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

CFX-10 mesh- element volume ratio

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

Reply
 
LinkBack Thread Tools Display Modes
Old   October 30, 2006, 14:08
Default CFX-10 mesh- element volume ratio
  #1
mike
Guest
 
Posts: n/a
Hi Everybody,

I am trying to improve the quality of my mesh. I am using cfx 10- mesh and checking the quality in cfx-10 post. whatever I do, I am getting element volume ratios more than 10 in some regions. even with setting expansion parameters 1.02, I could not get rid of the mesh having element volume ratio more than 10.

Any suggestions would be highly apreciated. Thanks,

Mike
  Reply With Quote

Old   October 30, 2006, 14:59
Default Re: CFX-10 mesh- element volume ratio
  #2
Robin
Guest
 
Posts: n/a
Hi Mike,

Check where this is occurring in your mesh by creating an isovolume of volume ratio (Volume Object using isovolume option). It is likely to occur between the last inflation layer and first layer of tets. Specifying the first node height and increasing the number of inflation layers can help. If you find that the number of layers is dropping in a particular region, try increasing the mesh density in this region.

The mesh quality criteria offer guidelines for avoiding common problems, but it is not strictly necessary to remove every bad element in your mesh. If the solver runs fine and the solution is OK, you can safely ignore it. Large element volume ratio's result in errors in the transient term (i.e. the element fluxes are not affected) and typically reveal themselves as poor convergence behavior (due to instability in the transient term, which is used to relax the equations in a steady state run).

If you don't have convergence problems and you have sufficient resolution, don't worry about it.

Regards, Robin
  Reply With Quote

Old   October 30, 2006, 15:26
Default Re: CFX-10 mesh- element volume ratio
  #3
mike
Guest
 
Posts: n/a
Hi Robin,

Thank you very much for the explanation. I had checked the quality as you suggested. Isovolumes show that the high element volume ratios are distributed thoughout the domain. And whatever I do, this scattered distrubition does not vary significatly. Slight improvements can be seen. I even tried first node hight and excessive amount of inflated layers, and it did not work out. In addition, I tried suppresing all control features, and just constant body spacing, and amazingly it did not work out either. i just can't understand how this is happening. I am using constant spacing thoughtout the domain (even without inflated layers), and still there are nodes having element volume ratios more than 10. By the way, I am trying to improve the mesh quality, since I have convergence problem.

thanks again for your help. I would be very glad to hear if you have additional comments.

regards,

Mike

  Reply With Quote

Old   October 30, 2006, 16:38
Default Re: CFX-10 mesh- element volume ratio
  #4
Robin
Guest
 
Posts: n/a
Hi Mike,

It's hard to say anything more without looking at the model. I suggest you send it into support for help. Convergence problems may not necessarily be mesh related either. Searching the forum will turn up many discussions on the topic.

As for getting a smooth mesh, the advancing front mesher will do it's best to maintain a smooth transition, but it is not always possible. As you refine the mesh it may improve. It also helps to specify a radius of influence around surface mesh controls. It could actaully get worse if you specify too low an expansion ratio, as the mesh may not expand sufficiently before meeting a mesh front advancing from an opposing side.

A couple other things you can try are to specify the default surface mesh control as "Volume Spacing" and only specify control on the important wall regions. Usually there is no reason to make "open" boundaries (i.e. inlets, outlets, fluid-fluid interfaces, etc.) any finer than the volume, so leave these under the default. The default body spacing should also be relatively close to the maximum surface spacing.

If you have a lot of small surfaces whose boundaries are not important (i.e. does not define a boundary condition or have sharp discontinuities in surface normal), try merging them into larger "virtual" surfaces using the VT feature. This will reduce the degree to which the mesh varies spatially.

If any of this actually helps, please let us know!!

Regards, Robin
  Reply With Quote

Old   October 31, 2006, 08:04
Default Re: CFX-10 mesh- element volume ratio
  #5
mike
Guest
 
Posts: n/a
Hi Robin,

Thanks alot for your suggestions. Actually, I had read the convergence problems in the forum and concluded that the oscillation type convergence plots are due to transient effects. (nothing worked out at that time, fine mesh, large-small time scale, changing boundary conditions, etc.) I was trying to find the steady state solution with taking time average field after transient run. But this looks not feasible for me. Then I decided to take a look at the mesh quality, and came across this problem.

What is interesting though, I am not using any control mech including any face spacings. I set all faces as "Volume Spacing" (you also mentioned about that). I am not using any space control, I am just specifying the default body spacing. Still I have this problem. I was even using some "virtual edge". (I have not used any "vitual face")

Anyway, I will try to solve this problem. If I find it, I will definetly let you guys know about it. Thanks alot for everything.

Mike

  Reply With Quote

Old   November 1, 2006, 02:48
Default Re: CFX-10 mesh- element volume ratio
  #6
Eric
Guest
 
Posts: n/a
Thank you for Mr. Robin and Mr.Mike.

I also use CFX-mesh for meshing. Maybe Element volume ratio less than 30 is OK.
  Reply With Quote

Old   November 1, 2006, 02:50
Default Re: CFX-10 mesh- element volume ratio
  #7
Dick
Guest
 
Posts: n/a
Dear Sir

Oscillation may be resulted from Physicial time?
  Reply With Quote

Old   November 1, 2006, 08:27
Default Re: CFX-10 mesh- element volume ratio
  #8
Mike
Guest
 
Posts: n/a
Hi Everybody,

Dick; thanks for the suggestion, however I had already tried changing physical time step. and it had not worked out either.

Eric; Thanks for your input. I am not sure about your comment though, since in the manual it is even talking about having element volume ratios less than 2 to have good enough results.

Any help would be appreciated.

Thanks alot guys,

Mike
  Reply With Quote

Old   November 1, 2006, 08:30
Default Re: CFX-10 mesh- element volume ratio
  #9
Eric
Guest
 
Posts: n/a
Dear Mike,

if possible, could you send the manual page to me. Element volume ratio<2 ?

Thank you

My email: qiuyifa@hotmail.com (MSN)
  Reply With Quote

Old   November 1, 2006, 08:42
Default Re: CFX-10 mesh- element volume ratio
  #10
Mike
Guest
 
Posts: n/a
Hi Eric, I don't have the electronic copy. It is in CFX-Post manual at page 148 under Mesh Visualisation Advice. Here is the statement;

"In many cases, the robustness of the CFX-Solver will not be adversly effected by high element volume ratios. However, you should be aware that accuracy will decrease as the element volume ratio increases. For optimal accuracy, you should try to keep the element volume ratio less than 2"

Mike
  Reply With Quote

Old   November 1, 2006, 08:44
Default Re: CFX-10 mesh- element volume ratio
  #11
Eric
Guest
 
Posts: n/a
Thank you Mike. I will consider this problem. Many thanks
  Reply With Quote

Old   October 8, 2012, 01:04
Default
  #12
New Member
 
mausam24's Avatar
 
Mausam Shresha
Join Date: Aug 2012
Posts: 13
Rep Power: 4
mausam24 is on a distinguished road
i have worked out with maximum element volume ratio but in terms the maximum edge length ratio seems to differ accordingly. so is there any solution to keep both in the limits
mausam24 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
[ICEM] Negative volume error in hybrid mesh siw ANSYS Meshing & Geometry 4 September 3, 2014 05:25
how to set periodic boundary conditions Ganesh FLUENT 13 January 22, 2014 05:11
snappyHexMesh won't work - zeros everywhere! sc298 OpenFOAM Native Meshers: snappyHexMesh and Others 2 March 27, 2011 21:11
Icemcfd 11: Loss of mesh from surface mesh option? Joe CFX 2 March 26, 2007 18:10
Gambit problems Althea FLUENT 21 February 6, 2001 08:05


All times are GMT -4. The time now is 11:49.