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

Remeshing in CFX using workbench meshing.

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

Like Tree1Likes
  • 1 Post By adeban

Reply
 
LinkBack Thread Tools Display Modes
Old   September 13, 2011, 06:54
Default Remeshing in CFX using workbench meshing.
  #1
New Member
 
Klas Johansson
Join Date: Mar 2009
Posts: 16
Rep Power: 8
adeban is on a distinguished road
Cheers,

Some long time ago I posted a tutorial regarding remehsing in CFX using ICEM CFD as meshing tool. It resulted in a lot of questions which i appreciate.

We recently posted a new way of doing remeshing in CFX. This time it uses some scripting in workbench and launches the remesh in ANSYS Meshing.

This is very useful since the implementation towards ICEM today have some limitations.

The workbench remesh tutorial can be found on:

http://www.edr.no/blogg/ansys_blogge...nch_cfx_remesh


Klas Johansson, Ph.D.
Technical Consultant


EDR | Engineering Data Resources AB |
+46 31 759 5035 (tel) | +46 (0)708 87 92 72 (mobile)
mailto:klas.johansson@edr.se

EDR blog http://www.edr.se/blogg

Newsletter http://www.edr.se/nyhetsbrev
nuaawubin likes this.
adeban is offline   Reply With Quote

Old   September 13, 2011, 08:14
Default
  #2
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,931
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
Nice one - good video, I will have to try it out some time.

You like doing things the hard way don't you? I would have been lazy and just used a rotating frame of reference
ghorrocks is offline   Reply With Quote

Old   September 13, 2011, 10:05
Default
  #3
Senior Member
 
Join Date: Apr 2009
Posts: 516
Rep Power: 12
stumpy is on a distinguished road
I've seen something similar from ANSYS, but it's nice to have a tutorial that anybody can access. One key point is that this approach is parameter driven, so if you have a body that bends for example (instead of behaving like a rigid body whose motion is easily described by parameters) then you still need to use the ICEM approach.
stumpy is offline   Reply With Quote

Old   September 14, 2011, 03:24
Default
  #4
New Member
 
Klas Johansson
Join Date: Mar 2009
Posts: 16
Rep Power: 8
adeban is on a distinguished road
I like doing it the hard way. I was expecting that comment but it is just for demo purpose. Actually the hardest thing when creating an example is creating a case for the demo.

Correct me if im wrong but as the ICEM remesh approach is shipped with the ANSYS installation it only allows for translation in the three main coordinate directions. The ICEM implementation is also parameter driven since you do send values to describe the motion in between the programs.

I did some hacking of the script that handles the communicaiton some time ago to allow for rotational motion as well in ICEM but it was difficult to get it correct. The workbench approach allow for any motion out of the box as long as you can describe it with a parameter (e.g. translation, rotation, expansion ...).

If you have a thing that is bending in a controlled fashion think you would either run fluent that have remeshing in the solver (e.g. http://www.edr.no/blogg/ansys_blogge...n_ansys_fluent) or use keyframe swapping of the mesh. If you have something that is bending due to the flow (FSI) you are pretty stuck if the mesh-defomer cant handle the motion since we cant combine FSI and remshing in the current version. The main reason for this is that the mapping of the FSI load is today done at the start of a FSI simulation and if you do a remesh along the way the mapping is ruined.

Cheers
Klas
adeban is offline   Reply With Quote

Old   September 14, 2011, 09:33
Default
  #5
Senior Member
 
Join Date: Apr 2009
Posts: 516
Rep Power: 12
stumpy is on a distinguished road
I thought there were two approaches with ICEM remeshing. One that was parameter driven and one that brought in the deformed mesh and created a faceted geometry. The latter would be suitable to general motion. I could be wrong since I haven't tried either of those.
Yes, with FSI you are basically stuck since you can't do re-meshing (without a lot of pain). Your best bet here is to try out the latest 14.0 preview release and use the new FLUENT 2-way FSI feature which allows remeshing.
stumpy is offline   Reply With Quote

Old   September 15, 2011, 21:30
Default
  #6
Senior Member
 
Bruno
Join Date: Mar 2009
Location: Brazil
Posts: 236
Rep Power: 12
brunoc is on a distinguished road
Quote:
Originally Posted by adeban View Post
If you have something that is bending due to the flow (FSI) you are pretty stuck if the mesh-defomer cant handle the motion since we cant combine FSI and remshing in the current version. The main reason for this is that the mapping of the FSI load is today done at the start of a FSI simulation and if you do a remesh along the way the mapping is ruined.
Hi Klas,

Actually I'm pretty sure ANSYS has put remeshing for FSI cases as a beta feature for R13. I haven't tested it yet though, so I can't say if it works. If I have the time I'll try it and let you know.

Cheers
brunoc is offline   Reply With Quote

Old   September 16, 2011, 03:13
Default
  #7
New Member
 
Klas Johansson
Join Date: Mar 2009
Posts: 16
Rep Power: 8
adeban is on a distinguished road
Would be nice with that second approach in ICEM but i havent seen any documentation for such a solution but i havent looked at it since version 12.1. The same goes for that beta feature. Sounds interesting if its true.

Im gonna look at this and come back with whats possible.

cheers
adeban is offline   Reply With Quote

Old   September 16, 2011, 03:20
Default
  #8
New Member
 
Klas Johansson
Join Date: Mar 2009
Posts: 16
Rep Power: 8
adeban is on a distinguished road
Looks like it is not doable with a facetted surface out of the box at least.


As indicated previously, only translational mesh motion is automatically handled by the ICEM CFD Replay remeshing option. This is accomplished by applying the displacements of centroids of boundaries in the ANSYS CFX analysis definition to parts in the ANSYS ICEM CFD geometry.
adeban is offline   Reply With Quote

Old   September 16, 2011, 15:21
Default
  #9
Senior Member
 
Join Date: Apr 2009
Posts: 516
Rep Power: 12
stumpy is on a distinguished road
You're right, the ICEM re-meshing with a faceted geometry can't be done out of the box, it needs a bit of user scripting to work (according to the FSI training course material).
Re-meshing with FSI is definitely not a beta feature in R13. ANSYS simply says they don't support it, which I agree with given what's needed to get it to work.
stumpy is offline   Reply With Quote

Old   September 19, 2011, 10:51
Default
  #10
Senior Member
 
Michael P. Owen
Join Date: Mar 2009
Posts: 195
Rep Power: 8
michael_owen is on a distinguished road
Unfortunately, there seems to be some critical piece of information that is missing from the tutorial, because as it stands it does not actually work. Once the remeshing criteria is reached, the solver just remeshes over and over again, but the mesh is not actually replaced. I notice that the WB_Remesh.wbjn journal file is not included in the tutorial, so perhaps the one I created is somehow in error.

I've emailed the author and hopefully will get it cleared up soon.
michael_owen is offline   Reply With Quote

Old   September 19, 2011, 18:41
Default
  #11
Senior Member
 
Bruno
Join Date: Mar 2009
Location: Brazil
Posts: 236
Rep Power: 12
brunoc is on a distinguished road
Quote:
Originally Posted by stumpy View Post
Re-meshing with FSI is definitely not a beta feature in R13. ANSYS simply says they don't support it, which I agree with given what's needed to get it to work.
You're right, I checked it and it apparently uses no special feature other then heavy manual work and scripting, plus setting almost everything (from the structural side) directly on ANSYS Classic.

I'm a CFD guy. Even though I have to use it from time to time, ANSYS Classic scares the hell out of me
brunoc is offline   Reply With Quote

Old   October 11, 2011, 13:43
Default
  #12
Member
 
anonymous
Join Date: Jun 2011
Posts: 55
Rep Power: 6
Doginal is on a distinguished road
Hello

I was trying to work through the tutorial but i do not know how to create the .wbjn file. I believe that is the "script" to actually create the mesh. Are there any tutorials for creating that or just any idea on how to do that.

The other question i have just deals with remeshing in V12.1 and V13. When i read up on V13 they talk about being able to stop, remesh and continue very easily and well. I assume the same goes for this tutorial. Is there a big difference in V13's ability to interpolate results when a new mesh is applied verses V12.1

Thank You,

DM
Doginal is offline   Reply With Quote

Old   July 24, 2012, 16:40
Default Wbjn. File
  #13
New Member
 
Join Date: Jun 2012
Posts: 2
Rep Power: 0
Dr-Nukem is on a distinguished road
Hi

I am currently trying to simulate the erosion rate on a mixers rotor blades. I find your remesh method to be the perfect solution for my problem. Sadly I had no luck getting the .Wbjn File to work.
The solver usually starts its calculations till it gets to remesh, while doing so, the design modeller and the mesher open up for a brief moment. Following that the solver continues its calculations. Everything seems fine except that the results show no remeshing whatsoever.

I guess I can ask a question right off the bat: In order to create the correct .Wbjn File, when do I start recording and when do I quit recording?.

What I did so far, is start recording as soon as I started the program and stopped as soon as my mesh was green lighted by WB. I gotta also add that when I tried running the .Wbjn File to see if it replays my commands correctly, it created the geometry and the mesh, except that the mesh had much larger elements than the ones I chose.

I would appreciate every bit of help I can get
Dr-Nukem is offline   Reply With Quote

Old   October 24, 2012, 15:43
Default Remeshing in Workbench
  #14
New Member
 
Anup
Join Date: Feb 2012
Posts: 5
Rep Power: 5
anup is on a distinguished road
The workbench remesh tutorial can be found on:

http://www.edr.no/blogg/ansys_blogge...nch_cfx_remesh


Hi Klas,
I am trying to remesh both way either by ICEM CFD or by workbench.During using ICEM I opened the replay ontrol window before importing the geometry from workbench and then I did the mesh and save as unstructured mesh usable in cfx and then save the replay file and close evrything. But when I used .tin and .rpl file in the cfx, the simulation ended with giving error(attached) just before starting the remesh. My remeshing condition was min orthogonality angle. I followed your(www.edr.no/bloog...) droping box tutorial using ICEM available in You Tube. My one is very similar, 'pipe penetration'. Can you/anyone please tell me what is the main reason. When should I open or close the replay window? Should anything more to do in replay control? or anything else?

On the other hand for using workbench I stuck in very earlier. How can I get the attached window(wndw 1) for input the parameter? I am using Ansys 13(academic). I can open 'mesh dialogue' and 'prameter set' seperately(as attached 'wndw 2') but how can I transfer/attached the parameter to the mesh? Please help me.

Thanks in advance!
Attached Images
File Type: png wndw 1.PNG (7.6 KB, 65 views)
File Type: png wndw 2.PNG (11.9 KB, 59 views)
Attached Files
File Type: docx Error in Replay File.docx (63.6 KB, 57 views)
anup is offline   Reply With Quote

Old   February 1, 2013, 12:10
Default
  #15
New Member
 
Ramin Mirzazadeh
Join Date: Aug 2012
Posts: 16
Rep Power: 5
raminmir is on a distinguished road
Quote:
Originally Posted by anup View Post
The workbench remesh tutorial can be found on:

http://www.edr.no/blogg/ansys_blogge...nch_cfx_remesh


Hi Klas,
I am trying to remesh both way either by ICEM CFD or by workbench.During using ICEM I opened the replay ontrol window before importing the geometry from workbench and then I did the mesh and save as unstructured mesh usable in cfx and then save the replay file and close evrything. But when I used .tin and .rpl file in the cfx, the simulation ended with giving error(attached) just before starting the remesh. My remeshing condition was min orthogonality angle. I followed your(www.edr.no/bloog...) droping box tutorial using ICEM available in You Tube. My one is very similar, 'pipe penetration'. Can you/anyone please tell me what is the main reason. When should I open or close the replay window? Should anything more to do in replay control? or anything else?

On the other hand for using workbench I stuck in very earlier. How can I get the attached window(wndw 1) for input the parameter? I am using Ansys 13(academic). I can open 'mesh dialogue' and 'prameter set' seperately(as attached 'wndw 2') but how can I transfer/attached the parameter to the mesh? Please help me.

Thanks in advance!


for creating the parameter, open your geometry in Design Modeler and select your sketch, on the Details View window check the box on the left hand of desired Dimension.
you have to start recording your replay file after opening your geometry. you need to set up your meshing settings and create the mesh and then save your .rpl file
raminmir is offline   Reply With Quote

Old   March 11, 2013, 04:11
Default
  #16
New Member
 
Seran Reschim
Join Date: Jun 2012
Posts: 7
Rep Power: 5
ch_ohm is on a distinguished road
I have tried http://www.edr.no/blogg/ansys_blogge...nch_cfx_remesh
but I can not complete it. If someone can help me about inform more detail about that tutorial, please help me.
Thank you.
ch_ohm is offline   Reply With Quote

Old   August 20, 2013, 03:04
Default
  #17
New Member
 
Abdullah Al Faruk
Join Date: Apr 2012
Posts: 5
Rep Power: 5
alfaruk is on a distinguished road
Quote:
Originally Posted by raminmir View Post
for creating the parameter, open your geometry in Design Modeler and select your sketch, on the Details View window check the box on the left hand of desired Dimension.
you have to start recording your replay file after opening your geometry. you need to set up your meshing settings and create the mesh and then save your .rpl file
In the tutorial of discussion, the rotational angle (Rotangle) was sat as parameter, but I failed to understand which dimension is the Rotangle in the geometry of the tutorial?
alfaruk is offline   Reply With Quote

Old   August 21, 2013, 08:48
Default
  #18
New Member
 
Abdullah Al Faruk
Join Date: Apr 2012
Posts: 5
Rep Power: 5
alfaruk is on a distinguished road
Quote:
Originally Posted by stumpy View Post
I've seen something similar from ANSYS, but it's nice to have a tutorial that anybody can access. One key point is that this approach is parameter driven, so if you have a body that bends for example (instead of behaving like a rigid body whose motion is easily described by parameters) then you still need to use the ICEM approach.
How do I give rotational motion of rigid body in Design Modeller? I didn't find rotational angle in Dimensioning. Please help.
alfaruk is offline   Reply With Quote

Old   August 25, 2013, 00:02
Default
  #19
New Member
 
Join Date: May 2011
Posts: 22
Rep Power: 6
Spring.s is on a distinguished road
Quote:
Originally Posted by adeban View Post
Looks like it is not doable with a facetted surface out of the box at least.


As indicated previously, only translational mesh motion is automatically handled by the ICEM CFD Replay remeshing option. This is accomplished by applying the displacements of centroids of boundaries in the ANSYS CFX analysis definition to parts in the ANSYS ICEM CFD geometry.

Hi adeban
So, can you prepare Script for rotational mesh motion with ICEM?
I can't find it yet! Can you help me?

Cheers
Spring.s is offline   Reply With Quote

Old   May 16, 2014, 07:29
Default
  #20
New Member
 
quan wen
Join Date: Jun 2013
Posts: 3
Rep Power: 4
killmask1945 is on a distinguished road
Hi Adeban,
Thanks for the share. I am currently trying to simulate the opening and closing of cantilever valve. Therefore, few gap (which local at the over-lip region between the cantilever and the base of the valve) will be variable from 0 (sealed) to some value (open). Is there a way to using the re-meshing function at that?
If yes, how can i do it?
killmask1945 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
[ANSYS Meshing] meshing quality for CFX icemaniac178 ANSYS Meshing & Geometry 0 April 23, 2011 20:21
CFX meshing _help needed_Two way FSI problem kmgraju CFX 0 March 19, 2011 23:11
CFX 12.0 remeshing error songxguan CFX 1 November 26, 2009 07:14
CFX meshing with Workbench anna CFX 1 December 19, 2006 15:35
cfx, meshing + examples mark Main CFD Forum 1 December 22, 2000 00:10


All times are GMT -4. The time now is 21:45.