CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   CFX (http://www.cfd-online.com/Forums/cfx/)
-   -   wall roughness effect on pressure drop (http://www.cfd-online.com/Forums/cfx/76600-wall-roughness-effect-pressure-drop.html)

 mactech001 May 30, 2010 20:51

wall roughness effect on pressure drop

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

 ghorrocks May 30, 2010 21:00

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.

 mactech001 May 30, 2010 21:34

form effects in CFX

Quote:
 Originally Posted by ghorrocks (Post 260927) 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.

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

 ghorrocks May 30, 2010 22:15

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.

 mactech001 May 30, 2010 23:00

Quote:
 Originally Posted by ghorrocks (Post 260932) 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.

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

 ghorrocks May 30, 2010 23:09

No, you won't see chunks of low pressure. You will see the pressure drop in chunks, as it progresses from high to low.

 mactech001 May 31, 2010 00:34

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?

 ghorrocks May 31, 2010 00:50

1 Attachment(s)
Try this, pretty rough but hopefully you get the idea.
Attachment 3585

 mactech001 May 31, 2010 20:56

Quote:
 Originally Posted by ghorrocks (Post 260932) 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.

 ghorrocks May 31, 2010 20:58

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.

 mactech001 November 8, 2010 00:30

separations/wall friction loss

Quote:
 Originally Posted by ghorrocks (Post 260932) 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,

 ghorrocks November 8, 2010 00:36

If your simulation is accurate then CFX will predict the prescence or absence of separations.

 mactech001 November 8, 2010 00:46

Quote:
 Originally Posted by ghorrocks (Post 282571) 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

 ghorrocks November 8, 2010 17:35

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

 Dr. Flow Squad February 22, 2013 03:38

Hi Glenn.
How to get the variable distance on the streamline?

 ghorrocks February 22, 2013 05:58

In CFD-Post it is one of the variables available on stream line objects.

 Dr. Flow Squad February 22, 2013 06:55

Im sorry but it is not there

 All times are GMT -4. The time now is 16:34.