[Hamid.de]

Hi there.
I've been using pointwise for a while and I'd like to make a hybrid mesh for a HAWT blade and the whole stationary and rotary domain all together in pointwise. my main source for practicing this method was the very informative tutorial on YouTube which was done by Mr. Travis Carrigan. I was able to create a hybrid mesh for my own model and after setting up the volume and boundary condition, I export my model to fluent. fluent identifies my zones and boundary conditions just fine (or at least it seems so), but at the mesh checking process it reports some warning based on left-handed faces detection in the mesh, I've done full search through this problem both in pointwise and fluent forums and I found some helpful threads that addressed this issue pretty well, like using orient command in pointwise to correct the structured domains and blocks orientation. But when I select my structured blocks and click on the orient command the status of all the blocks are right handed. Also, I have some issues with mesh analysis parameters, when I analyze the mesh in pointwise the max aspect ratio is approximately 1.4 e+4 which is somehow expected due to the very small first cell height in the boundary layer (around 1e-4) but this parameter is too much bigger than it must be ( around e+14) in fluent. I've already gone through this issue too and know that it might be for units inconsistency between pointwise and fluent, But my domain scale looks fine in both.
so my questions are:
1.How can I overcome the left-handed faces issue at mesh level?
2. why is there such a big difference between pointwise and fluent aspect ratio report?
I have attached some images of the mesh, Bc's setting panel, and fluent TUI panel. I took images of what I thought that might be helpful, so if any other information is needed I'll be glad to provide that.
At last, I'd like to express my gratitude to whom will provide the proper response to my problem and the other who shares their thoughts.
please forgive me if I've expressed too much or maybe unnecessary information, it's my first post here and I read the policy for new threads well, so I've tried to stick to it as much as I could.

[RcktMan77]

Without access to the mesh, it is difficult to answer your first question--perhaps the second as well. If you're able to share a Pointwise project file, then I may be able to take a closer look. Note, for these types of questions it's usually best to contact Pointwise support at support@pointwise.com with your customer ID and a description of the issue.

Looking at the screenshots you provided of your mesh, I will say there seems to be a number of places where you have a very large jump between adjacent cell sizes which is very undesirable and will likely lead to inaccuracies in your solution.

It also appears that you may have meshed the interior of the solid wall boundary of your blade unnecessarily. Including it as part of your simulation's control volume may be appropriate if you're considering a fluid-structure interaction type simulation, but probably shouldn't be meshed otherwise.

The aspect ratio in Pointwise is calculated uniquely for each type of cell (i.e. tetrahedra, pyramids, prisms, hexahedra). More about how Pointwise defines aspect ratio can be found by watching this video. FLUENT may calculate things differently (e.g. using the cell centers, rather than the nodes themselves).

[Hamid.de]

Thank you sir for your explanatory reply.I do agree with your statement about mesh quality issues, after some try and error i've came up with a mesh that the skewness of elements in sensitive places of the domain is good enough and the warning message in fluent just got away. But right now i'm struggling with a new problem which is bugging me. In the second mesh that i'm working on it i want to create a boundary layer with very small yplus and for that i need to put the first node at 1e0-5 but the normal extrusion at the root of the blade with database constrained criteria isn't working with this small initial delta s, i've seen my geometry tolerance and at this specific place it was bigger than 1e-05. I've even tried to extrude it by free condition and project it on the database but the first elements seem somehow peneterating through the database result in highly distorted cells in there. So my question is, is there anyway to remedy that? Btw my whole domain was created in design modeler and in pointwise the rotary and stationary domain is imported as models with their relevant quilts
I'll upload the .pw for the second case ASAP, and I'll be thankfull if you could take a look at it.
Cheers
s.h.delbari

[RcktMan77]

Seyed,

If the tolerance of your geometry is larger than the spacing required by your mesh, then you're going to encounter all sorts of problems. See this recent Let's Talk Meshing webcast for a more detailed explanation of why this is the case.

You can try manually re-setting the grid point tolerance to something more appropriate for your case in the Properties Panel via the File menu, and then try your extrusion again. However this isn't guaranteed to work.

You should determine either the boundary proximity or assembly tolerance for the model you imported using the corresponding metrics found under the Examine menu. Using these metrics will help you to identify the areas where there are large gaps between adjacent surfaces that may be preventing you from assembling a model using an assembly tolerance closer to what your mesh spacing requires. Once you find these regions, then you will want to try to improve the geometry in these areas, so that the model can be assembled using tighter tolerances that are more amenable to the mesh spacing needed.

Optionally, if you're creating the CAD geometry yourself, you might try increasing the built-in tolerance of your CAD tool before creating the surfaces in order to avoid this issue altogether.

[Hamid.de]

Mr. Z. Davis
thank for your prompt response. I really appreciate it. these links that you've attached work very well for me. the idea behind the hierarchy of the databases in the pointwise was somehow uncanny for me. but the webcast enlightened me about this.moreover, the other sets of quick tips videos give some insight to me about the hyperbolic extrusion parameters, although I've read the help document but this sort of explanatory tutorials worth the most. I've done a little trick to deal with my second problem to get rid of the database-constrained extrusion and the idea to do so was obtained from one of the quick tip tutorials. I take this solution to build up my whole domain mesh and see what results will obtain from this (hope it works). otherwise, I'll do your advise and try to improve the cad file from the scratch. again, thank you for your responses and the whole bunch of informative references that you shared with me.
kindly
s.h.delbari