CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > ANSYS Meshing & Geometry

[GAMBIT] Set up problem for moving mesh

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

Reply
 
LinkBack Thread Tools Display Modes
Old   February 22, 2010, 08:11
Default Set up problem for moving mesh
  #1
Member
 
Martin H.
Join Date: May 2009
Posts: 31
Rep Power: 8
bobmalaria is on a distinguished road
Dear group,

I try to model Cemical vapour deposition with a moving substrate plate. I found an article:

Using Dynamic Mesh Models to Simulate
Electrostatic Spray-Painting
//by Q. Ye
// Institut f¨ur Industrielle Fertigung und Fabrikbetrieb Universit¨at Stuttgart
Nobelstr. 12, D-70569 Stuttgart, Germany

which is in principle very similar to what I want to achive. Please have a look at the attached jpeg.

My inlet slot is a much simpler geometry (rectangular volume) and I imported it, and substracted it from a bigger (environment)volume.
The substracted volume was retained and I used a face as my inlet.

After importing into Fluent, this inlet is not found and skipped. Do I have to split the face with the volume?

The second question would be: How can I create a mesh as the one shown in the picture. I guess I have to create a virtual cylinder/cube around my geometry and mesh it. But how do I implement the size function so that the mesh becomes crude on the outside?

Best regards
Attached Images
File Type: jpg 1.jpg (41.1 KB, 113 views)
bobmalaria is offline   Reply With Quote

Old   February 23, 2010, 03:26
Default
  #2
Super Moderator
 
-mAx-'s Avatar
 
Maxime Perelli
Join Date: Mar 2009
Location: Switzerland
Posts: 2,961
Rep Power: 30
-mAx- will become famous soon enough
*check the warning in the transcript window while exporting
*check if you don't have superposed entitis at your inlet
*check in the Boundyry Panel if your inlet is still set (if it is already referenced in anoter Boundary, Gambit will skip it) --> one entity can only appear under one Boundary

To your 2nd question, apply a SF with outter edges from your cube/cylinder as source, and that's it
__________________
In memory of my friend Hervé: CFD engineer & freerider
-mAx- is offline   Reply With Quote

Old   March 2, 2010, 07:42
Default
  #3
Member
 
Martin H.
Join Date: May 2009
Posts: 31
Rep Power: 8
bobmalaria is on a distinguished road
Hi,

I tried to follow your hints but I still have one problem. If I draw a zylinder around my inlet, the fluid circulates inside this zylinder instead of spreading out in the whole domain. I specified the zylinder as a FLUID continuum type in gambit.

Do I have to split the zylinder volume with the bigger cube around it first?

Best regards
bobmalaria is offline   Reply With Quote

Old   March 2, 2010, 07:59
Default
  #4
Super Moderator
 
-mAx-'s Avatar
 
Maxime Perelli
Join Date: Mar 2009
Location: Switzerland
Posts: 2,961
Rep Power: 30
-mAx- will become famous soon enough
post a picture
__________________
In memory of my friend Hervé: CFD engineer & freerider
-mAx- is offline   Reply With Quote

Old   March 2, 2010, 08:06
Default
  #5
Member
 
Martin H.
Join Date: May 2009
Posts: 31
Rep Power: 8
bobmalaria is on a distinguished road
Hi,

thank you for the quick response.
Stupid me :-) after splitting the volumes with each other it works fine. Now I will check how it works when I apply my UDF for translational movement.

Would you suggest to try layering and to use hex meshes first and if that is not satisfactory move on to tet meshes with remeshing?
If I understood it correctly, with remeshing enabled in fluent I have to use tet meshed!?
bobmalaria is offline   Reply With Quote

Old   March 2, 2010, 09:01
Default
  #6
Super Moderator
 
-mAx-'s Avatar
 
Maxime Perelli
Join Date: Mar 2009
Location: Switzerland
Posts: 2,961
Rep Power: 30
-mAx- will become famous soon enough
yes with remeshed option, you need to work with tetras only.
Layering can also be used, but it depends on your geometry. You can also use sliding mesh + layering
__________________
In memory of my friend Hervé: CFD engineer & freerider
-mAx- is offline   Reply With Quote

Old   March 3, 2010, 09:03
Default
  #7
Member
 
Martin H.
Join Date: May 2009
Posts: 31
Rep Power: 8
bobmalaria is on a distinguished road
Hi,

after sorting out the previous mistakes, I am stuck at the next thing I want to do.

Please have a look at the attached picture.

I want to move the gray brick in x direction of the model. I wrote a UDF with the DEFINE_CG_MOTION macro. Everything seems to work, but after starting the iteration in FLUENT with, say, the layering model, I get an error after a few iterations "negative volumes"

Looking at the grid, it seems that the brick does not move and simply the mesh cells are stretched.

Could someone give me a description on how to create an object that can move within the domain please?

Thank you
Attached Images
File Type: jpg save1.jpg (80.1 KB, 53 views)

Last edited by bobmalaria; March 3, 2010 at 09:46.
bobmalaria is offline   Reply With Quote

Old   March 3, 2010, 10:11
Default
  #8
Super Moderator
 
-mAx-'s Avatar
 
Maxime Perelli
Join Date: Mar 2009
Location: Switzerland
Posts: 2,961
Rep Power: 30
-mAx- will become famous soon enough
If the grey brick will move using layering, you have to
check the tutorial "Using Dynamic Mesh"
It is based on layering, and everything is described.
Your issue sounds like your MDM parameters aren't well set
__________________
In memory of my friend Hervé: CFD engineer & freerider
-mAx- is offline   Reply With Quote

Old   March 4, 2010, 13:05
Default
  #9
Member
 
Martin H.
Join Date: May 2009
Posts: 31
Rep Power: 8
bobmalaria is on a distinguished road
Hi,

the dynamic mesh tutorial helped. I looked at it before but it seems that I did not read it very carefully though.
I forgot to specify the volume around my moving body as a stationary zone.

Also I only applied my UPF to the walls of my moving body and forgot to apply it on its interior as well.

Now everything seems to work so far :-)
bobmalaria is offline   Reply With Quote

Old   March 17, 2010, 10:07
Default
  #10
Member
 
Martin H.
Join Date: May 2009
Posts: 31
Rep Power: 8
bobmalaria is on a distinguished road
Hi,

I had some time to work on my model again and I have another problem. I hope you can tell me what I am doing wrong.

  • Imagine you careate a volume X=50mm, y=10mm, z=10mm centered.
  • In this you create another volume x=5mm, y=5mm, z=5mm
Now I want to move the second (small) volume with my UDF. This works fine so far, but the small volume is always detected as an interior by FLUENT and I can not change that.

However I need the flow (say air) to move around the moving smaller volume.
What do I have to change in Gambit or Fluent to make the small volume a solid object which moves inside of the domain?

Thank You
bobmalaria is offline   Reply With Quote

Old   March 17, 2010, 10:47
Default
  #11
Super Moderator
 
-mAx-'s Avatar
 
Maxime Perelli
Join Date: Mar 2009
Location: Switzerland
Posts: 2,961
Rep Power: 30
-mAx- will become famous soon enough
why do you want to keep the small volume? Are the outter surfaces not enough?
Except if you want to compute conduction in solid, you don't need the solid mesh.
Your mesh should contain a hole, which defines your moving body.
If still want to keep it, try to define the volume as solid (Specidy continuum, icon next to BC), but I never tried that
__________________
In memory of my friend Hervé: CFD engineer & freerider
-mAx- is offline   Reply With Quote

Old   March 17, 2010, 11:00
Default
  #12
Member
 
Martin H.
Join Date: May 2009
Posts: 31
Rep Power: 8
bobmalaria is on a distinguished road
hi,

the idea behind everything is:

A gas flows through a inlet gap from the top onto the small volume, around it and exits through an outlet. so the small volume has to be a solid object. this solid volume moves (translation in x direction) back and forth under the gas stream

when i split the large volume with the small volume, fluent creates a shadow of the walls and the object seems not to move.

when i specify the small interior in gambit as a solid, fluent does not recognize that as solid and the gas flows straight through. i also tried to define it as fluid and change it to 'wall' then but fluent crashes with a floating point error.

basically i would need to move a cavity through the fluid domain. Any idea on that?
bobmalaria is offline   Reply With Quote

Old   March 17, 2010, 14:13
Default
  #13
Super Moderator
 
-mAx-'s Avatar
 
Maxime Perelli
Join Date: Mar 2009
Location: Switzerland
Posts: 2,961
Rep Power: 30
-mAx- will become famous soon enough
can you post an hand-sketch of your model?
__________________
In memory of my friend Hervé: CFD engineer & freerider
-mAx- is offline   Reply With Quote

Old   March 17, 2010, 15:52
Default
  #14
Member
 
Martin H.
Join Date: May 2009
Posts: 31
Rep Power: 8
bobmalaria is on a distinguished road
hi,

i hope this makes it more clear
Attached Images
File Type: jpg sketck.jpg (39.4 KB, 32 views)
bobmalaria is offline   Reply With Quote

Old   March 18, 2010, 02:16
Default
  #15
Super Moderator
 
-mAx-'s Avatar
 
Maxime Perelli
Join Date: Mar 2009
Location: Switzerland
Posts: 2,961
Rep Power: 30
-mAx- will become famous soon enough
I confirm what I said: delete the blue square, and set its outter edges as rigid body motion
On the picture you can see that the square is empty.
Sans titre.jpg
__________________
In memory of my friend Hervé: CFD engineer & freerider
-mAx- is offline   Reply With Quote

Old   March 18, 2010, 05:50
Default
  #16
Member
 
Martin H.
Join Date: May 2009
Posts: 31
Rep Power: 8
bobmalaria is on a distinguished road
hi,

thank you very much, this is helpful (and i could bang my head on the table)

Just to confirm, when you say 'delete' you mean 'subtract', right?

How did you manage to create a hex-mesh around the small volume. The only thing that seems to work is a tet mesh.

cheers
bobmalaria is offline   Reply With Quote

Old   March 18, 2010, 06:11
Default
  #17
Super Moderator
 
-mAx-'s Avatar
 
Maxime Perelli
Join Date: Mar 2009
Location: Switzerland
Posts: 2,961
Rep Power: 30
-mAx- will become famous soon enough
I mean delete. There should be no cell in the square. (enable shaded mode an check if the square is empty, like in my picture)
my example is 2d, so gambit recognizes mappable surface and mesh it with quad directly. (mapp schema automatically selected)
__________________
In memory of my friend Hervé: CFD engineer & freerider
-mAx- is offline   Reply With Quote

Old   March 18, 2010, 06:57
Red face
  #18
Member
 
Martin H.
Join Date: May 2009
Posts: 31
Rep Power: 8
bobmalaria is on a distinguished road
hi,

ok the difference is the 2D or 3D modeling. In 3D, the hex map scheme is not longer available.

I tried to rebuild the 2D model as you suggested. after deleting/substracting, i meshed the 2D face and defined the (former) walls of the little sqaure as a 'wall' boundary condition.

after importing it into fluent and applying my UDF, the object won't move. Would you mind to send me your gambit model and fluent case file?

I ll send you my email in a private message
bobmalaria is offline   Reply With Quote

Old   March 18, 2010, 07:09
Default
  #19
Super Moderator
 
-mAx-'s Avatar
 
Maxime Perelli
Join Date: Mar 2009
Location: Switzerland
Posts: 2,961
Rep Power: 30
-mAx- will become famous soon enough
with moving mesh, you don't just only need to define the moving walls.
You need to create moving zone, deforming surfaces, etc..
check the tutorial about Moving Mesh, it will help you to understand for sure
__________________
In memory of my friend Hervé: CFD engineer & freerider
-mAx- is offline   Reply With Quote

Old   March 30, 2010, 05:42
Default
  #20
Member
 
Martin H.
Join Date: May 2009
Posts: 31
Rep Power: 8
bobmalaria is on a distinguished road
hi,

i had some time to work on the model again. i have a working version now, however it only works with a tri mehs (in 2D). whenever i try to use a hex/rectangular mesh the remeshing seems not to work.

well, i can live with that for now and will do some more testing when i find the time to do so
bobmalaria is offline   Reply With Quote

Reply

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
Moving mesh Niklas Wikstrom (Wikstrom) OpenFOAM Running, Solving & CFD 122 June 15, 2014 06:20
Ansys 12 Workbench problem when generating volume mesh Sveink ANSYS 5 January 6, 2010 04:17
fluent add additional zones for the mesh file SSL FLUENT 2 January 26, 2008 12:55
Mesh Deformation Problem Virag Mishra CFX 0 October 9, 2007 00:37
How to control Minximum mesh space? hung FLUENT 7 April 18, 2005 09:38


All times are GMT -4. The time now is 16:38.