Small wiggles in pressure distribution
 

Hi all,

using the search function revealed that a few others had similar problems (Wiggles in CP plots over Store Fins, Small Wiggles in Hydrofoil Pressure Distribution, ...) - but not exactly the same.

Problem:
When simulating the flow around a 2D airfoil (e.g. OAT15A), I get small wiggles in the cp distribution where the surface cell length is (considerably) smaller than the spacing of the underlying airfoil coordinates imported as a database!

I'm using the structured flow solver FLOWer at transonic flow condition. Before meshing with Pointwise (V17) I've used IGG and it worked absolutely fine! Therefore I'd exclude the flow solver or the setup as the source of error...
The mesh resolution should be fine: 300 points around the airfoil leading to a 2D mesh with approx. 100.000 cells. As stated in other posts, these wiggles hardly affect the overall aerodynamic coefficients (lift, drag, ...).

Since the wiggles only occur where Pointwise has to calculate several 'intermediate' points on the airfoil surface I assume that the interpolation of these points causes the wiggles. Where can I change the interpolation algorithm? The suction side and pressure side connectors are created by "Connectors on Database Entities" with a default setting of 100 points. I've also tried to create these connectors manually (Create --> Draw Curves --> Curve on Database) where I can select the interpolation method (Catmull-Rom, Akima, ...). But as soon as I select the first point on the database, pointwise automatically switches to "Line on Database"...

In addition, I've reduced the tolerances to 1e-9 and set the model size to 1 (airfoil coordinates from 0 (LE) to 1 (TE)) ...

Does anyone know how to get rid of this annoying probleme?
Just refining the provided airfoil coordinates with an external program might be possible but not really satisfying.

Some remarks to the pictures:

• black line: original airfoil coordinates imported in Pointwise via database
• red line: Surface grid after flow simulation
• blue line: Pressure distribution obtained from flow simulation

UPDATE: The surface curvature of the airfoil described by the grid (red line) shows exactly the same wiggles as the cp distribution...

http://www.directupload.net/file/d/4...w35hy5_png.htm

If you didn't fit a spline through the points when you imported the original airfoil coordinates, then you would be left when a simple linearly interpolated curve. Based on the results you're showing, this must what is going on. The CFD sees the airfoil as a faceted surface, hence the peaks/valleys in your Cp curve.

To smooth the airfoil geometry, after you import the coordinates create a spline (select curve(s) and use Edit>Spline).

To demonstrate, I imported NACA0012 with 63 points. The first image is after import - you can see the linear segments. The second image is after splining it - now smooth.

Hope that helps.

Dear cnsidero,

thank you very much for your reply! That's of course the solution of the problem!!! :)

As long as the grid density doesn't exceed the coordinate density of the imported airfoil geometry, a linear line is no problem!
As you can see from the attached file, as soon as more than 3 grid points are in between two adjacent 'supporting' airfoil coordinates, you get a constant surface curvature finally leading to the reported cp wiggles!

Changing the type of the imported database by selecting the database → edit → spline solved the problem and removed the cp wiggles!

Hi Rouven,

What type of database does it need in order to appear "spline" option in "edit"? Because I have tried it with my database but when I clicked on "edit", it does not appear "spline" option.

From the Pointwise User Manual, Ch 4.25: Spline

Hi giangcoikx,

I've used an ASCII-formatted file, containing the x-/y-coordinates of the airfoil split in two segments (suction side & pressure side).

So for example:

150 (<-- No. of points on 1st segment = pressure side)
x1 y1
x2 y2
...
150 (<-- suction side)
x151 y151
x152 y152
...