CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > STAR-CCM+

Non uniform trimmer mesh?

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

Reply
 
LinkBack Thread Tools Display Modes
Old   April 20, 2011, 18:15
Default Non uniform trimmer mesh?
  #1
New Member
 
Anonymous
Join Date: Apr 2011
Location: Rotherham, England
Posts: 13
Rep Power: 6
freddyk is on a distinguished road
Hello all,

i'm performing analysis of flow over a step using a trimmer mesh and would really like to experiment with variable mesh sizing. The obvious application would be to make the mesh finer around key points of my (basic) object.

In addition the flow over the step comes in axially and thus the depth (z axis) doesnt matter much, is it possible to set the mesh to be wider in this direction, if so how?

Thanks!
freddyk is offline   Reply With Quote

Old   April 21, 2011, 03:48
Default
  #2
Senior Member
 
Join Date: Oct 2009
Location: Germany
Posts: 637
Rep Power: 12
abdul099 is on a distinguished road
It's possible to set a anisotropic trimmer size in a volumetric control. However, this affects only the mesh far from boundaries. The mesh at boundaries will always have the same size in both directions.
abdul099 is offline   Reply With Quote

Old   April 21, 2011, 19:43
Default thanks
  #3
New Member
 
Anonymous
Join Date: Apr 2011
Location: Rotherham, England
Posts: 13
Rep Power: 6
freddyk is on a distinguished road
Quote:
Originally Posted by abdul099 View Post
It's possible to set a anisotropic trimmer size in a volumetric control. However, this affects only the mesh far from boundaries. The mesh at boundaries will always have the same size in both directions.
That's a little dissapointing since its currently generating 100 nodes of depth whereas 10 would probably suffice - the flow is completely stable accross the depth (ie im using no slip walls with a simple x-direction input flow over a step in the y direction).

How do I set up a higher concentration around the step though, thats a decent consolation. I couldn't find a clear enough example in the training guide so any help is appreciated greatly!
freddyk is offline   Reply With Quote

Old   April 28, 2011, 16:56
Default
  #4
Senior Member
 
Join Date: Oct 2009
Location: Germany
Posts: 637
Rep Power: 12
abdul099 is on a distinguished road
It seems to be disappointing, but just have a look in the user guide, there's an explanation why CD-adapco choose not to give that option...
When the flow is really 2-dimensional, you can convert the mesh to 2D. This will save a lot of cells.

To refine the mesh near the step, you can set up a volumetric control.
In v5.02 - v6.02 (don't know about the older versions), go to Tools -> Volume shapes (at the end) -> right-click and choose a new one. When a scene is open, you can drag some points to define the size of the volume shape.
After that, you go to the mesh continuum to volumetric controls, right-click and choose new and choose the volume shape as input part. Now you can set the mesh values for your meshing models in that volumetric control.
The value used for meshing is usually the one with the lowest size. So you can't coarse the mesh with a volumetric control but refine it.
abdul099 is offline   Reply With Quote

Old   April 29, 2011, 09:21
Default
  #5
New Member
 
Anonymous
Join Date: Apr 2011
Location: Rotherham, England
Posts: 13
Rep Power: 6
freddyk is on a distinguished road
That certainly makes sense, if i was doing experimental work rather than a case study then that would be fine! I've played with anisotropic settings in the volume control node and that works, give or take some odd problems. For example the width is 0.01m and i need 8 nodes accross that gap, hence setting z size to 0.00125m should do the trick. however STAR produces 10 accross, very odd. I've got localisation working very nicely, that was just a case of playing with the curve proximity and surface proximities and learning what the parameters control. I am fairly new to STAR and it seems like an art rather than a science - sometimes putting in odd values gives the right mesh!

Im not sure what you mean about dragging points for the refinement, i've used proximity for that, are you suggesting this is an alternative / better way?
freddyk is offline   Reply With Quote

Old   May 1, 2011, 06:30
Default
  #6
Senior Member
 
Join Date: Oct 2009
Location: Germany
Posts: 637
Rep Power: 12
abdul099 is on a distinguished road
When you can do it with proximity refinement, that's fine. I've suggested to use volumetric controls, which are another option to partially refine the mesh.
That are just some simple shapes or parts which define an area where the mesh should have a specific property.
The input part for a volumetric control is either a part (from the parts node where imported geometry can be found) or a volume source (from the tools node). A volume source is one of the simple shapes, a block, a sphere, a cylinder etc. When you create one of them, you will see some points to drag, which will change the size and position of the volume shape...
Just try it and you will understand.

And no, it is no art. A specific input gives a specific output. Sometimes it is not what the user expected, sometimes it could be a bug (which should be reported), but anytime there is a reason for the result.
abdul099 is offline   Reply With Quote

Old   May 17, 2011, 16:23
Default
  #7
New Member
 
Anonymous
Join Date: Apr 2011
Location: Rotherham, England
Posts: 13
Rep Power: 6
freddyk is on a distinguished road
Quote:
Originally Posted by abdul099 View Post
When you can do it with proximity refinement, that's fine. I've suggested to use volumetric controls, which are another option to partially refine the mesh.
That are just some simple shapes or parts which define an area where the mesh should have a specific property.
The input part for a volumetric control is either a part (from the parts node where imported geometry can be found) or a volume source (from the tools node). A volume source is one of the simple shapes, a block, a sphere, a cylinder etc. When you create one of them, you will see some points to drag, which will change the size and position of the volume shape...
Just try it and you will understand.

And no, it is no art. A specific input gives a specific output. Sometimes it is not what the user expected, sometimes it could be a bug (which should be reported), but anytime there is a reason for the result.

Excellent advice, i appreciate it. I have a custom control using a block shape now, but it doesn't affect the generated mesh. Within the block i'd like double sized cells for example, but the same mesh occurs when i use the block as when i dont. Any ideas what has gone wrong?
freddyk is offline   Reply With Quote

Old   May 22, 2011, 07:29
Default
  #8
Senior Member
 
Join Date: Oct 2009
Location: Germany
Posts: 637
Rep Power: 12
abdul099 is on a distinguished road
Yes, I've got an idea. It's quite simple: You can NOT coarse a mesh with a volumetric control. All you can do is to refine a mesh.
When there are several settings affecting one boundary, always the finest one will be considered.
You can try to set a coarser size in general and refine all but the former volumetric control.
abdul099 is offline   Reply With Quote

Old   May 23, 2011, 04:20
Default
  #9
New Member
 
Anonymous
Join Date: Apr 2011
Location: Rotherham, England
Posts: 13
Rep Power: 6
freddyk is on a distinguished road
Quote:
Originally Posted by abdul099 View Post
Yes, I've got an idea. It's quite simple: You can NOT coarse a mesh with a volumetric control. All you can do is to refine a mesh.
When there are several settings affecting one boundary, always the finest one will be considered.
You can try to set a coarser size in general and refine all but the former volumetric control.
I got there in the end, the reason for the behavior was simple enough, it was just taking common factors such that a whole number of cells fit in the inlet as in the bottom of the step so it was just a case of being patient and working out what sizes were actually viable solutions.

I think the conclusion here is rather obvious, CFD packages are NOT meant to be used for trivial investigations - I was needing exact grid spacings which isn't really important for true engineering, in which rough estimates against target sizes are all that would be needed.

Thanks for the patience anyway, and the volume shape method you taught me works great around the step.
freddyk is offline   Reply With Quote

Reply

Tags
non-uniform mesh, trimmer

Thread Tools
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 On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
trimmer mesh vs Polyhedral mesh Marcelo CD-adapco 2 February 4, 2015 10:00
3D Hybrid Mesh Errors DarrenC ANSYS Meshing & Geometry 11 August 5, 2013 06:42
Converting a mesh with splitted cells using fluentMeshToFoam jlpelerin OpenFOAM Other Meshers: ICEM, Star, Ansys, Pointwise, GridPro, Ansa, ... 4 April 25, 2011 16:56
buoyantSimpleRadiationFoam msarkar OpenFOAM 0 February 15, 2010 07:22
Icemcfd 11: Loss of mesh from surface mesh option? Joe CFX 2 March 26, 2007 18:10


All times are GMT -4. The time now is 03:46.