Hi,

I've been working with very small geometry (1/16" holes and smaller) and I've been running into trouble. Basically, my pressures are either way smaller (off my 48 psi) or way larger (50 psi) than experimental values. I've checked everything and I've finally concluded that perhaps my mesh resolution is the culprit. For a simple 1/16" tube (ID) here is my mesh: 5 inflation layers w/ max height of 0.002" Tetra mesh of max 0.01" Although it does sacrifice some resolution in the tetra nodes, I've found that below these values the mesh can get huge. Just to be safe, I have a 5 gpm (0.6942 lbs/sec) massflow in, an averaged 0 pressure out. I'm also using k-eps with a medium intensity. Any pointers would be most appreciated.

-W

Wooster, have you checked the values of Y+ for 0.002" ? also I think you may need to have more than 5 layers. I suggest using quad cells "Hexahedras" to overcome some of the problems with huge mesh. If you are using CFX mesh use the extruded option!

-O

I've give it a try, thanks Omar.

-W

Hi,

Just goes to show results without a mesh sensitivity study are worthless. Don't forget to also consider convergence sensitivity and timestep size (if transient).

What Reynolds does the device operate at?

Glenn Horrocks

Actually, this was a sensitivity study. The original model was very complex and I wanted to do a sensitivity study on smaller and smaller tubes with an L/D of 50. The large the tube, the better answers I get. I'm using "Handbook of Hydraulic Resistance" by Idelchik as well as a few other papers to give me some guidance. I'm afraid I mis-typed on my inlet conditions. I'm basically keeping all my inlet conditions for a Reynolds of 3.8*10^5. One thing that I've read over and over (and still am shaky on) is this y+ value. Now I can examine my model and see the y+'s but I'm not sure how to interpret them even after delving into the CFX manual. If I have a small (1-11) y+, I'm assuming I probably need more boundary layers. Anything larger than 11 and it seems I'd need fewer. Did I get that backwards or am I on the right track? On a different note, the original models mesh puts me right on top of the lab values. But I'm thinking I lucked out with a good mesh. -W

Hi,

For further reading on boundary layer modelling and y+ I recommend looking at Wilcox's book "Turbulence for CFD".

For y+<11 (approx) the first node will be in the viscous sub-layer. For y+>11 the first node will be in the log-layer region. Traditional wall functions use a logarithmic approach which is only valid in the log-layer region. This is why traditional wall functions need y+>11 for the first node. Turbulence models which fully resolve the boundary layer (that is can model the viscous sublayer, such as k-omega) need y+=1 about for the first node so the viscous sublayer is correctly resolved.

The automatic wall function approach in CFX automatically blends from the viscous sublayer approach is y+<11 to a log-layer approach if y+>11. To my knowledge this is the only turbulence model which can handle the full range of boundary layer resolutions.

Note the boundary layer extends well beyond the log-layer region and therefore other factors, such as having sufficient nodes in the full boundary layer (15 is the manual's recommendation) for accurate boundary layer modelling, regardless of what approach you use.

Regards, Glenn

Thanks Glen,

I had read in the manual about the CFX blends and had wondered if it was a feature for easy resolution of the y+.

Again, I've gotten my large models (diameter >1") to come out perfect but once you go below 1" your file size begins to go up as you struggle to maintain resolution and boundary layers. There are the hexa cores, etc, but I don't think our license covers us on that.

Wilcox was just returned to the library so I'll dig him out again and read a little further.

-W