CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   Pointwise & Gridgen (http://www.cfd-online.com/Forums/pointwise/)
-   -   Beginning with Pointwise (http://www.cfd-online.com/Forums/pointwise/119510-beginning-pointwise.html)

rita June 18, 2013 21:48

Beginning with Pointwise
 
I looked for basic tutorials about what I need but I couldnt find, so I am asking it here.

I am using a program (SUMO) that generates the geometry of a winglet in igs format. I need to create the surface mesh over it. How can I do that? Is there any tutorial about this?

I could find only stuff about using a NACA airfoil and extruding it, but this is not my case.

Please, I need to this asap to my college work.

Thank you

rita June 18, 2013 21:51

This program (SUMO) gives me the surface mesh too, but it is really poor.
With Pointwise can I just redo this surface mesh with a better skewness?

dgarlisch June 19, 2013 10:30

As long as your surface geometry is clean, you literally click a few buttons to get a "default" surface mesh. To micro-manage the surface grid, you will first need to learn a little more.

There are tutorials included with the Pointwise install. Use the Help/Tutorial Workbook... menu.

Also, there are many good tutorial videos available on the Pointwise DIY training page.

The Pointwise webinars on youtube are also excellent.

rita June 20, 2013 15:55

1 Attachment(s)
I looked at some of these tutorials and now I can mesh my wing.
But when I try to mesh the winglet, it just doesnt happen.

You can see on the attached picture what I am doing. I click at Domains on Database Entities and nothing happens.

dgarlisch June 20, 2013 18:04

It is hard to tell from the image, but it looks like the toolbar indicates you are in structured grid mode.

If you want a structured surface grid, you need to be sure the connectors are properly balanced.

If you really want unstructured surface grids, you need to first click the unstructured grid toolbar button.

If that still does not work, then you may need to assemble the domains "manually" using the Create/Assemble special... tool.

Other than that, you will need to submit your grid model to PW support for more detailed help.

rita June 20, 2013 20:29

Thank you very much, the structured selection was the problem!

To finish my work, I would like to know how can I save in .cas format.

rita June 20, 2013 20:58

1 Attachment(s)
I have just noticed that not all points are being used to build the mesh. As you can see in the picture attached, my l eading edge is not smooth.

rita June 21, 2013 00:41

1 Attachment(s)
Another problem is showed on the picture attached here.
Two faces that intersect each other has nodes that are not merged.

dgarlisch June 21, 2013 10:58

Quote:

To finish my work, I would like to know how can I save in .cas format.
When a new PW file is created, the export (CAE) solver defaults to CGNS.

If you want a .cas (Fluent case) file, use the CAE/Select Solver... menu and change the solver to "ANSYS FLUENT".

Once the solver is specified, you can use CAE/Set boundary conditions... and CAE/Set volume conditions.... The available BC and VC types change depending on the current solver.

To export grid with its BC/VC information, use File/Export/CAE....

FYI... At any time, you can export grid only data (without any BC/VC information), using File/Export/Grid.... Grid only export does not care which CAE solver is currently set.

dgarlisch June 21, 2013 11:09

Quote:

Originally Posted by rita (Post 435165)
I have just noticed that not all points are being used to build the mesh. As you can see in the picture attached, my leading edge is not smooth.

It looks like you have coincident, duplicate connectors along these edges. The domains on the adjacent surfaces are using these different connectors.

Normally, connectors are automatically merged. However, since these connectors have a different number and distribution of points, they are not auto-merged.

You must make sure there is only one connector along these edges. The domains on database surfaces tool does this automatically, so I am not sure how you ended up with this grid.

You should also look at the Pointwise Solid modeling tools. They help you better control the logical surface/grid regions. If the user manual or tutorials are not enough, you can call Pointwise support.

rita June 25, 2013 14:51

The problem was my database that had lots of coincident lines.
Now it is solved, but I still have a problem.
When I create the connectors using Connectors on Databse Entities, I have to do some adjusments using a new Spacing setting. Then, I select the hole figure and click Domains on Database Entities. But it ignores the new Spacing that choose and the domains are built over the older connectors.... Why it does not use the new connectors spacing?

Another issue is about structures mesh. What are the balance requirements to allow this type of mesh? When I try to mesh the wing, just the plane part get meshed, but the winglet dont.

dgarlisch June 25, 2013 15:29

Quote:

Originally Posted by rita (Post 435932)
The problem was my database that had lots of coincident lines.
Now it is solved, but I still have a problem.
When I create the connectors using Connectors on Databse Entities, I have to do some adjusments using a new Spacing setting. Then, I select the hole figure and click Domains on Database Entities. But it ignores the new Spacing that choose and the domains are built over the older connectors.... Why it does not use the new connectors spacing?

Not sure. I would need to try this. Can you attach your pw file to this post along with detailed steps to repeat? Or better yet, call Pointwise support.

Quote:

Originally Posted by rita (Post 435932)
Another issue is about structures mesh. What are the balance requirements to allow this type of mesh? When I try to mesh the wing, just the plane part get meshed, but the winglet dont.

Structured meshes are topologically rectangular (I x J) and MUST have the same number of points on "opposite" edges. That is, the minI and maxI edges must have same number of points (Ni) and minJ and maxJ edges must have same number of points (Nj). However, Ni and Nj can be different.

Keep in mind, an "edge" can be composed of multiple connector entities. As long as the balance is maintained.

In the diagram below, the top edge is composed of two connectors. The bottom edge only has one connector. However, the number of points on each of these opposing edges is the same (balanced).

Code:

  o = connector end point (node)
  x = connector internal point
  . = domain internal point

o--x--x--o--x--x--o
|                |
x  .  .  .  .  .  x
|                |

x  .  .  .  .  .  x
|                |
o--x--x--x--x--x--o


rita June 25, 2013 15:50

1 Attachment(s)
I balanced, but it is not meshing yet the selected quilt as attached. Is it balanced, right?

rita June 25, 2013 15:55

Sorry, you asked the .pw file.

http://www.4shared.com/file/diX_qyqn/teste.html

dgarlisch June 26, 2013 10:34

Quote:

Originally Posted by rita (Post 435942)

I cannot access the file on the download site. Please just zip it and attach to this forum.

If that fails, just email the zipped file to support@pointwise.com with the subject line "debug file for dgarlisch".

Archiving (zip, gzip, rar, etc) the file is best because it is smaller and zip files have a checksum that ensures the data was not corrupted during transport.

Honey July 22, 2015 08:19

Dear David,

I have similar problem in creating a structured domain on database entity.

After importing the database (in stl format), I tried "Domains on Database Entities" with active icon of "structure". It has generated connectors but not capable to make the structured domain. The connectors have equal number of grid points which means it meets the requirement to make a structured domain, right? However, there was no problem in creating "Unstructured, Domains on Database Entities" but in my case, I strongly need a structured one.

So, I tried to split the connectors (generated by Domains on Database Entities). Only then, software was able to generate a structured domain (from selected connectors). BUT, the generated domain did not use the database, ONLY the connectors (or lets say the Database Boundaries). However, the same steps has WORKED with unstructured grid.

I would highly appreciate if you guide me how to solve this problem??

Kind regards,
Honey

dgarlisch July 22, 2015 10:26

If you can, please attach the STL file to this post. And some images.

There is not much I or anyone else can do without more details.

Please read:
http://www.cfd-online.com/Forums/poi...-get-help.html

Honey July 22, 2015 11:18

Quote:

Originally Posted by dgarlisch (Post 556520)
If you can, please attach the STL file to this post. And some images.

There is not much I or anyone else can do without more details.

Please read:
http://www.cfd-online.com/Forums/poi...-get-help.html


Here is the link to the stl file: https://onedrive.live.com/redir?resi...hint=file%2c7z

Thank you in advance for your time and help!

dgarlisch July 22, 2015 13:15

1 Attachment(s)
Okay.

The main problem is that the terrain STL data is located VERY far away from the global origin (0,0,0). This effectively kills any precision you have in the grid. The fine details of the STL data get lost in numerical precision.

To fix:
After import, I moved the STL database object to the origin. Then the structured domain on database worked fine.

Possible fixes (not tested by me):
If your process prohibits moving the STL data, start with a File/New... grid and set the model size to around 10,000 or 100,000 BEFORE you import the STL database. Then try structured domain on database.

Suggestion:
If your solver supports it, I also suggest you split the grid into two domains. One domain over the detailed area. One domain over the flat area. That way, you can reduce the grid point count in the flat area where you don't have any flow details. See attached image.

Honey July 22, 2015 17:46

1 Attachment(s)
Quote:

Originally Posted by dgarlisch (Post 556558)
Okay.

The main problem is that the terrain STL data is located VERY far away from the global origin (0,0,0). This effectively kills any precision you have in the grid. The fine details of the STL data get lost in numerical precision.

To fix:
After import, I moved the STL database object to the origin. Then the structured domain on database worked fine.

Possible fixes (not tested by me):
If your process prohibits moving the STL data, start with a File/New... grid and set the model size to around 10,000 or 100,000 BEFORE you import the STL database. Then try structured domain on database.

Suggestion:
If your solver supports it, I also suggest you split the grid into two domains. One domain over the detailed area. One domain over the flat area. That way, you can reduce the grid point count in the flat area where you don't have any flow details. See attached image.

Dear David,

Sure, I will split the domain into several parts and will have different grid resolutions for each based on the aim. But, before this I need to solve the problem of structured grid.

Though, it took some time but my computer was able to finish the process and move the terrain to the location of the origin. The number of grid points has been take cared. However, the structured domain on database has created ONLY the two connectors but not the domain (see attached image). The same result has been achieved after relocating/nearing the origin to (almost) the centre part where there is more detailed change.

Furthermore, I tried with changing the model size (file>properties>Tolerances) from 10 to 1e-6 before importing the STL file and then created structured domain on database but again it did not work.

I wonder where I do wrong!? you get it work but I can not :( Kindly help!

May I request you to attach the image of the structured grid close to the fine details of the terrain,too?


All times are GMT -4. The time now is 02:07.