[Eli]

URGENT PLEASE

Hi there,

I want to simulate a very LONG air channel, about 40Km with complex and twisted path, while the channel's width is just about 2m.
How is it possible to model and analyze Huge geometries like this?
I could not even model it in DesignModeler or Solidworks... because of dimension!!!!

waiting for your kind hints
many thanks,
Eli

[cfd_newbie]

Originally Posted by Eli

URGENT PLEASE

Hi there,

I want to simulate a very LONG air channel, about 40Km with complex and twisted path, while the channel's width is just about 2m.
How is it possible to model and analyze Huge geometries like this?
I could not even model it in DesignModeler or Solidworks... because of dimension!!!!

waiting for your kind hints
many thanks,
Eli

Can't you split the geometry, for geometry modification, meshing and simulation ?

[Eli]

Originally Posted by cfd_newbie

Can't you split the geometry, for geometry modification, meshing and simulation ?

Thank you so much for your reply,
I guess I should do something like that, but would you please explain it more? how can I connect the split parts while I am meshing or simulating in CFX?
I have no idea of Splitting a huge problem to some smaller ones.

Thank again cfd-newbie

[cfd_newbie]

Originally Posted by Eli

Thank you so much for your reply,
I guess I should do something like that, but would you please explain it more? how can I connect the split parts while I am meshing or simulating in CFX?
I have no idea of Splitting a huge problem to some smaller ones.

Thank again cfd-newbie

1. Split the geometry in Designmodeller.
2. Mesh the parts individually.
3. Set up interfaces between the adjoining faces of different parts in CFX.
4. Setup boundary conditions for each part individually.
5. Simulate

[ghorrocks]

You are more likely to have a successful simulation using a 1D CFD simulation for this, so I would forget about CFX. 1D simulation models are pretty easy to write yourself, or many commercial ones are available.

What are you modelling anyway?

If you insist in doing this in CFX anyway I strongly recommend you mesh the long straight bits with a high aspect ratio swept mesh. In fact the more you can sweep the better. Any tets will be a disaster. And you will need double precision. But even the best mesh in the world will have problems with a geometry with an aspect ratio of 20000:1.

[Eli]

Originally Posted by cfd_newbie

1. Split the geometry in Designmodeller.
2. Mesh the parts individually.
3. Set up interfaces between the adjoining faces of different parts in CFX.
4. Setup boundary conditions for each part individually.
5. Simulate

Well! Great! It seems quite easy to work
But after step 2: importing all of the parts in CFX-Pre, setting up interfaces and boundary conditions for each one and simulating whole the huge geometry together.... Isn't it toooo much for CFX to do?

I think I will have a massive computational cost and lots of errors in front!

[ghorrocks]

If you do the meshing tutorials you will see you do not need to connect the sections with interfaces but can make the mesh contiguous. This is much better if it is possible.

No, you will need to find a very big simulation before it is too complex for CFX. CFX has been run on multiprocessor runs up to many thousands of CPUs. That allows you to run a pretty big simulation. The limitation is your available hardware and licenses, not CFX.

[Eli]

Originally Posted by ghorrocks

You are more likely to have a successful simulation using a 1D CFD simulation for this, so I would forget about CFX. 1D simulation models are pretty easy to write yourself, or many commercial ones are available.

What are you modelling anyway?

If you insist in doing this in CFX anyway I strongly recommend you mesh the long straight bits with a high aspect ratio swept mesh. In fact the more you can sweep the better. Any tets will be a disaster. And you will need double precision. But even the best mesh in the world will have problems with a geometry with an aspect ratio of 20000:1.

Dear Glenn

Thank you so much for your attention.
I attached a picture of cross section of channel and a rough sketch of the path.
Would you please take a look at them and tell me what you think?
It is much more complex than I explained.
Is it really possible to use a 1D cfd simulation for this problem or I should still use CFX? What is the best way to simulate it?

Thanks again Glenn, you are the best!

Cross section: Cross section.jpg

Path of the channel: Path.JPG

[ghorrocks]

What type of fluid - incompressible or compressible? Heat transfer? What Reynolds number and or Mach number?

You may be able to model a short section of the cross section with a periodic boundary so you get fully developed flow. Then you will get the pressure drop versus flow for a given length of duct. Model a few flow rates and you will get a pressure drop versus flow rate curve. Then you can do some pretty simple calculations to work out the flow in the ducts using the pressure drops you just calculated on the network you drew. And no need for geometries with aspect ratio 20000:1.

[Eli]

Originally Posted by ghorrocks

What type of fluid - incompressible or compressible? Heat transfer? What Reynolds number and or Mach number?

You may be able to model a short section of the cross section with a periodic boundary so you get fully developed flow. Then you will get the pressure drop versus flow for a given length of duct. Model a few flow rates and you will get a pressure drop versus flow rate curve. Then you can do some pretty simple calculations to work out the flow in the ducts using the pressure drops you just calculated on the network you drew. And no need for geometries with aspect ratio 20000:1.

Certainly it is the best solution, but it is my fault that I didn't explain enough about the problem.
I should have mentioned that there are 2 blowers and 2 other suction fans in different points of this duct which control the air (as incompressible fluid) through the channel.
The main purpose of this ventilation project is to find out the best flow rate for each fan and the pressure profile anywhere in the duct !!!

I truly appreciate if you let me know your opinion now.

[singer1812]

CFD is overkill for this problem. If you insist using CFD, only model a 2D cross section of the channel, get the Pdrop vs flow rate for the cross section. Use that in a pipe flow calc (you can set this up in a spread sheet even).

If you need (want) more fidelity, you could also model short portions of the T intersections and the angles, and get a Pdrop vs flow rate and use that in the pipe flow calc.

CFD of the entire problem would be a waste.

[Eli]

Originally Posted by singer1812

CFD is overkill for this problem. If you insist using CFD, only model a 2D cross section of the channel, get the Pdrop vs flow rate for the cross section. Use that in a pipe flow calc (you can set this up in a spread sheet even).

If you need (want) more fidelity, you could also model short portions of the T intersections and the angles, and get a Pdrop vs flow rate and use that in the pipe flow calc.

CFD of the entire problem would be a waste.

Thank you for your reply,
I think you are right, CFD does not work for the entire problem.

[ghorrocks]

I should have mentioned that there are 2 blowers and 2 other suction fans in different points of this duct which control the air (as incompressible fluid) through the channel.

That is fine, you include them as fan curves in the network model. As Edmund and I have both said the way forward is to get the pressure drop and use a 1D approach to solve this on your network. Easy, I have done this sort of thing many times before and it can be done in simple packages like excel.

[juliom]

I think it would be better to do a non-dimensional analysis, and make a scale prototype.
Before doing the scale prototype, you have to make a dynamic similarity analysis.
I´m quite sure that through this approach you will get faster results!!
Kind regards
Julio M