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

[ICEM] further refinment - Radial turbine

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

View Poll Results: Which mesher is your first choice for turbo-machinery
ICEM CFD 63 67.02%
TurboGrid 31 32.98%
Voters: 94. You may not vote on this poll

Like Tree1Likes
  • 1 Post By Far

Reply
 
LinkBack Thread Tools Display Modes
Old   January 1, 2012, 12:40
Default further refinment - Radial turbine
  #1
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,946
Blog Entries: 6
Rep Power: 39
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
Dear Frends

Right now I am working on generic turbocharger radial turbine. I am practicing on the ICEM meshing part (geometry part is discussed below). I am getting the quality of 0.25 and in Fluent maximum cell squish is .97, this is where I am confused.



Now My questions are:
1) I dont see any bad quality mesh and still I am getting the low quality mesh (though in very few cells may be 10 or 20 out of 0.4 million).

2) could any body suggest me the better topology as compared to turbo grid?

3) please guide me in creating topology so that I get the one-one periodicity.






Now lets discuss geometry part:
As I have already mentioned above that I am working on generic radial turbine, so geometry was made in ANSYS blade modeler V 13.0 with default parameters and exported as ICEM file. So I got all geometry entities such as sector cut of 36 degrees with periodic surfaces, shroud, hub, inlet, outlet and blade. Now my questions are:

1. If I had the IGES file of complete wheel then how one would get/create the all above geometric parts in ICEM CFD.
2. Assume that the blade has some gap from hub so one has also to consider to extend the blade and then make the Boolean operation on hub and blade. So how to extend the blade geometry so that it does not change the geometry of original blade and then how to cut it with hub.
3. a) How to make the hub and shroud as they are highly curved parts.
3. b) Is there any option in ICEM CFD like net surfaces in Gambit.
Far is offline   Reply With Quote

Old   January 1, 2012, 13:13
Default
  #2
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,946
Blog Entries: 6
Rep Power: 39
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
Geometry and blocking files are attached here

http://www.4shared.com/zip/YTVkYbfn/blocking_2.html
http://www.4shared.com/zip/ufIkaaLW/geometry.html
http://www.4shared.com/zip/bsG4JJqP/project.html
Far is offline   Reply With Quote

Old   January 2, 2012, 12:42
Default
  #3
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,946
Blog Entries: 6
Rep Power: 39
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
I am also facing this uneven meshing problem in scan planes. I have already used the mesh copy to all parallel edges and projected faces to part (shroud in this case).

Far is offline   Reply With Quote

Old   January 4, 2012, 12:29
Default
  #4
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,946
Blog Entries: 6
Rep Power: 39
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
I have also observed this problem at hub, although I have cross checked the associations many times. I haven't come across this sort of problem in axial machines and why this is happening in this case? I am sure that ICEM CFD takes into account the high curvature.




Far is offline   Reply With Quote

Old   January 5, 2012, 12:20
Default
  #5
Senior Member
 
PSYMN's Avatar
 
Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,662
Blog Entries: 1
Rep Power: 36
PSYMN has a spectacular aura aboutPSYMN has a spectacular aura about
It looks like your curves are not quite on your surfaces... Hexa works by projecting the curve projected nodes to the curves and the surface projected nodes to the surface. In your case, since these are not really aligned, you get a problem.

Zoom in and turn these geometry entities on for confirmation. You may find that you can simply improve your geometry or at least increase your triangulation tolerance (Settings => Model). If the curves were just badly placed in the imported geometry, You could also try removing the curves and recreating them from the actual geometry in ICEM CFD. There are other solutions, but you may just decide that fixing the geometry is too much hassle.

Fortunately, you are not the first to have this sort of geometry mismatch and we have blocking based solutions that don't require repair.

The first solution is to assume that the curves are correct. The pan is to "interpolate" between the curve and the surface projected nodes for some distance. It is like putting in a more gradual ramp. Just go into Settings => Meshing Options => Hexa Mixed and play with the "Projection Limit". Now that you know the name of the setting, you can look up the help on that.

The alternative solution assumes that the surfaces are good and the curves are bad. It uses a two step projection process so that your curve associated nodes will first project to the curve and then project to the nearest surface... This can be a little harder to control, but it is still easy to setup. Under "Blocking (tab) => Associate => Edge to Curve" you will see a check box for "Project to surface intersection". You will find that using this option colors the edges purple rather than green.
__________________
-----------------------------------------
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   January 5, 2012, 12:27
Default
  #6
Senior Member
 
PSYMN's Avatar
 
Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,662
Blog Entries: 1
Rep Power: 36
PSYMN has a spectacular aura aboutPSYMN has a spectacular aura about
I have no idea about your January 2nd post... I will think about it.
__________________
-----------------------------------------
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   January 5, 2012, 12:35
Default
  #7
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,946
Blog Entries: 6
Rep Power: 39
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
@Jan 2, 2012 post
I was able to solve this problem by splitting the blocks at further downstream position (out of screen) but don't know why this happened and why problem solved by another split.
Far is offline   Reply With Quote

Old   January 5, 2012, 12:43
Default
  #8
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,946
Blog Entries: 6
Rep Power: 39
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
Quote:
It looks like your curves are not quite on your surfaces
I would like to explain that how I got this geometry and therefore I also think there shouldn't be problem in geometry and domain (although you are right about the geometry problem, it is there).

1. Opened work bench and linked blade modeler to design modeler.
2. Geometry was designed in Ansys Blade modeler(with some arbitrary design inputs), then this geometry was imported into design modeler and domain (inlet, outlet, shroud, hub and periodic entities) was created automatically.
3.Then this was exported in para solid format (which I heard is the best option for geometry import/export).
Far is offline   Reply With Quote

Old   January 5, 2012, 21:31
Default
  #9
Senior Member
 
PSYMN's Avatar
 
Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,662
Blog Entries: 1
Rep Power: 36
PSYMN has a spectacular aura aboutPSYMN has a spectacular aura about
You could actually read the Design modeler geometry directly into ICEM CFD...

Maybe also check the triangulation tolerance in ICEM CFD... Go an order of magnitude smaller and see if it improves the situation.
__________________
-----------------------------------------
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   January 7, 2012, 02:05
Default
  #10
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,946
Blog Entries: 6
Rep Power: 39
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
Some more Pics @ Jan 02, 2012 post
After another split at downstream location (please refer to attached pic and for problem refer to jan 02 post), now I am able to solve this problem.



Any clue why this problem solved by this method?

Quote:
It looks like your curves are not quite on your surfaces... Hexa works by projecting the curve projected nodes to the curves and the surface projected nodes to the surface. In your case, since these are not really aligned, you get a problem.

Zoom in and turn these geometry entities on for confirmation. You may find that you can simply improve your geometry or at least increase your triangulation tolerance (Settings => Model). If the curves were just badly placed in the imported geometry, You could also try removing the curves and recreating them from the actual geometry in ICEM CFD. There are other solutions, but you may just decide that fixing the geometry is too much hassle.

Fortunately, you are not the first to have this sort of geometry mismatch and we have blocking based solutions that don't require repair.

The first solution is to assume that the curves are correct. The pan is to "interpolate" between the curve and the surface projected nodes for some distance. It is like putting in a more gradual ramp. Just go into Settings => Meshing Options => Hexa Mixed and play with the "Projection Limit". Now that you know the name of the setting, you can look up the help on that.

The alternative solution assumes that the surfaces are good and the curves are bad. It uses a two step projection process so that your curve associated nodes will first project to the curve and then project to the nearest surface... This can be a little harder to control, but it is still easy to setup. Under "Blocking (tab) => Associate => Edge to Curve" you will see a check box for "Project to surface intersection". You will find that using this option colors the edges purple rather than green.
They are really very advance options and I really appreciate this and (I guess) I would have not been able to learn these commands in very short time (may took months or years). It seems my problem is still not solved:

1. with geometry operation I get curves on the hub but then blade span wise edges are disconnected with hub edges (they should be making the closed loops) --------> Therefore this solution is not working.

2. With Hexa mixed when I gave some non zero values (0.1, .01, .001 and .0001), I observed that the edges are not following curves at all. For example instead of curved mesh at leading edge I am getting a straight line.

3."Blocking (tab) => Associate => Edge to Curve" The mesh is similar to the previous one i.e. without "Project to surface intersection" option.
Far is offline   Reply With Quote

Old   January 25, 2012, 13:00
Default Problem solved
  #11
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,946
Blog Entries: 6
Rep Power: 39
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
Dear PSYNM

This problem is now solved. Before discussing the valid and failed solutions, I want to recall the problem once again.

I am meshing generic turbocharger. Geometry made in bladegen and

1. exported bladegen file as ICEM geometry (.tin)
2. imported file to design-modeler/blade editor and exported as parasolid.
3. I also tried workbench reader and but got problems

I tried following to fix the problem (as suggested by PSYMN) :

1. triangulation tolerance: It did not solve the problem since geometry is highly distorted. In other words it was not the problem of tolerance at all.

2. Meshing Options => Hexa Mixed and play with the "Projection Limit" This did not solve the problem, again geometry is highly distorted.

3. Under "Blocking (tab) => Associate => Edge to Curve" you will see a check box for "Project to surface intersection This is again not working due to above reason.

Finally the solution to problem was found in ICEM 14. I did this

1. Linked the bladegen to blade editor and opened in geometry in blade-editor geometry (exactly same file as posted above).
2. Save the project and opened file in ICEM as workbench
3. opened same blocking posted previously and did not get any problematic elements near the hub-blade interface.

My conclusions from this exercise are:

1. The direct export from bladegen to ICEM is not good option, although it perfectly works for turbogrid. May be due to some problem in data compatibility.

2. There were bugs (may be) in ICEM 13 and older versions and these are now fixed in ICEM 14.

3. It is best to directly read the files into ICEM with the option of workbench reader and/or direct CAD readers (if files are made in CAD softwares)

4. It is better to check the different surfaces with the 2-D planner blocking to ensure that you would not end up with these problems. Therefore instead pushing ICEM, it is better option to try to get the perfect geometry.

I shall post pics and related material tomorrow.
aerospace84 likes this.
Far is offline   Reply With Quote

Old   March 19, 2014, 03:46
Default
  #12
New Member
 
chiranjivi
Join Date: Mar 2014
Posts: 5
Rep Power: 3
vega6 is on a distinguished road
how did you cut the sections into equal halves.
vega6 is offline   Reply With Quote

Old   March 19, 2014, 05:24
Default
  #13
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,946
Blog Entries: 6
Rep Power: 39
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
Quote:
Originally Posted by vega6 View Post
how did you cut the sections into equal halves.
which sections you are talking about?
Far is offline   Reply With Quote

Old   March 19, 2014, 06:10
Default
  #14
New Member
 
chiranjivi
Join Date: Mar 2014
Posts: 5
Rep Power: 3
vega6 is on a distinguished road
CAD sections. You have more than 10 blades in the model and you have done the meshing for just one section of it. How did you manage to cut the section into equal space to create a symmetric.

I was curious to know that technique cause the blade I have been trying to do is of a Francis turbine and I couldn't create the symmetric section.
vega6 is offline   Reply With Quote

Old   March 19, 2014, 09:12
Default
  #15
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,946
Blog Entries: 6
Rep Power: 39
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
Quote:
Originally Posted by vega6 View Post
CAD sections. You have more than 10 blades in the model and you have done the meshing for just one section of it. How did you manage to cut the section into equal space to create a symmetric.

I was curious to know that technique cause the blade I have been trying to do is of a Francis turbine and I couldn't create the symmetric section.
It was done automatically by bladegen software
Far 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
Direction of Rotation of Radial Turbine ghoshi1983 CFX 8 June 19, 2012 10:16
radial turbine blade simulation with dynamic mesh 6dof(fluent) mamyjooooon FLUENT 0 April 7, 2011 14:28
Non-nominal conditions in a radial turbine Petro FLUENT 0 December 29, 2010 09:04
Axial Thrust in a Radial Turbine Amit Roghs CFX 3 May 31, 2010 16:47
axial in, radial out turbine. flyingbird Main CFD Forum 0 August 3, 2009 14:39


All times are GMT -4. The time now is 09:04.