CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   ANSYS Meshing & Geometry (http://www.cfd-online.com/Forums/ansys-meshing/)
-   -   [ICEM] Mesh sizing - Rule of thumb !!! (http://www.cfd-online.com/Forums/ansys-meshing/113217-mesh-sizing-rule-thumb.html)

Far February 15, 2013 01:41

Mesh sizing - Rule of thumb !!!
 
I am very much confused about the mesh size for the tetra module. I really dont understand how I can assign the mesh sizes in beginning. I know we can do it by measuring the overall geometry size on particular location and using trial and error but this method does not seem to be robust and efficient.

Now my question is (with reference to octree):

1. How to define sizes on global level. Like scale factor, max element size and curvature and proximity.

2. How to define the sizes in part mesh set-up for :
a) local geometry (e.g. wing, aircraft etc)
b) For the far-field parts
c) For Fluid (material point)

mjgraf February 16, 2013 15:55

For me it depends (the universal answer). hehe.

I typically set the global scale factor 0.001, so if you have parasolid, typically in meters, this will allow me to think in millimeters.

I also ensure that the tri tolerance is small, 1e-6 for final meshing. HEXA use the b-surface option.

One can also think in scale of features to resolve. When thinking in mm this is easy. Also being restricted to the Octree growth formula simplifies things too.

Another indicator I use is the Surface Dev Quality metric to ensure I am resolving the geometry properly.

these are all pretty easy for the RANS models. Going to DES, SAS, etc. the mesh needs further refinement than just resolving the geometry and areas I know have large gradients or recirculations.

Just some thoughts.

Calculate and refine as necessary for things you may have missed like wall spacing, etc.

Quote:

Originally Posted by Far (Post 407944)
I am very much confused about the mesh size for the tetra module. I really dont understand how I can assign the mesh sizes in beginning. I know we can do it by measuring the overall geometry size on particular location and using trial and error but this method does not seem to be robust and efficient.

Now my question is (with reference to octree):

1. How to define sizes on global level. Like scale factor, max element size and curvature and proximity.

2. How to define the sizes in part mesh set-up for :
a) local geometry (e.g. wing, aircraft etc)
b) For the far-field parts
c) For Fluid (material point)


BrolY February 18, 2013 05:00

Maybe I didn't understand what's your problem is, but go to : Mesh -> Part Mesh Setup and Mesh -> Global Mesh Setup ...

Far February 21, 2013 14:03

My problem is " I always end up with ICEM stuck up in making mesh more than 30-40 million and progress bar is at 20% or less" . In my estimate I should get around one million mesh size for full volume.

I am always confused in :

1. Specifying the curve mesh parameters : Should I specify size or no of nodes. Will it be used in octree?

2. Surface mesh size: There are many large and small parts. If I specify the size as per smallest part then I have very large mesh due to over refinement in large parts. If I consider the largest part, I get the under resolved smaller parts.

3. Both curve mesh and surface mesh parameters are used for octree?

4. What is the role of the max element size.

In short I want the rule of thumb in setting the sizes for octree for any model and with one click on compute I get the one decent volume mesh.

mjgraf February 21, 2013 14:25

You probably have a max deviation set that is very small? I have had cases where using this creates really odd mesh densities that I feel should not be there. I have also had issues when using a UG generated parasolid and a simple surface, at least appears simple (cylinder for example) would take forever to mesh. I deleted the surface and used the remaining edge curves to create surface using ICEM surfacing and poof, issue gone.

1. just starting to investigate defining on curve and multiple material points, but to fully answer your question, refer to the Global Mesh Setup Tables in the ICEM CFD Help.

2. split by parts (be aware where curves and points go) and use the Part Mesh Setup. Then utilize the tetra size ratio to control the surface mesh growth from the small to large size parts (then for the volume, Delaunay Spacing Scaling Factor)

3. refer to 1.

4. allows control of the max element size on a part/curve/surface/body. Read the Help about Global Element Scale Factor. Ensure that Global Element Seed Size is larger or the max element size will not be what you expect. I have found an issue with Volume tetra max size where it can not be smaller than the Global Element Seed Size, but works for hexa-core, really odd.

A one click good mesh only comes with using similar models day-to-day. for the strange one that comes in that I am not sure, after running Build Topology and creating my parts, I use the Surface mesher part by part to fine tune. So much faster than waiting for the octree to complete for a large mesh just to look at the surface mesh. You also catch where the mesher messes up with the max deviation setting. When this happens I turn off max deviation, reduce my max element and then use the Surface Dev quality to make sure my deviation is within machining tolerance.


Quote:

Originally Posted by Far (Post 409369)
My problem is " I always end up with ICEM stuck up in making mesh more than 30-40 million and progress bar is at 20% or less" . In my estimate I should get around one million mesh size for full volume.

I am always confused in :

1. Specifying the curve mesh parameters : Should I specify size or no of nodes. Will it be used in octree?

2. Surface mesh size: There are many large and small parts. If I specify the size as per smallest part then I have very large mesh due to over refinement in large parts. If I consider the largest part, I get the under resolved smaller parts.

3. Both curve mesh and surface mesh parameters are used for octree?

4. What is the role of the max element size.

In short I want the rule of thumb in setting the sizes for octree for any model and with one click on compute I get the one decent volume mesh.


Far February 22, 2013 04:41

What is the effect of putting zero size?

I also want to know about hexa merge? How do we use it in tetra mesh generation process for the wings? (Reference Page No 70 ICEMCFD_Tips&Tricks2010.PDF

http://img801.imageshack.us/img801/9510/hexamerge.png

Far February 22, 2013 04:59

Quote:

Originally Posted by mjgraf (Post 409372)
You also catch where the mesher messes up with the max deviation setting. When this happens I turn off max deviation, reduce my max element and then use the Surface Dev quality to make sure my deviation is within machining tolerance.

Can you describe in detail the purpose of max deviation with some images if possible !!!


All times are GMT -4. The time now is 06:07.