[mactech001]

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]

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]

Originally Posted by ghorrocks

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

[ghorrocks]

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]

Originally Posted by ghorrocks

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

[ghorrocks]

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]

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]

Try this, pretty rough but hopefully you get the idea.
Chunks.jpg

[mactech001]

Originally Posted by ghorrocks

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]

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]

Originally Posted by ghorrocks

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]

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

[mactech001]

Originally Posted by ghorrocks

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]

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]

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

[ghorrocks]

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

[Dr. Flow Squad]

Im sorry but it is not there