CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Mesh Generation & Pre-Processing Software > Pointwise & Gridgen

Meshing the airship's hull

Register Blogs Members List Search Today's Posts Mark Forums Read

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   July 26, 2015, 21:51
Default Meshing the airship's hull
  #1
New Member
 
NGUYEN TRUONG GIANG
Join Date: Sep 2013
Posts: 18
Rep Power: 9
giangcoikx is on a distinguished road
Hi everyone,

I am a student, very first experience with Pointwise. I am facing a problem that I would like to get your helps. Our school has a small airship, and we have drawn its hull on Catia, now import it in into Pointwise for meshing. Our solver is FLUENT v15.

1. In CATIA, we draw an 1/10th scale of the airship. The drawing's length is 600mm ( the original length is 6m). I know Pointwise is dimensionless, but when I import the drawing in igs file, Pointwise shows the distance from the nose to the tail is 600.
The hull's length has medium curvature, it is like here, the wind condition is about 15m/s. From your experience, how many points do you think is necessary to capture the hull's curvature on our 600mm drawing without strong difference with the drawing's curves? I use here about 200 points.

2. I used the unstructured mesh for the hull's surface domain. But when I tried to concentrate delta s on the nose, it appears like the pictured I attached. I think it is meaningless since the hull is axisymmetrical, but a number of triangles distributed along the skeleton's curve are considerably
bigger than those in another area.

So how can I resolve it? I mean to focus points on the nose without influencing asymmetry as like the picture I attach here

As well I do not see the elliptic solver for unstructured mesh. Do you think my cells attach well to the surface?

3. I use T-rex function with collision buffer =2 as recommended all my surface meshes are as good as Mr. Carrigan suggested here, as well as max included angle are ok, but when I export the file to case file used by FLUENT. The equiangle skewness at some cell is still > 0.98. I have combined cells, it reduces number of cells considerably. How can I resolve this problem?

4. Instead of T-rex, I have tried to use a normal extrusion for boundary layer, but is it as good as T-rex, in terms of smooth transition? When I checked it in FLUENT, FLUENT said that "this page is not applicable under current settings", so what is wrong with my mesh?

5. For the far field, I created the region with radius = 3.5 length of the airship, from your experience with such a slow speed vehicle, do you think it is enough? I know I should try another things to obtain grid independence, but having some range is easier to me to guess.

Thank you for your answers.

Do you need any my mesh's pictures?
Attached Images
File Type: jpg Screenshot 2015-07-27 02.35.07.jpg (60.9 KB, 62 views)
File Type: jpg Screenshot 2015-07-27 02.41.06.jpg (35.7 KB, 49 views)
File Type: jpg Screenshot 2015-07-27 02.46.30.jpg (97.4 KB, 57 views)
File Type: jpg length.jpg (12.6 KB, 38 views)
File Type: jpg GenericLauncherMesh_01.jpg (38.5 KB, 53 views)
giangcoikx is offline   Reply With Quote

Old   July 27, 2015, 11:08
Default
  #2
Senior Member
 
Chris Sideroff
Join Date: Mar 2009
Location: Ottawa, ON, CAN
Posts: 415
Rep Power: 18
cnsidero is on a distinguished road
All good questions, none with black/white answers. I'll do my best.

Quote:

1. In CATIA, we draw an 1/10th scale of the airship. The drawing's length is 600mm ( the original length is 6m). I know Pointwise is dimensionless, but when I import the drawing in igs file, Pointwise shows the distance from the nose to the tail is 600.
The hull's length has medium curvature, it is like here, the wind condition is about 15m/s. From your experience, how many points do you think is necessary to capture the hull's curvature on our 600mm drawing without strong difference with the drawing's curves? I use here about 200 points.
Number of points resolving curvature is never obvious nor straightforward. I'll put it in the context of a circle. If I'm trying to resolve the curvature of flow around a circle (2D cylinder), my experience has been that a grid point every two degrees is sufficient. In your case the shape is more elliptical, meaning the curvature changes, so one should use a non-uniform spacing. Closer spacing at ends with high curvature and lesser elsewhere (as I see you've done). See below for my example.

Quote:
2. I used the unstructured mesh for the hull's surface domain. But when I tried to concentrate delta s on the nose, it appears like the pictured I attached. I think it is meaningless since the hull is axisymmetrical, but a number of triangles distributed along the skeleton's curve are considerably
bigger than those in another area.

So how can I resolve it? I mean to focus points on the nose without influencing asymmetry as like the picture I attach here
I believe you just need to increase the Boundary Decay (Grid>Solver, Attributes) on the domains. Increase it to 0.98-0.99. See the first image for an example I threw together for the 6:1 prolate spheriod where I've used 0.99.

Quote:
As well I do not see the elliptic solver for unstructured mesh. Do you think my cells attach well to the surface?
The elliptic solver is a structured meshing only technique. Speaking of which, since your geometry is so simple, you could consider using a structured mesh (see second image).

Quote:
3. I use T-rex function with collision buffer =2 as recommended all my surface meshes are as good as Mr. Carrigan suggested here, as well as max included angle are ok, but when I export the file to case file used by FLUENT. The equiangle skewness at some cell is still > 0.98. I have combined cells, it reduces number of cells considerably. How can I resolve this problem?
You likely won't entirely. Even though Fluent indicates high skew cells, it will still likely run OK and you can get decent results. It depends on how many high skew cells and where they're located. Can you provide this info?

Quote:
4. Instead of T-rex, I have tried to use a normal extrusion for boundary layer, but is it as good as T-rex, in terms of smooth transition? When I checked it in FLUENT, FLUENT said that "this page is not applicable under current settings", so what is wrong with my mesh?
That is a strange message from Fluent. There should be no reason why that mesh won't work. Can you provide more info (or images as to what's going on).

Quote:
5. For the far field, I created the region with radius = 3.5 length of the airship, from your experience with such a slow speed vehicle, do you think it is enough? I know I should try another things to obtain grid independence, but having some range is easier to me to guess.
This really depends on what quantity you're after. Since drag on streamlined bodies tends to be quite low, it is the most sensitive to farfield proximity. Simulations I have seen of submarine hulls (which is geometrically similar to yours) sometimes use farfields of this size. What you suggested would be a good starting point but I would suggest trying a couple or larger sizes and monitoring the influence on the quantity of interest to you.

Regards, Chris
Attached Images
File Type: jpg prolate-uns-bd-0.99.jpg (53.6 KB, 45 views)
File Type: jpg prolate-struc.jpg (24.1 KB, 44 views)
cnsidero is offline   Reply With Quote

Old   August 16, 2015, 22:50
Default
  #3
New Member
 
NGUYEN TRUONG GIANG
Join Date: Sep 2013
Posts: 18
Rep Power: 9
giangcoikx is on a distinguished road
Dear Dr. Sideroff,

Sorry for replying late, because after running calculation, I detect a seriously wrong results, the drag of the airship is approximately zero. SO I take a lot of time to review both my mesh and my setup in FLUENT

Quote:
Originally Posted by cnsidero View Post
You likely won't entirely. Even though Fluent indicates high skew cells, it will still likely run OK and you can get decent results. It depends on how many high skew cells and where they're located. Can you provide this info?
Yes, I can force FLUENT running, there are only a few cells of bad quality.


That is a strange message from Fluent. There should be no reason why that mesh won't work. Can you provide more info (or images as to what's going on).
This message disappears when I setup the mesh fully. It appears only when I click on "check case" button immediately after opening the mesh.


This really depends on what quantity you're after. Since drag on streamlined bodies tends to be quite low, it is the most sensitive to farfield proximity. Simulations I have seen of submarine hulls (which is geometrically similar to yours) sometimes use farfields of this size. What you suggested would be a good starting point but I would suggest trying a couple or larger sizes and monitoring the influence on the quantity of interest to you.

As I read on others book, the volumetric drag coefficient lies somewhere between 0.02 and 0.03. Although I have extended the aft-wake to 5L, and the pressure on "pressure outlet" surface agrees well with the distance, the drag coefficient is still ridiculously low. I attach here my picture of pressure distribution on this pressure outlet.

Regards, Chris
Attached Images
File Type: jpg static pressure on pressure outlet surface.jpg (38.1 KB, 29 views)
giangcoikx is offline   Reply With Quote

Old   August 16, 2015, 23:23
Default
  #4
New Member
 
NGUYEN TRUONG GIANG
Join Date: Sep 2013
Posts: 18
Rep Power: 9
giangcoikx is on a distinguished road
Dear Dr. Sideroff,

Let me explain my mesh here. Here is my mesh, it is save, no virus.

For simplicity of dynamic similarity, I draw again my mesh on full-size airship.
L = 6.5 meter,
Max diameter D = 1.73 m,
Volume = 14 m^3

I have watched your video on youtube. However, due to our geometry, the structured mesh at the nose and tail causes 1 bad quality cell on each direction that will show a distorted connectors during extrusion process (I attached the picture here). Meanwhile the unstructured mesh does not cause this problem but it generates more cells the structured type. Therefore, I decide to design a hybrid type with unstructured mesh on the nose and structured mesh on the mid-body.

Unfortunately, one more problems appears, I have chosen both surfaces at the same time, applied the same attributes, it still has shown a weird curve on the boundary of extrusion domain on the symmetry plane. Except for being look weird, Pointwise does not warn anything during examination. From your expert's view, could you help me explain this phenomena?

In addition, I have created a front and aft wakes as you suggested. However, it has a small number of bad quality cells in terms on equivolume skewness near the outer and inner surfaces of the wakes. but I heard you said that this kind of quality checker does not matter much, right?

About my computational domain, both yplus estimation and after calculation are below 1 (I use k-w SST turbulence and Spalart Allmaras model).
Bloackage ratio is 1%, 30m (5 times of its length) velocity inlet boundary in front of the hull and 30m behind. The pressure distribution on pressure outlet agrees well with my expect. (All calculations are in standard atmosphere)

Total cells = about 2.5 mil.

I would like to hear your review about my mesh. Does it fine enough? Is it the cause of error I got?
Here is my pictured of Cd, it is so disappointing, , especially the viscous force.

I have tried my best to review everything including theory, but I have not found any source of errors yet. So I decide to ask experts.

Thank you so much.
Attached Images
File Type: jpg distorted nose extrusion connector.jpg (74.5 KB, 36 views)
File Type: jpg 1.jpg (89.9 KB, 36 views)
File Type: jpg y plus after calculation.jpg (35.1 KB, 26 views)
Attached Files
File Type: txt force report .txt (2.2 KB, 3 views)
giangcoikx is offline   Reply With Quote

Old   August 17, 2015, 10:16
Default
  #5
New Member
 
NGUYEN TRUONG GIANG
Join Date: Sep 2013
Posts: 18
Rep Power: 9
giangcoikx is on a distinguished road
Dear Dr. Sideroff,

As far as I understood, the "solve" function for structured mesh is to enhance domain's mesh matching with a geometrical surface. However, sometimes, I see it gives a worse result in terms of maximum included angle and equiangle skewness. So what does it mean? What should I do?
For example, the wake domain on the symmetry plane.

Thank you so much.
giangcoikx is offline   Reply With Quote

Reply

Thread Tools Search this Thread
Search this Thread:

Advanced Search
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are Off
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Error in meshing a Ship hull using snappyhexmesh Sachin m OpenFOAM Pre-Processing 1 August 28, 2014 00:27
Hydrostatic Pressure and Gravity miliante OpenFOAM Running, Solving & CFD 132 October 7, 2012 23:50
Meshing a Hull davedave121 Siemens 1 May 17, 2010 21:48
[GAMBIT] Meshing complex geometry (Hull) vmeertens ANSYS Meshing & Geometry 26 March 29, 2010 11:24


All times are GMT -4. The time now is 05:14.