Discussion Groups

Simulation CFD

Reply
Active Member
CFDNewbie1
Posts: 7
Registered: ‎11-27-2012

Accurate Airflow model

359 Views, 10 Replies
11-27-2012 01:33 PM

I have set up a model to simulate airflow through a canopied generator set.

 

The model is very simple with a fan pulling airflow through inlet ducts, over an engine, through a cooling core and out a 90 Degrees vertical outlet duct at the top of the canopy.

 

The geometry has been set up with 0 gage pressure only as a boundary condition, the fan has a fan curve from the supplier and the cooling core has an air restriction curve from the supplier.

 

I am looking to run an accurate model as possible but due to computational restraints, cubes represent engines etc.

 

The outcome I am looking for is a pressure restriction of the canopy and a volumetric flow at the outlet.

 

I know there is a summary report, but is there a way to set up a plane to show volumetric flow at the outlet? Or the pressure drop through the system?

 

Also, I know increasing meshing size will help accuracy of the model, but is there any other tips/help more experienced users can offer to better setup this model. For example, does setting a free air ratio as a resistance instead of a restriction curve better represent reality within Autodesk Simulation?

 

Thanks in advance

Please use plain text.
Product Support
wildej
Posts: 971
Registered: ‎08-25-2011

Re: Accurate Airflow model

11-28-2012 12:46 AM in reply to: CFDNewbie1

Hi,

 

Sounds like you have the right approach, there are a few things to mention that might help:

 

  1. Suppress all solid parts from the mesh if you are not interested in heat transfer though them, this will save on mesh count
  2. A resistive region should be accurate with either approach, so long as whatever you assign matches reality
  3. You need a good uniform mesh on resistance regions and fans, aim for at least 4 elements through their thickness
  4. You can measure flow or pressure on planes by addingn a cut-plane and using the bulk calculator - search the help and use the Wiki if you need more detail, it explains it all well.


Jon Wilde
Please use plain text.
Active Member
CFDNewbie1
Posts: 7
Registered: ‎11-27-2012

Re: Accurate Airflow model

11-29-2012 12:20 AM in reply to: wildej

Thanks Mr. Wilde,

 

Does suppressing solid parts just stop heat transfer through them? Do they not have to be meshed for the CFD program to ascertain aiflow patterns around/ past/over solid objects?

 

Would this mean the only meshing I would be applying would be to the fan and the cooling core?

 

If I am modelling a fan, is ther any rules of thumb for the modelling? Currently I am using a cylinder, with no inner fixed hub modelled. It is set to the thickness of the suppliers drawing from one side of a blade tip to the other.

 

I feel I will have to play about with the resistive regions,  at the moment I have a grill outlet setup as a pattern from the model which is creating alot of nodes. I think it might be better to set this as a resistive region with a free air ratio.

 

Thanks.

Please use plain text.
Product Support
wildej
Posts: 971
Registered: ‎08-25-2011

Re: Accurate Airflow model

11-29-2012 12:53 AM in reply to: CFDNewbie1

Not a problem :smileyhappy:

 

Does suppressing solid parts just stop heat transfer through them? Do they not have to be meshed for the CFD program to ascertain aiflow patterns around/ past/over solid objects? You are correct, it will just stop the heat transfer, the flow patterns around them would not be affected.

 

Would this mean the only meshing I would be applying would be to the fan and the cooling core? And the air, yes.

 

If I am modelling a fan, is ther any rules of thumb for the modelling? Currently I am using a cylinder, with no inner fixed hub modelled. It is set to the thickness of the suppliers drawing from one side of a blade tip to the other. What you have souds sensible, although it is worth including a solid part around the outer diameter to ensure that no flow can leak. also ensure it has a good uniform mesh.

 

I feel I will have to play about with the resistive regions,  at the moment I have a grill outlet setup as a pattern from the model which is creating alot of nodes. I think it might be better to set this as a resistive region with a free air ratio Yes, this might be worthwhile. You can set the resistance to be different in each of the x.y,z directions to try to mimic the grill pattern.



Jon Wilde
Please use plain text.
Active Member
CFDNewbie1
Posts: 7
Registered: ‎11-27-2012

Re: Accurate Airflow model

12-12-2012 04:41 AM in reply to: wildej

Hi,

 

Many thanks for the reply.

 

I just have a couple more questions.

 

1. When I am modelling the fan, is it better to have a solid cylinder in the center to represent the hub? I have set a solid exterior to stop flow leak.

 

2. I have set up  the geometry as a 0 Pa gage pressure. Is there any need to specify inlets as 0 Pa gage pressure as well?

 

Thanks in advance.

Please use plain text.
Product Support
wildej
Posts: 971
Registered: ‎08-25-2011

Re: Accurate Airflow model

12-12-2012 07:08 AM in reply to: CFDNewbie1

 

1. When I am modelling the fan, is it better to have a solid cylinder in the center to represent the hub? I have set a solid exterior to stop flow leak - It does not really matter althuogh you can do - suppress it from the mesh if you do.

 

2. I have set up  the geometry as a 0 Pa gage pressure. Is there any need to specify inlets as 0 Pa gage pressure as well - I am unsure what this means. You only want to assign a p=0 to the fluid where there is an opening and only on the boundary of the model - nothing internally 

 

Does that make sense?

 

Thanks,

Jon



Jon Wilde
Please use plain text.
Active Member
CFDNewbie1
Posts: 7
Registered: ‎11-27-2012

Re: Accurate Airflow model

06-11-2013 12:54 PM in reply to: wildej
I have been working on/off with modelling on this simulation and had been getting good ball park data with good convergence until I realised the fan had been set to zero slip factor. When I start to increase this the convergence plots look like a sinusoidal wave plot with sharp drops and peaks creating nonsensical summary data.

I have checked the model, materials, meshing and input data and all seem to be accurate for a steady state airflow simulation.

Am I missing a further check? Is it reasonable to assume a slip factor of a pusher fan to be closer to 1 when using supplier curve data?

I have also noticed this happening when I change the advection from 1 to 2.
Please use plain text.
Product Support
wildej
Posts: 971
Registered: ‎08-25-2011

Re: Accurate Airflow model

06-12-2013 01:42 AM in reply to: CFDNewbie1

Hi,

 

We usually have the slip at about 0.7.

ADV5 is normally the best scheme for this type of model too.

 

Do you find that the model eventually converges? Perhaps you need more mesh or difference BC's?



Jon Wilde
Please use plain text.
Active Member
CFDNewbie1
Posts: 7
Registered: ‎11-27-2012

Re: Accurate Airflow model

06-12-2013 02:51 AM in reply to: wildej

Hi John,

 

Thanks for replying.

 

I am using CFDesign 2011 which doesn't have ADV5. The meshing is as fine as can be for the fan.

 

The model eventually converges but the summary data does not read correctly - Please see attached screenshot. This is with the ADV set to 1 and the slip set to 1.0 (I stopped this into the run due to the convergence plot display). I have tried this with alip at 0.25, but the outcome is the same (Iterations converges around 1100).

 

The only boundary condition I have set is 0 Pa for the four walls and roof of the surrounding space. No other BC has been set.

Please use plain text.
Product Support
wildej
Posts: 971
Registered: ‎08-25-2011

Re: Accurate Airflow model

06-12-2013 02:56 AM in reply to: CFDNewbie1

Hi,

 

I would certainly say that ADV2 would be best then.

 

This convergence plot does not suggest convergence, if you ever see anything like this, just stop the model as it is not right.

Do you have some thin parts in there too (looks like you may do), resitances maybe? If so, are you using surface or volume resistances? Is the mesh tight on these also? 3-4 elements inlet to outlet (same as the fan)?

 

How large is the overall domain?



Jon Wilde
Please use plain text.