
[Sponsors] 
August 11, 2011, 19:56 
[Pointwise] wing mesh, project connectors

#1 
Member
Join Date: May 2010
Posts: 44
Rep Power: 7 
Dear All,
I am modelling flow around a wing. I generated the hybrid mesh in Pointwise. When I plot the chordwise distribution of pressure coefficient (Cp), I get wiggles in it at the leading edge. I believe its because the mesh is not precisely projected to the underlying geometry database (though the domains are purple in Pointwise). I know there is a project tool in Pointwise but whichever projection method I use it does not change anything. Does anyone know how to use it properly? Also, how can I decrease the tolerance of the underlying geometry databases? They are just approximated too coarsely. Thanks for any help in advance! P.S. see attached picture of the mesh and the resulting Cp plot. 

August 12, 2011, 17:54 

#2 
New Member
Nick
Join Date: Mar 2009
Location: England (South West)
Posts: 25
Rep Power: 8 
I would suggest that your connector is properly projected onto the database, its just the edge resolution is a bit coarse. Try upping the number spacing on the connecter and it should follow the database more closely.


August 13, 2011, 18:53 

#3  
Member
Join Date: May 2010
Posts: 44
Rep Power: 7 
Quote:
Anyways the chord length of the wing is 735mm, the first cell at the leading edge of the wing is 1mm ! Should be fine. Thanks for the comment though... 

August 14, 2011, 14:29 

#4  
Senior Member
Vieri Abolaffio
Join Date: Jul 2010
Location: Always on the move.
Posts: 308
Rep Power: 8 
Quote:
every meshing sw uses straight lines to approximate curves. where have you seen a cell with a curved edge? if the number of points is high enough you will not notice the difference. if you don't want to increase the overall number of cell you might try to increase the refinement near the LE and coarsening it where the gradients will be less sharp, for example in the middle of the foil. 

August 14, 2011, 15:04 

#5 
Super Moderator
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,953
Blog Entries: 6
Rep Power: 39 
may be it is due to the transition from laminar to turbulent flow with small separation bubble.
use klktw or sst gamma thetta model. 

August 14, 2011, 17:23 

#7 
Senior Member
John Chawner
Join Date: Mar 2009
Location: Fort Worth, Texas, USA
Posts: 224
Rep Power: 9 
Hello la7low:
Let's start with the wing geometry (aka the database). You mention that they are "approximated too coarsely." Pointwise does not approximate the geometry. It uses it in whatever form you provide it. If you provide a discrete surface, it will keep it discrete and faceted. If this is how you're using it, you can choose to fit a cubic curve or surface through a linear or bilinear, respectively, database surface. That will give you a cubic shape on which to generate your mesh. However, keep in mind that a cubic, while smooth, doesn't necessarily match the true geometry. If on the other hand your database was imported from a CAD system (for example, via an IGES file), Pointwise uses the surfaces as defined in that file. So if you give it a surface that's a 7th degree BSpline surface, the mesh will be generated on that shape. If I'm interpreting your picture correctly, your arrows point to regions where the grid lines (green) cut inside the geometry. In high curvature regions that will happen if the grid points are too widely spaced. In other words, the grid points are connected by straight lines and may cut through the geometry. You fix that by changing your mesh spacing to make it smaller in regions of high curvature. Regarding Pointwise's projection command and whether or not it's working, you can select your surface mesh and use the Examine command with function DB Associativity to see whether Pointwise thinks all the points are on the database or not. Of course, the projection command also gives you a tally of percent on and off. There is also another subtlety that you may be seeing. Depending on how small the grid is in the picture you attached and how far zoomed in you are, you may be seeing a graphical artifact due to how the database is discretized for display. I don't think that's the case, but sometimes if you zoom in far enough you can make the grid and database seem to diverge even though they're not. In summary, consider two things. If your database is discrete, Pointwise will put points on that discrete, faceted shape. The option here is to use the Fit command to make a new database shape that's a cubic. Second, if you put too few grid points on a highly curved surface, the mesh will be a poor approximation to the shape. Hope this helps.
__________________
John Chawner / jrc@pointwise.com / www.pointwise.com Blog: http://blog.pointwise.com/ on Twitter: @jchawner 

August 16, 2011, 14:14 
fit?, curved cells?

#8  
Member
Join Date: May 2010
Posts: 44
Rep Power: 7 
Quote:
Would be great if I could put a smooth cubic surface on the discrete surface. How can I do that? You mentioned Fit command. When I select the Solid database or the quilts the EditFit command is still inactive... Quote:
Quote:
Quote:
To sum up, the problem is then twofold: firstly, my geometry is a bad representation of the original, smooth wing (this was spoiled in Solidworks). Secondly, the cells at the walls can be straight lines only (I suppose), which means that even a smooth wing geometry will be zigzaggy in the solver, but it is even worse for dsicrete geometries when the underlying geometry is zigzaggy at the first place. So the solution is to use at least smooth geometry with refined mesh at the curvatures. Thanks for the comments! 

August 16, 2011, 14:31 

#9 
Senior Member
John Chawner
Join Date: Mar 2009
Location: Fort Worth, Texas, USA
Posts: 224
Rep Power: 9 
If you have a model and quilts your geometry is a NURB, not discrete/faceted. We can't make solid models out of discrete geometry yet. This is why Fit is inactive with the quilt selected.
Pointwise generates linear elements meaning cells cannot be curved. Said another way, adjacent grid points are connected with a straight line. The only way to make your grid a better approximation of your geometry is to cluster the points closer together. If DB Associativity is 100% that means all your grid points are on the database. Given all these facts, my last conjecture about graphics precision is not a factor here. Without knowing how the geometry was created, I can't blame SolidWorks for anything you're seeing.
__________________
John Chawner / jrc@pointwise.com / www.pointwise.com Blog: http://blog.pointwise.com/ on Twitter: @jchawner 

August 16, 2011, 16:50 

#10  
Member
Join Date: May 2010
Posts: 44
Rep Power: 7 
Quote:
Quote:
Would be nice though if one could set the tolerance when exporting to iges. So that is not this curvy/wavy. 

August 16, 2011, 17:22 

#11 
Senior Member
John Chawner
Join Date: Mar 2009
Location: Fort Worth, Texas, USA
Posts: 224
Rep Power: 9 
Pointwise renders discrete surfaces exactly, point for point. For analytic surfaces, it uses an algorithm to sample and evaluate the surface at a sufficient number of points to ensure an accurate rendering.
Yes, there are meshes that use higherorder elements. This is typically the finite element method of which there are relatively few CFD solvers. Never having done it myself, I'll say it's equivalently (but not equally) difficult to write an FEA solver versus a finite volume solver. Why doesn't everyone use Cartesian? We are talking about two types of linear approximation. In a grid like the ones you've made, the grid lines are bodyfitted meaning they follow the contours of the body. So even though the grid lines are faceted, they can still provide a good approximation of high curvature. With a Cartesian grid you either end up with stairstepping on the boundary (which is awful from a CFD standpoint) or you create cut cells near the wall to retain boundary conformance. Cut cells make your solver more complicated (because you end up having to handle cells with an arbitrary number of faces) plus you don't have any alignment of grid lines with the flow near the body which is a good thing when it comes to accurately capturing the boundary layer. Tolerancing in IGES only comes into play with trimmed surfaces  how accurately do trimming curves match the surface they're on and how well to adjacent surfaces fit together. If you start with just BSpline surfaces (entity 128 in IGES) there's no tolerance issue at all.
__________________
John Chawner / jrc@pointwise.com / www.pointwise.com Blog: http://blog.pointwise.com/ on Twitter: @jchawner 

Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
Moving mesh  Niklas Wikstrom (Wikstrom)  OpenFOAM Running, Solving & CFD  122  June 15, 2014 06:20 
mesh missing after import in fluent  morteza08  FLUENT  0  July 23, 2010 02:22 
How to control Minximum mesh space?  hung  FLUENT  7  April 18, 2005 09:38 
how to mesh a 3d wing with Gambit?  Ben Vernieres  FLUENT  2  October 30, 2004 13:11 
How to mesh a delta wing in the middle of a sphere  David  FLUENT  0  September 2, 2004 13:19 