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

[ICEM] 3D turbine blade modeling

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

Like Tree1Likes

Reply
 
LinkBack Thread Tools Display Modes
Old   March 11, 2010, 20:38
Unhappy Turbine geometry
  #21
New Member
 
Zaqie
Join Date: Jul 2009
Posts: 22
Rep Power: 9
Zaqie is on a distinguished road
I know I have been persistent. I am not really getting it right.

Can you give me a method to block the blade. I am having trouble at the hub area, the problem as mentioned below

I collapsed the blade section. Since collapsing of blade section was leading to collapse of section underneath it effecting the hub area, i split the blade block to two, one a larger one above and a smaller one below. Then I used index control for the upper larger section for collapsing for the blade. Associated vertices and curves to edges of the blade. Since the splitting of upper block created a additional block in the hub area , i merged the two blocks inside the hub. Then I tried creating the ogrid using the two blocks, i.e one in the blade and and the other at the hub. But I got an error message on the lines of "Ogrid could not be created".

Please help. If possible please give me tips on blocking the domain completely. I am really stuck.

Zaqie
Attached Images
File Type: jpg turbine1.jpg (59.8 KB, 299 views)
Zaqie is offline   Reply With Quote

Old   March 11, 2010, 22:40
Default Ok sure Zaqie, let’s go…
  #22
Retired from CFD Online
 
PSYMN's Avatar
 
Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,660
Blog Entries: 1
Rep Power: 38
PSYMN has a spectacular aura aboutPSYMN has a spectacular aura about
Ok sure Zaqie, let’s go…

First things first… How to make hexa blocking periodic.

Go to “mesh tab => Global Mesh Setup => Set up Periodicity”


Zaqie_01.gif



We will get back to making the blocking periodic later…

Next we initialize a new blocking. Since I want the blocking to follow the walls and to focus more mesh in the core of this wedge shape, I will want a quarter ogrid right away… Use the ogrid tool, face the flat sides (2 eventual periodic sides and the inlet and outlet.) and apply. It will look something like this.

Zaqie_02.jpg



Now it is time to make things periodic. Go to “Blocking Tab => Edit Block => Periodic Vertices”. Choose create and then select pairs of verts. On older versions it mattered that you stayed consistent with your ordering… I don’t think it matters any more, but I still do it out of habbit. Pick a vetex on one side and then the vert that will be its periodic twin. Because you actually have the axis as part of your model, you will just click those corner verts twice. If we do this now while the blocking is simple, you should only have to take care of six pairs… If you right click in the model tree, you can turn on the display of periodic verts and periodic faces…

I took it one more step and associated to points before taking this pic…


Zaqie_03.gif


Note, any further splits of a periodic face will already be periodic, so it is usually easier to do this now than later.

Similarly, I would finish up and associate all the edges with curves as needed (better now while I have fewer edges and later splits will already be associated).

Next I want to get the rest of my topology right before I complicate things with further splits. On the inlet or the outlet, I drag the verts for the hgrid core of the Ogrid, so they are smaller than the hub. (as shown).


Zaqie_04.jpg



My next step will be to align along the flow direction so that both ends are the same. (select the axis as the edge direction and the reference verts as one of the ones you moved toward the axis…

Zaqie_05.jpg

To be continued…
PSYMN is offline   Reply With Quote

Old   March 11, 2010, 22:44
Default Zaqie Continued...
  #23
Retired from CFD Online
 
PSYMN's Avatar
 
Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,660
Blog Entries: 1
Rep Power: 38
PSYMN has a spectacular aura aboutPSYMN has a spectacular aura about
Ok, so now we need to split the Ogrid edge twice… Once for the hub and once for the tip…
Zaqie_06.jpg


Next I zoom in and make 2 splits across the axis, one for upstream of the hub, one for downstream. Then associate to the hub edges and delete the blocks in the hub its self…
Zaqie_07.jpg


Now two more splits. One for upstream of the blade and one for downstream of the blade.
Zaqie_08.jpg



Then three more splits and we will be done with splitting ;^). The first goes just ahead of the airfoil… then a second right behind the airfoil…


Lets associate edges to keep things clean, but only loosely fit to the trailing edge of the blade… (if things are getting cluttered for you now, use the index control to limit what you see down to just what you need to work on, turn of surfaces and other clutter. You only need to look at a few edges and the blade right now.)
Zaqie_09.gif



And one more thing… Don’t just leave things associated… Move things into place so that future splits, ogrids, etc. work out better (we won’t be making any more, but it is still good practice).
Zaqie_12.gif



You can also delete the two blocks inside the blade now.

To be continued…
PSYMN is offline   Reply With Quote

Old   March 11, 2010, 23:36
Default Zaqie Continued...
  #24
Retired from CFD Online
 
PSYMN's Avatar
 
Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,660
Blog Entries: 1
Rep Power: 38
PSYMN has a spectacular aura aboutPSYMN has a spectacular aura about
The last split is only necessary because our model is periodic. We want to collapse the trailing edge block and normally we would collapse all the way to the wall to avoid wedges, but we can’t have fewer nodes on one side than the other, so we must only collapse a section within the volume. The last split goes half way between the split behind the trailing edge and the periodic boundary… In my case, I limited the index to just between the hub ends… But you could have done it from inlet to outlet…

Zaqie_13.jpg



Ok, now is the collapse block bit… We want to reduce the index control so you just see what you need to see. Namely, that middle layer that passes thru the blade and these blocks behind the blade… We need to see these blocks all the way out to the model extents because we need to make sure to collapse it out thru the top or we will get 7 noded blocks…

GO to “Blocking tab => Merge Vertices => Collapse Blocks”. It asks for the collapse edge… Any of these “i” direction edges will do, but I usually pick the one we are trying to get rid of right down at the root of the trailing edge…


Zaqie_14.jpg



Then select the blocks out to the far field...


Zaqie_15.jpg


This will collapse that trailing block… then go in and clean things up. Start by associating the trailing edge and trailing edge verts…


Oops, I forgot, one more split to capture the sudden change in the blade shape. Not necessary, but will give a cleaner blade. It should look something like this now…


Zaqie_16.jpg


Next I would play with it for a while… Work with some of the move vertex options to align vertices in a line, set location, etc. to generally clean it up… Again, I find adjusting the index control to only deal with one Ogrid layer at a time is the easiest way to not get confused by the edges… In this image, you can see that layer 03=2 looks good now… (I just used “align vertices in a line”).


Zaqie_17.jpg

I would repeat this for the other layers and then between layers by stepping thru i, j or k planes.

To be continued…
PSYMN is offline   Reply With Quote

Old   March 11, 2010, 23:40
Default Zaqie... The end.
  #25
Retired from CFD Online
 
PSYMN's Avatar
 
Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,660
Blog Entries: 1
Rep Power: 38
PSYMN has a spectacular aura aboutPSYMN has a spectacular aura about
Then I add some edge params (I just did a rough job here. You should take your time to make sure you have good smooth transitions, etc…


These pics are rough, but here is the scan plane around the blade...
Zaqie_18.jpg
Then here is a zoom in on the hub...
Zaqie_19.jpg
Then here is a zoom out, you can see the mesh down at the outlet also...

Zaqie_20.jpg

Of course, this all assumes your solver doesn’t mind some prisms (most unstructured solvers don't).

Also, I guess I could have wrapped the blade with a CGRID before the collapse. You can see how to do that earlier in this post when I was working on Shane Stan’s model. It would have given us a much more controllable boundary layer around the airfoil.

Hope this helps…
PSYMN is offline   Reply With Quote

Old   March 15, 2010, 16:53
Default Error while import to Fluent
  #26
New Member
 
Zaqie
Join Date: Jul 2009
Posts: 22
Rep Power: 9
Zaqie is on a distinguished road
Simon, thanks for the help.

I have meshed the geometry, assigned the boundary conditions and created the mesh file. But I get a error in fluent as below

************************************************** ******

Warning: Inappropriate zone type (periodic) for one-sided face zone 17.
Changing to wall.
Warning: Inappropriate zone type (periodic) for one-sided face zone 18.
Changing to wall.
Cell Centroid is xc -17.950718 yc 2493.581787 zc 1681.828125
WARNING: no face with given nodes. Thread 13, cell 201934
Clearing partially read grid.

Error: Build Grid: Aborted due to critical error.

************************************************** ******

I had encountered similar problem earlier when I had done tetra/prism mesh. Then, I had made the two periodic face in one part. The problem was rectified when they were separated into two parts and meshed separately

Now when I do this in a similar manner I get this issue. Any idea why this is happening.

Regards

Zaqie
Zaqie is offline   Reply With Quote

Old   March 15, 2010, 20:41
Default Periodicty check...?
  #27
Retired from CFD Online
 
PSYMN's Avatar
 
Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,660
Blog Entries: 1
Rep Power: 38
PSYMN has a spectacular aura aboutPSYMN has a spectacular aura about
Did you do the periodicity check in ICEM CFD? It is one of the options under "check mesh" that is off by default...

Perhaps your line elements or corner nodes are not in the periodic parts?

Simon
PSYMN is offline   Reply With Quote

Old   March 16, 2010, 17:19
Default
  #28
New Member
 
Zaqie
Join Date: Jul 2009
Posts: 22
Rep Power: 9
Zaqie is on a distinguished road
Hi

One quick doubt.

I dont understand why you have selected Spacing2 as 50.4044. I find such values in all the edges. I assume you will be putting some whole numbers. But these numbers are intriguing me.

And I understand what spacing1, spacing2 are. But not able to comprehend the spacing values. Is there some thing that I am missing.

Regards

Zaqie
Attached Images
File Type: jpg edge parameter.jpg (95.6 KB, 92 views)
Zaqie is offline   Reply With Quote

Old   March 17, 2010, 10:17
Default Relative Vs. Absolute.
  #29
Retired from CFD Online
 
PSYMN's Avatar
 
Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,660
Blog Entries: 1
Rep Power: 38
PSYMN has a spectacular aura aboutPSYMN has a spectacular aura about
Zaqie also asked me another more general question (privately) about how I set these edge distributions. The answer is that in this case, it was just arbitrary.

As for this specific case of the spacing 2 set to 50.4044, I don’t think I set anything, it just picked something. But if you look closely at your edge parameters DEZ (Data Entry Zone) you will see an option to set the sizing “relative” or “absolute”. If I set it “Absolute” and then copy to parallel edges, it will copy each spacing2 exactly as it is. So if I set it to 40, it will be 40 everywhere. It also must keep the number of nodes constant, so it is the ratio that will need to adjust if the edge length changes. Conversely, if I set it to “relative”, then the ratio will be held constant, the number of nodes will be held constant, but the end spacing will be adjusted relative to the edge length. So, if I had set spacing2 to 40 on the side edge, with relative sizing, and the middle edge was 26% longer, then the Spacing2 would be scaled up to 50.4044… Make sense? I usually use “Relative” unless I have been told that the analyst is really picky about Y+ and wants the initial height held very constant.

As for the more general question about how do you set these edge parameters (other than arbitrary)… Many users will calculate the Y+ to know the initial height off the wall and then it is common to use a growth ratio of 1.2. But then some people vary it as necessary. For instance, if you have too many elements, then maybe reduce your node count and increase your growth ratio to 1.5. Many ICEM CFD users do the same sort of models every time (always blades or always car mirrors or always drone aircraft), so they have already solved a few and may even have done a mesh refinement study to know if their mesh parameters are sufficient to resolve their physics. They may develop habits like always setting the initial height to 1e-6 and ratio to 1.2… Then they just increase the number of nodes on the edges until this is satisfied and they have a relatively smooth mesh. Actually, some have rules about how many nodes on each edge in the model, this way they remove one variable (mesh density) from result comparisons. This becomes a very natural thing to do if they have the same topology and can actually copy the blocking file from one model and fit it to the next without adjusting any of the distributions (no need to start over with the blocking).
PSYMN is offline   Reply With Quote

Old   March 18, 2010, 16:02
Default periodicity
  #30
New Member
 
Zaqie
Join Date: Jul 2009
Posts: 22
Rep Power: 9
Zaqie is on a distinguished road
Simon,

Thanks for the reply.

I am still having problems with the periodicity. I checked the mesh for periodicity and got errors like as mentioned below

shell 614980 has node 361165 which has no twin

I had put all the curves and points and nodes in different parts (curves and points respectively). The first time I got this error I moved them to points and curves to corresponding parts(like periodic_1 and periodic_2).
For the curves and points which is at the junction of periodic face 1 and periodic face 2i created duplicate curves and nodes so that they can be put a peice in periodic_1 and periodic_2.(I hope you understand what I am saying)

Even this doesnt seem to help. Any idea why this happening.

regards

zaqie reza
Zaqie is offline   Reply With Quote

Old   March 20, 2010, 20:56
Default Not fully setup...
  #31
Retired from CFD Online
 
PSYMN's Avatar
 
Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,660
Blog Entries: 1
Rep Power: 38
PSYMN has a spectacular aura aboutPSYMN has a spectacular aura about
Hey Zaqie,

I took a quick look at this yesterday morning, but only had a minute to load the blocking and take a couple pics. I didn't have time to finish fixing it or test if it work. I usually like to test before I respond, but i am having a busy weekend.

Here is what I know...

First thing I checked was turning on verts with periodic and faces with periodic faces. I could see right away that the blocking was not completely periodic.

Zaqie_30_NotQuitePeriodic2.jpg

I needed to make a few more pairs of verts periodic and that fixed the problem. When you see the red faces across both periodic sides, then convert to unstructured and test again...

As I said, I didn't have time to finish testing or see if there were other problems, but this should get you going again.

Simon
PSYMN is offline   Reply With Quote

Old   March 23, 2010, 11:47
Default Periodic turbine blade passage modelling
  #32
New Member
 
Andy Good
Join Date: Jul 2009
Posts: 11
Rep Power: 9
Andy QUB is on a distinguished road
Dear PSYMN,

I've used a slightly differnet method to the one you suggested to Shane. I haven't used O-grids or C-grids as my domain is a 90 degree wedge of a turbine blade. Instead I've split the block to create two blocks for the airfoil and then collapsed blocks at the leading and trailing edges (leaving a diamond shape to associate to the blade). I have managed to capture the geometry but my mesh has poor quality, as far as I can see for 2 reasons.

1: The twist is quite high towards the hub and this is causing large deformations in the blocking at the root. (see hub surface mesh)

2: The requirement for periodic vertices means I can't move the vertices individually for the leading edge and trailing edge.

Any advice you can offer would be wonderful,

Many thanks,
Andy
Andy QUB is offline   Reply With Quote

Old   March 23, 2010, 14:35
Default Cell Skewness
  #33
New Member
 
Zaqie
Join Date: Jul 2009
Posts: 22
Rep Power: 9
Zaqie is on a distinguished road
Hi Simon,

I have fixed the periodicity problem. Thanks.

And I imported the mesh to Fluent. But there is a new problem.

When I check for the mesh quality I get high Skewness

Maximum cell squish = 9.94699e-001
Warning: maximum cell squish exceeds 0.99.
Maximum cell skewness = 9.97481e-001
Warning: maximum cell skewness exceeds 0.98.
Maximum aspect ratio = 2.00392e+003


My aim is to restrict the skewness to below 0.7. Any tips on achieving this. Will smooth transitions of spacing help in this?.

Regards

Zaqie
Zaqie is offline   Reply With Quote

Old   March 23, 2010, 20:19
Default Move a vertex.
  #34
Retired from CFD Online
 
PSYMN's Avatar
 
Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,660
Blog Entries: 1
Rep Power: 38
PSYMN has a spectacular aura aboutPSYMN has a spectacular aura about
Zaqie,

Look at the mesh quality in ICEM CFD. You can use the TGrid Skew Metric if you have 12.0 or newer. Actually display the Bad elements on the screen so you can get a good feel for why the shape is bad. Some times I run a scan plane thru the bad elements to get a better understanding.

Chances are you will see that it has to do with a badly placed vertex. Think about moving a vertex a bit to reduce the skew, but keep in mind that moving it too far will create other skew. It should be possible to get very high quality for your model, but you don't really need 0.7. You can run just fine on 0.95.

Simon
PSYMN is offline   Reply With Quote

Old   March 23, 2010, 20:36
Default Highly curved blades?
  #35
Retired from CFD Online
 
PSYMN's Avatar
 
Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,660
Blog Entries: 1
Rep Power: 38
PSYMN has a spectacular aura aboutPSYMN has a spectacular aura about
Hey Andy,

This thread just keeps on growing... Maybe its time to create a new one if any one else has any new questions...

If you meant to include an image, you forgot to. Please try again.

So you are viewing the space between the hub and the shroud as a H-Grid (bent to fit) and then you split for the blade and collapsed it... No problem, sounds good.

But then it sounds like you were having trouble due to a lot of curvature in the blade... Yes, there are some interesting strategies for blocking high lift blades. I am pretty sure I have already posted this somewhere else, but basically the trick is to use a quarter ogrid so you can shift the periodicity one index and relax the requirement.

ShiftedPeriodic.jpg

Another trick (if your model does not include a tip gap) is to model the channel between blades instead of around the blade its self. This greatly reduces the periodicity requirements to just the upstream and down stream regions and allows for a lot of flexibility in blocking the blades and the channel.
PSYMN is offline   Reply With Quote

Old   March 24, 2010, 20:47
Default Skewness
  #36
New Member
 
Zaqie
Join Date: Jul 2009
Posts: 22
Rep Power: 9
Zaqie is on a distinguished road
Simon,

Perhaps last post in this thread. Dragged it for too long I guess.

Please see the attached pics. Skew elements are along the collapsed edge. I guess moving the vertices at that point wont help. The squeness seems to be because of the narrowing edges at the vertex. I tries moving the two vertex adjacent to the collasped vertex at the blade end(it has limited area to move along the blade surface), so that I can get wider angle at the collapsed vertex, but to no avail. The number of skewed elements remained the same.

Also, tried reducing the spacing at that location (from 8 to 6 to 5). Number of skewed elements reduced by about a score(I have about 320 elements above 0.95)

Any suggestions

Regards

Zaqie
Attached Images
File Type: jpg skew elements 1.jpg (59.3 KB, 73 views)
File Type: jpg skew elements 2.jpg (70.4 KB, 64 views)
File Type: jpg skew elements 3.jpg (72.4 KB, 78 views)
Zaqie is offline   Reply With Quote

Old   March 24, 2010, 22:12
Default Skew
  #37
Retired from CFD Online
 
PSYMN's Avatar
 
Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,660
Blog Entries: 1
Rep Power: 38
PSYMN has a spectacular aura aboutPSYMN has a spectacular aura about
Don't forget that skew is just a number...

And it doesn't apply very well to wedges. If you can't open up that angle any more, you could add a few more nodes across... It wouldn't get rid of the tight angle but it may help your mesh by reducing the high aspect ratio... (you can make up for it by increasing the element size as you approach the far field)

But at some point, I would just say "enough is enough" and run it. If it doesn't diverge (probably won't just because of 300 wedges), then just keep an eye out in those areas during post processing...

Simon
PSYMN is offline   Reply With Quote

Old   March 25, 2010, 10:01
Default
  #38
New Member
 
Andy Good
Join Date: Jul 2009
Posts: 11
Rep Power: 9
Andy QUB is on a distinguished road
Dear Simon,

Thanks again for all the help. I think the description of my turbine may have been a little confusing (hopefully now things will be clearer from the files i sent). Its a tidal turbine with no shroud very similar to Zaqie's, the only difference being I'm meshing a 90 degree wedge of smaller radius, which I then plan to copy for a full rotor mesh to place within a large stator to determine the wake.

I've gone through the method you laid out for Zaqie and it seems more logical than my previous method. I then tried to clean up some of the quality issues but made a bit of a mess! So I started again and have deliberately not moved the vertices too far so that (If you are willing!) you can have a look and see if this method will work for my geometry. There's obviously some distortion in the premesh around the rotor 'Top-Rotor outlet' surface' which I haven't been able to figure out this time but hopefully what I'm attempting is clear. I'm still a little concerned at the level of twist I have in the tight region close to the hub.

Please let me know if you need any other files or explanation.

Many thanks,
Andy
Andy QUB is offline   Reply With Quote

Old   March 25, 2010, 15:42
Default Took a look...
  #39
Retired from CFD Online
 
PSYMN's Avatar
 
Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,660
Blog Entries: 1
Rep Power: 38
PSYMN has a spectacular aura aboutPSYMN has a spectacular aura about
Hey Andy, I won't have time to try this out, but I gave it a few minutes of thought and may have a blocking solution for you...

Basically, the problem is that your blade is so close to the periodic boundary and the leading and trailing edges are so far shifted that it is very difficult to get good quality... The solution, as I hinted in an earlier post, is to shift the periodicity. I know it is sometimes hard to apply these concepts, so I will include an image for you particular model...

ShiftedPeriodic2.jpg

Basically, just look at the section between 2 and 6. Note that the edge is periodic and we did it by adding 2 quarter ogrids on the bottom right and one on the top left... (we usually need these in equal supply, but because we are collapsing the trailing edge, we only needed on on the opposite side... You may also want to put an OGrid around the airfoil. If you put a CGrid around the airfoil (quality would be better at the sharp trailing edge) you would just need to balance those extra periodic edges on the other side. Note: I made the less important edges grey...

This image is the hub face blocking. You would have the same topology on the shroud and the blocks pretty much just swept between them... upstream of your cone, you would need another block with its corner edge on the axis, but that is no problem. You could build this in a "top down" way, or you could create a 2D blocking just like this and "extrude" it up to attach it to the FF and then add the final blocks upstream of the cone.
PSYMN is offline   Reply With Quote

Old   March 26, 2010, 08:12
Default
  #40
New Member
 
Andy Good
Join Date: Jul 2009
Posts: 11
Rep Power: 9
Andy QUB is on a distinguished road
Psymn,

That makes a lot of sense. It seems complex but doable! Unfortunately I'm out of the office for a week and then it may take me a while to wrestle with it but I'll let you know how I get on eventually.

Regards,
Andy
Andy QUB is offline   Reply With Quote

Reply

Tags
3d analysis, blade, rotating, turbine

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
Calculating lift force of a wind turbine blade problem LittleBart CFX 4 June 29, 2011 02:33
Inlet Flow Velocity or pressure gradient - modeling of a Wind Turbine Blade case LittleBart Main CFD Forum 5 January 10, 2011 16:07
force acting on gas turbine blade.... vvj Main CFD Forum 1 March 3, 2010 02:04
Wind Turbine Blade Geometry SeanieB Main CFD Forum 0 November 27, 2009 11:18
Flow study through Turbine Blade passage Subrata FLUENT 1 May 4, 2007 11:28


All times are GMT -4. The time now is 09:05.