CFD Online URL
[Sponsors]
Home > Forums > ANSYS Meshing & Geometry

[ICEM] How to separate two tri meshes with a line

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

Reply
 
LinkBack Thread Tools Display Modes
Old   October 4, 2013, 05:32
Default How to separate two tri meshes with a line
  #1
Senior Member
 
Francisco
Join Date: Mar 2012
Location: Spain
Posts: 270
Rep Power: 5
Bollonga is on a distinguished road
Hello everybody,

I have created a 2d tri mesh with a boundary layer using the advanced
BLayer2D option.

The issue is I had to mege two zones of tri meshes to get the prism layer properly (picture 1) and now I want to split them back. The meshes are conformal with the zones boundaries (picture 2).

I guess it is a rather simple question, but I'm not very skillful with unstructured meshes, so how can I separate both meshes by this contour?

Thanks a lot!
Attached Images
File Type: jpg Meshes001.jpg (92.3 KB, 22 views)
File Type: jpg Zone_zoom001.jpg (20.6 KB, 15 views)
Bollonga is offline   Reply With Quote

Old   October 7, 2013, 09:24
Default
  #2
Senior Member
 
PSYMN's Avatar
 
Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,660
Blog Entries: 1
Rep Power: 34
PSYMN has a spectacular aura aboutPSYMN has a spectacular aura about
Do you have surfaces (2D) between the curves? That really is best practice. If you have surfaces (or can add them now), and your mesh was generated with that curve (as it appears), you can use Edit Mesh > Repair Mesh > Associate Mesh (with geometry). This will put the triangles in the part of the surface they are sitting on.

If you want to use a curve to split a mesh that is not aligned with it, you could convert the mesh to facets, then use the segment surface by curve, then convert the facets back to mesh.
__________________
-----------------------------------------
Please help guide development at ANSYS by filling in these surveys

Public ANSYS ICEM CFD Users Survey

This second one is more general (Gambit, TGrid and ANSYS Meshing users welcome)...

CFD Online Users Survey
PSYMN is offline   Reply With Quote

Old   October 7, 2013, 17:43
Default
  #3
Senior Member
 
Francisco
Join Date: Mar 2012
Location: Spain
Posts: 270
Rep Power: 5
Bollonga is on a distinguished road
Yes, I have surfaces between the curves so I've followed your first approach. In the Repair mesh menu I've gone to associate mesh with geometry and I've selected the elements inside the surrounding rectangle, in some cases I had to pick them up one by one. Then I've applied, without having to select any geometry.
1) Does it automatically pick the appropiate surface?

I also have some basic questions about unstructured meshes.

2) How can I control the rate at which elements are growing in size?

3) How can I know the minimun resulting element size?

Thanks a lot Simon!
Bollonga is offline   Reply With Quote

Old   October 7, 2013, 18:15
Default
  #4
Senior Member
 
PSYMN's Avatar
 
Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,660
Blog Entries: 1
Rep Power: 34
PSYMN has a spectacular aura aboutPSYMN has a spectacular aura about
1) it draws a normal vector from the center of the shell element to the nearest surface and assigns it to the same part. You shouldn't have to pic carefully, just box select or select all and let it do its thing...

2) Element growth rate is controlled a few different ways. I assume you are using Patch Conforming, so there are two main options. There is a ratio you can set on the curves, there is a max size you can set on the surface (and then check the global setting to "Adapt mesh interior". These are called "soft" parameters (not strictly enforced, more like goals with quality as a driving criterion).

3) You can use Edit mesh (tab) > Display mesh quality and use a criterion like "Min Side" or "X size". You will get a histogram and the message window will tell you min/max and mean.

Here is what it gave for the little wing I am working on right now. In this case, it is just checking the min size of each element.

Min = 0, max = 11.8006, mean = 0.836419250598
40539 elements with the "Min side" diagnostic
Histogram of Min side values
11.21057 -> 11.8006 : 9 (0.022%)
10.62054 -> 11.21057 : 5 (0.012%)
10.03051 -> 10.62054 : 3 (0.007%)
9.44048 -> 10.03051 : 13 (0.032%)
8.85045 -> 9.44048 : 18 (0.044%)
8.26042 -> 8.85045 : 36 (0.089%)
7.67039 -> 8.26042 : 89 (0.220%)
7.08036 -> 7.67039 : 83 (0.205%)
6.49033 -> 7.08036 : 183 (0.451%)
5.9003 -> 6.49033 : 344 (0.849%)
5.31027 -> 5.9003 : 203 (0.501%)
4.72024 -> 5.31027 : 353 (0.871%)
4.13021 -> 4.72024 : 469 (1.157%)
3.54018 -> 4.13021 : 452 (1.115%)
2.95015 -> 3.54018 : 474 (1.169%)
2.36012 -> 2.95015 : 748 (1.845%)
1.77009 -> 2.36012 : 1329 (3.278%)
1.18006 -> 1.77009 : 3040 (7.499%)
0.59003 -> 1.18006 : 6178 (15.240%)
0.0 -> 0.59003 : 26510 (65.394%)
__________________
-----------------------------------------
Please help guide development at ANSYS by filling in these surveys

Public ANSYS ICEM CFD Users Survey

This second one is more general (Gambit, TGrid and ANSYS Meshing users welcome)...

CFD Online Users Survey
PSYMN is offline   Reply With Quote

Old   October 7, 2013, 18:39
Default
  #5
Senior Member
 
Francisco
Join Date: Mar 2012
Location: Spain
Posts: 270
Rep Power: 5
Bollonga is on a distinguished road
1) Ok

2) I am using patch independent. I don't know why patch dependent fails whenever I try to use it (see attached picture). What can be wrong in my patch conforming setup?
Would you recommend patch dependent or independent for simple cases like this?
What I use to control the element size is to specify the max size at surfaces, and to select the number of divisions in the curves. But this doesn't control the growth rate, and I find it to be quite fast.
You say I can control the growth rate selecting a ratio on the curves? What is its name? Is it in the setup curve mesh menu or the curve mesh?

3) Ok
Attached Images
File Type: jpg patch_dependent.jpg (53.2 KB, 12 views)
Bollonga is offline   Reply With Quote

Old   October 8, 2013, 01:02
Default
  #6
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,902
Blog Entries: 6
Rep Power: 37
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
I would try hybrid mesh...
Far is offline   Reply With Quote

Old   October 8, 2013, 05:44
Default
  #7
Senior Member
 
Francisco
Join Date: Mar 2012
Location: Spain
Posts: 270
Rep Power: 5
Bollonga is on a distinguished road
Quote:
Originally Posted by Far View Post
I would try hybrid mesh...
It is for a moving mesh, that's why I've chosen a tri mesh.
Can I use an hex mesh in a moving mesh zone?
Bollonga is offline   Reply With Quote

Old   October 8, 2013, 07:37
Default
  #8
Senior Member
 
Francisco
Join Date: Mar 2012
Location: Spain
Posts: 270
Rep Power: 5
Bollonga is on a distinguished road
Following your advice, Far, I'm trying with a hybrid mesh.
I've donde the tutorial Hybrid Tube which is 3D, but I'm finding some difficulties in my 2D case.

I've made a central rectangle for the tri mesh, and surrounding this one 8 rectangles for the hex blocks (see picture). The thing is that even if I choose just the central rectangle for the tri mesh everything get tri-meshed!
In the tutorial a material point is created to choose the zone to be meshed, should I do the same for 2D and create a mass point?

Which are your steps to create a 2D hybrid mesh?

Thanks!
Bollonga is offline   Reply With Quote

Old   October 8, 2013, 09:23
Default
  #9
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,902
Blog Entries: 6
Rep Power: 37
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
Take a look on this tutorial

https://dl.dropboxusercontent.com/u/..._2dairfoil.rar

For moving mesh, I always choose the tri mesh, where i know mesh is going to be deformed. However in limited area (boundary layer), I would use hexa and merge it with tetra.
Far is offline   Reply With Quote

Old   October 8, 2013, 13:33
Default
  #10
Senior Member
 
Francisco
Join Date: Mar 2012
Location: Spain
Posts: 270
Rep Power: 5
Bollonga is on a distinguished road
Quote:
Originally Posted by Far View Post
Far, how do you make meshing conforming in curves separating unstructured from structured? By chosing the same number of divisions?
I'm interested in a way to make this curves conformal once the tri and quad meshes are done.
In the tutorial Hybrid_Pipe this is made by selecting Edit mesh tab, then merge nodes and then merge meshes. However this procedure looks to be for volume meshes. How can I do that for 2d meshes?

As I posted previously, I'm not able to use the patch conforming method. Which are the steps to correctly accomplish it?

Thanks a lot.
Bollonga is offline   Reply With Quote

Old   October 8, 2013, 13:51
Default
  #11
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,902
Blog Entries: 6
Rep Power: 37
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
The procedure is as follows:

1. Set sizes on curves

2. generate hexa mesh

3. Set shell mesh parameters with "respect line elements"

4. Generate tri mesh (patch dependent)

5. Do the steps as described in the pdf and word files.
Far is offline   Reply With Quote

Old   October 9, 2013, 05:48
Default
  #12
Senior Member
 
Francisco
Join Date: Mar 2012
Location: Spain
Posts: 270
Rep Power: 5
Bollonga is on a distinguished road
Quote:
Originally Posted by Far View Post
The procedure is as follows:

1. Set sizes on curves

2. generate hexa mesh

3. Set shell mesh parameters with "respect line elements"

4. Generate tri mesh (patch dependent)

5. Do the steps as described in the pdf and word files.
This is not giving result for me.
Hexa mesh goes all right, then I select patch dependent mesh with respect to line elements, and specify max size on the surface to be tet-meshed. I've tried specifying curve divisions too and not doing so, both were the same. As usual patch dependent is a disaster (picture 1), I don't know why this is happening. There must be a simple step I am skipping.
I've also tried the patch independent approach, mesh is fine this time, but it doesn't match the hex mesh in the curves (picture 2). Why?
What can I do to get a hybrid mesh?
Attached Images
File Type: jpg patch_conforming.jpg (55.1 KB, 6 views)
File Type: jpg Non_comformal_corner.jpg (70.5 KB, 7 views)
Bollonga is offline   Reply With Quote

Old   October 9, 2013, 06:16
Default
  #13
Senior Member
 
Francisco
Join Date: Mar 2012
Location: Spain
Posts: 270
Rep Power: 5
Bollonga is on a distinguished road
Following carefully the tutorial and using its own files that's what happens when I execute the patch conformal mesh:
Attached Images
File Type: jpg tutorial_patch_conform.jpg (44.0 KB, 10 views)
Bollonga 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
is internalField(U) equivalent to zeroGradient? immortality OpenFOAM Running, Solving & CFD 7 March 29, 2013 03:27
channelFoam for a 3D pipe AlmostSurelyRob OpenFOAM 3 June 24, 2011 14:06
Installation OF1.5-dev ttdtud OpenFOAM Installation 46 May 5, 2009 03:32
errors Fahad Main CFD Forum 0 March 23, 2004 14:20
Problems of Duns Codes! Martin J Main CFD Forum 8 August 15, 2003 00:19


All times are GMT -4. The time now is 16:08.