media and then build that into the HX.
If you don't have that and are only interested in the pressure loss then use a square block and use the dimensions of the square block as reference sizes and therefore make it a unit size for which exactly these pressure losses apply. Any change in size will then extrapolate the pressure loss.
This change is in some way the issue you have in your model, the geometry is not a square block, it has chamfers at the edges.
The data you try to use is more useful for a 1D system simulation in which a full component will be used rather than using a full component data on a 3D simplification of the details.

There is a new webinar on the Mentor Graphics website which explains how such a porous media in such a case is modeled.
https://www.mentor.com/products/mech...gn-performance

If you do it the way it is in the webinar then the results should match but as you can see, here the pressure loss is of the interior structure, not of the full component with its complex boxed shape.

To help you more I would need to know what you are trying to do at the end. At the moment you are analyzing something that is already given. This is like buying a pump and trying to model the housing and apply a pump curve between inlet and outlet. For what? Why do you model the housing and not simply inlet and outlet and apply the pump curve? In your case the housing seems to fixed, so why model what is inside if you cannot change it?
If it would be your design then you would have the interior structure that you could analyze just like in the webinar and then optimize the housing if that is what you are trying to do.

I hope this helps,
Boris
Boris_M is offline   Reply With Quote

Reply

Tags
floefd, heat exchanger, orthotropic, porous medium, pressure drop

Thread Tools Search this Thread
Search this Thread:

Advanced Search
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are Off
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Turbulent heat transfer in a plate heat exchanger P_P Main CFD Forum 0 July 16, 2015 10:46
Ansys Fluent analysis of heat exchanger MStudent FLUENT 2 April 20, 2015 09:40
UDF for Heat Exchanger model francois louw FLUENT 2 July 16, 2010 03:21
Heat Exchanger Simulation tightaznbreaka FLUENT 0 March 18, 2010 16:45
REAL GAS UDF brian FLUENT 6 September 11, 2006 09:23


All times are GMT -4. The time now is 17:16.