CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > CFX

wall roughness effect on pressure drop

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

Reply
 
LinkBack Thread Tools Display Modes
Old   May 30, 2010, 20:51
Default wall roughness effect on pressure drop
  #1
Senior Member
 
Join Date: Nov 2009
Posts: 125
Rep Power: 7
mactech001 is on a distinguished road
Dear all,

i'm trying to figure out how much wall roughness on my design could effect my pressure drop in my water cooling jacket for electrical machine.

so far, i've tried 50um and 1mm, but there doesn't seem to be ANY significant increase in pressure drop between the inlet and outlet of the cooling jacket.

in fact, in CFX-Post, under the 'Physics Report' -> 'Boundary Physics' part, the Interface on the solid that defines the interface between fluid and solid doesn't show that the wall roughness is applied, even though in the *.def file, the Wall roughness on the interface on the solid is applied as 1mm.

is there something i missed during the setup please?

Look forward to hear of any comments/suggestions.

Thanks!

Regards,
mactech001
__________________
Thank you for your kind attention.

Kind regards,
mactech001
Currently using: ANSYS v13
mactech001 is offline   Reply With Quote

Old   May 30, 2010, 21:00
Default
  #2
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,665
Rep Power: 84
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
That suggests form effects (ie separations and the like) are the significant contributor to flow resistance, not wall friction affects. This is not really surprising in a geometry like a cooling jacket.
ghorrocks is offline   Reply With Quote

Old   May 30, 2010, 21:34
Default form effects in CFX
  #3
Senior Member
 
Join Date: Nov 2009
Posts: 125
Rep Power: 7
mactech001 is on a distinguished road
Quote:
Originally Posted by ghorrocks View Post
That suggests form effects (ie separations and the like) are the significant contributor to flow resistance, not wall friction affects. This is not really surprising in a geometry like a cooling jacket.
Hi Glenn, thank you so much for your prompt reply.

will i be able to consider these form effects into my simulation model please? how can i do that please?

in addition, i've considered using SST turbulence model in my simulations.

regards,
mactech001
__________________
Thank you for your kind attention.

Kind regards,
mactech001
Currently using: ANSYS v13
mactech001 is offline   Reply With Quote

Old   May 30, 2010, 22:15
Default
  #4
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,665
Rep Power: 84
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
Plot total pressure on the jacket walls. The pressure should start high and get lower. If the main pressure drop is caused by separations the total pressure will decrease in chunks where each chunk is a separation. If the total pressure decreases gradually it suggests wall friction effects - but we already suspect this is small so you might not see this.

An alternate approach is to draw a single streamline from the inlet to the outlet and colour it by total pressure. If you export the data on the streamline (include total pressure and distance along the streamline) you should see the high pressure decay to the low pressure exit. You should be able to identify from there where the big pressure drops are, and that is where the bad separations/nozzles/jetting/whatever will be.
ghorrocks is offline   Reply With Quote

Old   May 30, 2010, 23:00
Default
  #5
Senior Member
 
Join Date: Nov 2009
Posts: 125
Rep Power: 7
mactech001 is on a distinguished road
Quote:
Originally Posted by ghorrocks View Post
Plot total pressure on the jacket walls. The pressure should start high and get lower. If the main pressure drop is caused by separations the total pressure will decrease in chunks where each chunk is a separation. If the total pressure decreases gradually it suggests wall friction effects - but we already suspect this is small so you might not see this.
Hi Glenn, thanks again for your prompt reply.

At the moment, i'm plotting 'total pressure' on the fluid domain's fluid-solid interface (when i plot 'total pressure' on the solid domain's fluid-solid interface, no contour displayed), and i do see pressure high at inlet and getting lower towards the outlet. i don't see chunks of low pressure.

would this suggest the wall friction effect dominates over separation effects?

Furthermore, i'm sorry i've not been clear with my problem description. current test suggests that the pressure drop is higher than what i calculated previously, and i'm trying to improve my model setup to consider any other effects to make my calculation more real.

regards,
mactech001
__________________
Thank you for your kind attention.

Kind regards,
mactech001
Currently using: ANSYS v13
mactech001 is offline   Reply With Quote

Old   May 30, 2010, 23:09
Default
  #6
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,665
Rep Power: 84
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
No, you won't see chunks of low pressure. You will see the pressure drop in chunks, as it progresses from high to low.
ghorrocks is offline   Reply With Quote

Old   May 31, 2010, 00:34
Default
  #7
Senior Member
 
Join Date: Nov 2009
Posts: 125
Rep Power: 7
mactech001 is on a distinguished road
Hi Glenn, thanks again.

i'm sorry, but i can't entirely visualize what you described. do you have pictures to show gradual decrease of 'total pressure' and another to show pressure drop in chunks please?
__________________
Thank you for your kind attention.

Kind regards,
mactech001
Currently using: ANSYS v13
mactech001 is offline   Reply With Quote

Old   May 31, 2010, 00:50
Default
  #8
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,665
Rep Power: 84
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
Try this, pretty rough but hopefully you get the idea.
Chunks.jpg
ghorrocks is offline   Reply With Quote

Old   May 31, 2010, 20:56
Default
  #9
Senior Member
 
Join Date: Nov 2009
Posts: 125
Rep Power: 7
mactech001 is on a distinguished road
Quote:
Originally Posted by ghorrocks View Post
An alternate approach is to draw a single streamline from the inlet to the outlet and colour it by total pressure. If you export the data on the streamline (include total pressure and distance along the streamline) you should see the high pressure decay to the low pressure exit. You should be able to identify from there where the big pressure drops are, and that is where the bad separations/nozzles/jetting/whatever will be.
Hi Glenn,

this alternate approach you described, is it part of the 3D streamline command? or should i define my own poly-line please in CFX-Post?

my main difficulty in doing this is that, my cooling jacket has helical channels from inlet to outlet.... drawing a helical line will be easy in 3D CAD softwares but difficult in CFX-post.
__________________
Thank you for your kind attention.

Kind regards,
mactech001
Currently using: ANSYS v13
mactech001 is offline   Reply With Quote

Old   May 31, 2010, 20:58
Default
  #10
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,665
Rep Power: 84
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
Quote:
streamline command? or should i define my own poly-line
Either approach is fine. Streamlines can be easier but they don't always go where you want them to.
ghorrocks is offline   Reply With Quote

Old   November 8, 2010, 00:30
Default separations/wall friction loss
  #11
Senior Member
 
Join Date: Nov 2009
Posts: 125
Rep Power: 7
mactech001 is on a distinguished road
Quote:
Originally Posted by ghorrocks View Post
Plot total pressure on the jacket walls. The pressure should start high and get lower. If the main pressure drop is caused by separations the total pressure will decrease in chunks where each chunk is a separation. If the total pressure decreases gradually it suggests wall friction effects - but we already suspect this is small so you might not see this.

An alternate approach is to draw a single streamline from the inlet to the outlet and colour it by total pressure. If you export the data on the streamline (include total pressure and distance along the streamline) you should see the high pressure decay to the low pressure exit. You should be able to identify from there where the big pressure drops are, and that is where the bad separations/nozzles/jetting/whatever will be.
Hi again Glenn,

rebounding back to the enquiry here, can i consider these effects in order to obtain a more realistic pressure drop result please?

or has CFX already considered separation effects?

regards,
__________________
Thank you for your kind attention.

Kind regards,
mactech001
Currently using: ANSYS v13
mactech001 is offline   Reply With Quote

Old   November 8, 2010, 00:36
Default
  #12
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,665
Rep Power: 84
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
If your simulation is accurate then CFX will predict the prescence or absence of separations.
ghorrocks is offline   Reply With Quote

Old   November 8, 2010, 00:46
Default
  #13
Senior Member
 
Join Date: Nov 2009
Posts: 125
Rep Power: 7
mactech001 is on a distinguished road
Quote:
Originally Posted by ghorrocks View Post
If your simulation is accurate then CFX will predict the prescence or absence of separations.

'...simulation is accurate...' points to domain imbalance is <0.01, all RMS errors converges to <1e-4?

regards,
mactech001
__________________
Thank you for your kind attention.

Kind regards,
mactech001
Currently using: ANSYS v13
mactech001 is offline   Reply With Quote

Old   November 8, 2010, 17:35
Default
  #14
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,665
Rep Power: 84
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
Convergence is only one of many things to consider when you assess whether your simulation is accurate. Have a look here: http://www.cfd-online.com/Wiki/Ansys..._inaccurate.3F
ghorrocks is offline   Reply With Quote

Old   February 22, 2013, 03:38
Default
  #15
New Member
 
Dr. Flow Squad
Join Date: Mar 2009
Posts: 14
Rep Power: 8
Dr. Flow Squad is on a distinguished road
Hi Glenn.
How to get the variable distance on the streamline?
Dr. Flow Squad is offline   Reply With Quote

Old   February 22, 2013, 05:58
Default
  #16
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,665
Rep Power: 84
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
In CFD-Post it is one of the variables available on stream line objects.
ghorrocks is offline   Reply With Quote

Old   February 22, 2013, 06:55
Default
  #17
New Member
 
Dr. Flow Squad
Join Date: Mar 2009
Posts: 14
Rep Power: 8
Dr. Flow Squad is on a distinguished road
Im sorry but it is not there
Dr. Flow Squad is offline   Reply With Quote

Reply

Thread Tools
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 On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Fluent3DMeshToFoam simvun OpenFOAM Other Meshers: ICEM, Star, Ansys, Pointwise, GridPro, Ansa, ... 48 May 14, 2012 05:20
Errors running allwmake in OpenFOAM141dev with WM_COMPILE_OPTION%3ddebug unoder OpenFOAM Installation 11 January 30, 2008 21:30
Neumann pressure BC and velocity field Antech Main CFD Forum 0 April 25, 2006 02:15
Gas pressure question Dan Moskal Main CFD Forum 0 October 24, 2002 22:02
what the result is negatif pressure at inlet chong chee nan FLUENT 0 December 29, 2001 06:13


All times are GMT -4. The time now is 20:57.