Hi everyone,

Here's something I have noticed recently when looking at the pressure distribution around a hydrofoil I'm investigating. I have created a high quality hex mesh around a NACA profile using ICEM 5.1. The points which describe the NACA section have be generated with an accuracy of 6 decimal places. The curves and hence surfaces created within ICEM 5.1 have been produced using these points. A total of 50 points have been used to describe the section.

The mesh created around the section has been refined so that the first node near wall normalised wall distance (Y+) is < 1.0. The section has a chord of 1m. The near wall first node distance is 0.00000146m.

I pass this mesh to CFX-5.7.1 and use the k-e SST turbulence model to solve the flow over the section. I manage to obtain a well converged solution in 500 iterations down to a MAX residual of 1.0e-05.

The computed CL, CD and CM values compare favourably with experimental data and potential flow solutions obtained using a panel code.

Now, when I produce a Cp plot for the section, I notice that although the Cp distribution is close to those found by experiment and using a panel methods, there are small wiggles in the Cp at various locations around the section. Although these are not significant, just slightly annoying!, I'm trying to ascertain their origin. Has anyone else come across the phenomena when solving aero/hydrofoil flows using CFX-5.7.1.

I have a few ideas what might be causing these wiggle's, but as yet haven't had a chance to investigate them fully. Is it because the points describing the section have not been specified with enough accuracy, since the near wall spacing is of a similar order?

Would specifying points with an accuracy of say 10 decimal places over come this problem? Or possibly using section defined using fewer points with 6 decimal place accuracy?

Any pointers would be gratefully received.

James

Hi,

I assume Cp is the surface pressure coefficient. How have you extracted the Cp data? It might just be a function of post-processing.

Glenn Horrocks

Glenn

I created a plane positioned at 50% span and created a polyline which intersected the section. I then used the export facility to export the x and cp data for the polyline to a file.

James

This can be little bugs in post... Like sometimes problems with streamlines and values on streamlines - I enccountered many times values outside of range of solution variable. Areas for improvements still exists...

It's a little bit annoying when you go to extremes to make your mesh and boundary conditions as accurate as possible, to find that the data output in post has errors.

So has any one got any good solutions for getting around these possible errors CFX-Post.

James

In Icem, did you se the "Project to B-Splines" option?

Charles

I've seen the project to Bspline option under Hexa/Mixed meshing option but was unaware of what it actually did?. Out of interest what effect does altering the transfinite degree to quadratic also have?

James

Hi James,

Maybe try using some monitor points to extract the values direct from the solver.

Another way of looking at it in Post - If you draw contour lines on the wing surface does it also show the wiggles or other weird stuff, or is it smooth? That might help identify whether the wiggles come from Post or the solver.

Regards, Glenn

I've just tried projecting to Bsplines in ICEM and I received a negative volume error when I tried solving the mesh in CFX!. I would still like to know the advantage of doing this all the same.

I have looked at the contour plot on the surface of the section; there seem to be slight changes in the pressure in the regions already identified although it is very hard to tell. Placing monitor points along the surface of the section might be a bit tedious!

Perhaps, my problem is still with the accuracy of the initial points which have been used to describe the section!

Any more tips guys?

James

Try changing the geometry tolerance in ICEM. You can find this under Mesh > Global Mesh Size > Options: Triangle Tolerance. The default is usually 0.001 and I think it controls the accuracy to which the geometry is approximated. I have seen the wiggles you have mentioned before and reducing the geometry tolerance made them go away.

p.s. you have to change the value, save your .tin file, close it and then reload it into ICEM for the change to have an effect.

Robin

Robin

You were spot on. I changed the "Triangle Tolerance", trying both 0.0001 & 0.00001 and the wiggles disappeared pretty much all together!

So is there a rule of thumb for setting this value. Does the value have units of metres or is it an arbitrary number?

Thanks ever so much for the tip.

James

P.S. When should you use the project to Bspline option suggested by Charles, what advantages does it give?

James,

I think it is unitless like all things in ICEM. So if you are making your geometry in meters with a tolerance of 0.001 then your tolerance is actually 1 mm which clearly could cause problems on a yplus 1 grid where the first grid point is at 0.01 mm from the surface. As for a rule of thumb, I'm not sure, I guess at least an order of magnitude below your first grid point size might be a good start. So if your geometry is in metres and you want a yplus one grid (i.e. first grid point at 0.000001) then 0.0000001 would probably be a safe value.

Robin

Robin

Cheers for the advice. I'm sure others will find this very useful.

James