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

CFX Build 5 question...

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

Reply
 
LinkBack Thread Tools Display Modes
Old   May 25, 2001, 11:34
Default CFX Build 5 question...
  #1
cfd guy
Guest
 
Posts: n/a
Hi everyone...

I've been using CFX-4 for simulations, but recently we acquired the CFX-5 package here at the university for researches, so I'm a new user in this code.

And I would like to know from you about the meshing aspects. Since we want to solve unstructured meshes in CFX-5, we must know how to generate the grid files for it. In BUILD 4, it is suggested to create as many blocks as your geometry requires, for avoiding future problems in convergence, etc... But in the BUILD 5, almost all tutorials examples works with one simple block (a B-REP Solid), generated by several surfaces. Why that?
Is there some recommendation to avoid create multi-blocking, as I use to work with Build 4? I was trying to generate a multi-block grid in Build 5, but it failed when I tried to set up a interior wall (Thin surface) in the domain. I searched the manual and I found out how to create thin walls, but it seems that doesn't work with multi-blocks, since I must take care with domains and sub-domains fluids, which I suspect that I created them correctly. So, if anybody could supply me a hint, I'd be very thankful...
Regards!


cfd guy

  Reply With Quote

Old   May 25, 2001, 14:24
Default Re: CFX Build 5 question...
  #2
B Malone
Guest
 
Posts: n/a
One block is all there is. Your domain will be made up of one or more B-rep solids.

If your domain is simple try the default mesh parameters and work from there.
  Reply With Quote

Old   May 27, 2001, 01:42
Default Re: CFX Build 5 question...
  #3
Dan Williams
Guest
 
Posts: n/a
Ahh, the joy of unstructured meshing. Basically you can throw out everything you know about multiblock meshing. You only need to get a single b-rep solid of your computational domain in order to generate a grid.

The unstructured mesher simply meshes the surface representation (surface triangulation if you want to call it that) of your geometry, then uses that surface mesh to seed the creation of the entire volume mesh. No blocking is necessary, unless of course, as you mention you want to create thin surfaces.

Make sure you read the sections of the manual on topolgy and understand them before proceeding to make thin surface problems, which require creating sub-domains.

Dan.

  Reply With Quote

Old   May 28, 2001, 07:35
Default Re: CFX Build 5 question...
  #4
cfd guy
Guest
 
Posts: n/a
Hi Mr. Williams,

That's exactly the answer I was hoping for. As you said and I suspected, there's no need at all for multiblock grids, unless, as you also said, when it's necessary to work with thin surfaces.

In fact, in one of my problems, I must work with a thin surface, and as suggested, I'll assume to create an extra block for the thin surface i.e. a fluid sub-domain. But, before performing any operations, I'll take a look at topologies section manual.

Thanks for your help. Regards,

cfd guy
  Reply With Quote

Old   May 28, 2001, 18:20
Default Re: CFX Build 5 question...
  #5
Dan Williams
Guest
 
Posts: n/a
Hi,

Thin surfaces have to be created on a bounding surface of a fluid subdomain. The main problem when trying to use fluid subdomains is figuring out how to get a b-rep with more than one 3d solid. Once you figure out the plan though, it's not too bad.

Probably the main thing to keep in mind is that each solid region has to be bounded by "currently existing" surfaces. So, for example you can't simply create two XYZ solids and pick both of them to make a B-Rep. There are a couple of ways to do it right, but one way would be to create two XYZ solids, break one of them apart into surfaces, then delete the duplicate surface (where it would overlap with the first solid) and recreate a new solid out of the leftover surfaces plus the overlap surface on the first XYZ solid.

Sort of convoluted (and inconvenient), but that's the way it is. It gets more tricky, or tedious ;-), if your geometry is complicated.

Have fun.

Dan.

  Reply With Quote

Old   May 30, 2001, 07:39
Default Re: CFX Build 5 question...
  #6
Stuart Orme
Guest
 
Posts: n/a
Hi I agree with Dan's comments, unstructured meshing and single or multi brep solid generation requires a different approach. However your previous experience of structured meshing will still be useful. One example of this is when a surface can not be used to generate a Brep solid. The surface may have poor topology and may be too curved. Often such a surface needs to be broken down into more simple surfaces which can then be used to generate a Brep. Its at times like these when I usually find older techniques become useful. 2 things I would recomend:

1) Have a practice on a very simple model geometry first, ie flow round a cube sitting on the ground. This will allow you to check out any methodology that you are unsure about and also test the concept of generating a thin surface. Using Breps, multiple B'reps, generating cuouts, using standard Blue solids within a model etc.

2) When generating your Brep always use the verify/surface option before trying to create your Brep. This will check all your surfaces and highlight any problems there may be and will in the long run save you time.

Hope this helps, it can be a little frustrating to start with, but the general concept and mind set are much simplar and straight forward.

Stuart
  Reply With Quote

Old   June 19, 2001, 22:38
Default Re: CFX Build 5 question...
  #7
Robin Steed
Guest
 
Posts: n/a
With regards to the badly parameterized surfaces, there are facilities in Build to fix these. The Create|Surface|Composite function will take one or more surfaces and project new paramterization over the surface, basically by rotating the view and drawing horizontal and vertical lines across the screen. The only limitation is that the surface(s) must not have normals which are 180 degrees apart; the edges of a hemisphere, for example.

That little trick has gotten me out of many binds.
  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
launch cfx from command line question windhair CFX 3 May 19, 2011 07:16
[ICEM] Node Number vs. Node_ID & ICEM vs. CFX Araz ANSYS Meshing & Geometry 1 April 25, 2011 11:03
Question about the shock wave in CFX software nucharin Main CFD Forum 1 January 25, 2005 09:26
simple question about ICEM CFX sleepinglily CFX 0 October 27, 2004 13:15
Question about meshing / solution scheme of CFX Coriolius CFX 8 August 1, 2004 18:39


All times are GMT -4. The time now is 16:59.