CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   ANSYS Meshing & Geometry (http://www.cfd-online.com/Forums/ansys-meshing/)
-   -   [ICEM] HEXA-Fan blade with 2 sharp edges+tip clearance_Pics Attached (http://www.cfd-online.com/Forums/ansys-meshing/116025-hexa-fan-blade-2-sharp-edges-tip-clearance_pics-attached.html)

Catthan April 11, 2013 07:56

HEXA-Fan blade with 2 sharp edges+tip clearance_Pics Attached
 
Hi guys,

I thought it's about time I asked for some help on this.

So, a fan periodic section where the blade has 2 sharp edges and I want to consider the tip clearance.

The problem is the triangular blocks extruding from the tips of the blade to the shroud.. Too small and twisted for my skills to apply a y-block in the corner..

Converting the blocks to free or swept doesn't seam to work (not that I fully understand how to use this feature.. :o)

I have posted pictures of my 2 main attempts

1. I use a y-block to wrap the grid around the trailing edge. This worked in a simpler case without the tip clearance..
The problem is that edges are not parallel near the trailing edge so node spacing and quality is tough to handle inside the projected blade profile on the shroud.. Elements extruding from the tip to the shroud are bad..

http://i1219.photobucket.com/albums/...ps13b3d63c.jpg

2. A simpler attempt to block this similar to the pipe-blade tutorial. Here the only problem is the triangular blocks from the tip to the shroud..

http://i1219.photobucket.com/albums/...ps12e4da6e.jpg

If anyone could explain also how to use the swept/free blocks features I would appreciate this a lot..

I can't figure how to post the files, they're too big apparently :confused:
I can send them privately if anyone's interested or wants to practice blocking..

Thanks a lot!
Best,

Far April 12, 2013 04:27

why you want to use sweep blocks?

Catthan April 12, 2013 04:51

Quote:

Originally Posted by Far (Post 420074)
why you want to use sweep blocks?

Hi Far,

I don't "want" to necessarily, just thought it would take care of the elements inside the sharp corners of the projected blade profile on the shroud.

But as I said, I'm not sure how this feature works. Was hoping to fit triangular elements there if possible.

Would you suggest a different blocking strategy?

Thanks,

stuart23 April 15, 2013 02:02

1 Attachment(s)
IMHO if your edge angle is less than ~10 degrees, I think swept triangles would be a good way to go.

Don't be afraid of the triangles! If you start modelling squealer tips, it will be almost impossible to mesh everything structured.

Creating a swept block is as simple as going to Blocking > Edit Block > Convert Block Type, then set the type as swept. You only need to do it on the tip blocks, everything else can stay mapped.

To change the free face meshing type, go to the Settings menu > Meshing Options > Hexa Meshing and set the Free face mesh type to All Tri. If you want unstructured Quad mesh on the swept face, there is now the option to use the Gambit Pave. I think for tris, it uses PD no matter what you select. Simon?

Stu

Catthan April 15, 2013 03:28

Thanks Stu,

I will have a look at the example when I have access to a workstation later on today hopefully.

One more question if you don't mind.

After setting for swept block as you suggested, how do i get the tri-elements?
My understanding is they don't load with the rest of the hexa premesh, am I correct?
Should I compute the mesh?

'Cause I've been trying those settings myself but couldn't get any tri elements

I apologize for my naivety :o

Thanks,

stuart23 April 15, 2013 03:59

It should face mesh "on the fly". Mine did.

Stu

Catthan April 15, 2013 04:10

Quote:

Originally Posted by stuart23 (Post 420587)
"on the fly"

I assume you meant load straight from hex premesh

stuart23 April 15, 2013 09:56

Quote:

Originally Posted by Catthan (Post 420591)
I assume you meant load straight from hex premesh

Exactly :)

Catthan April 15, 2013 10:24

Quote:

Originally Posted by stuart23 (Post 420669)
Exactly :)

Yup, you're right..

Thanks!

stuart23 April 15, 2013 10:28

Whats the triangle quality like though? I'm slightly concerned given the thinness of your rotors.

Catthan April 15, 2013 11:57

Quote:

Originally Posted by stuart23 (Post 420683)
Whats the triangle quality like though? I'm slightly concerned given the thinness of your rotors.

You're right, quality is low (0.2) in the triangles near the blade edges and I'm trying to work around it.

Pospelov April 16, 2013 06:41

1 Attachment(s)
It's better to use hexa mesh. And you forgot about boundary layer.
My blocks for this geometry in the attach file. )
Alexander

Catthan April 16, 2013 08:26

Quote:

Originally Posted by Pospelov (Post 420881)
It's better to use hexa mesh. And you forgot about boundary layer.
My blocks for this geometry in the attach file. )
Alexander

That's briliant Alexander, thanks a lot!

You're right, there was not any boundary layer in my original blocking.

I will try and apply your strategy to my geometry.

Thanks again!

Catthan April 26, 2013 06:26

Ok guys,

sorry for resurfacing an old thread but still need some help.

So,

I applied Alexanders blocking strategy (great!), however I could not fine-tune the quality.

The problem was with the elements fitting in the 2 sharp corners, low angle particularly

I then again went back to a swept block to see what those elements would be like if I specified a tri-mesh.

The overall quality improved and I have 22 elements between 9-18 degs.
I was hoping Fluent would take those.

The Det. 3x3x3 is 0.3

For hexa quality (not premesh) I have 4 elements (2 in each sharp angle) at 0.2 and the rest >0.35

Here is a picture

http://i1219.photobucket.com/albums/...ps97962e42.jpg

Those are 2 elements on one sharp edge, one on the shroud and on the blade. There are 2 more on the opposite edge.

Fluent crashes on the first iteration ( AMG, pressure correction etc..) and I try to figure out what is so wrong with the mesh.

Is it those 4 elements?

If anyone wants, I can email blk. and tin file. The latter is too big to attach here.

Any ideas will be appreciated.

Thanks,

Pospelov April 26, 2013 07:29

I don't think that the problem in the mesh. But you can check it in Fluent.
I've got some quetions.
- Which geometry angle do you have?
- Do you use the rotational domain?
- Which settings do you use(Pressure based, tubulent model and others)
You can send me the latter, if you want. My mail is PospelovAlex@mail.ru.
Pospelov Alexander.

Catthan April 26, 2013 08:08

Quote:

Originally Posted by Pospelov (Post 423321)
I don't think that the problem in the mesh. But you can check it in Fluent.
I've got some quetions.
- Which geometry angle do you have?
- Do you use the rotational domain?
- Which settings do you use(Pressure based, tubulent model and others)
You can send me the latter, if you want. My mail is PospelovAlex@mail.ru.
Pospelov Alexander.

Thanks Alexander.

-min angle 9-13.5 degs
-yes, rotational domain
-pressure based, Spal- Alm., mass flow inlet, standard pressure discretization, SIMPLE scheme.

I am sending you the ICEM files.

Best,

Pospelov April 26, 2013 09:06

Quote:

Originally Posted by Catthan (Post 423324)
Thanks Alexander.

-min angle 9-13.5 degs
-yes, rotational domain
-pressure based, Spal- Alm., mass flow inlet, standard pressure discretization, SIMPLE scheme.

I am sending you the ICEM files.

Best,

OK. 9/2 = 4.5 degree. This angle you would have if you use that blocks.
I've tested you mesh. It's OK. I think that you use the mixing plane as rotor-stator interface. In this case the mistake in Solution Initialization. You must have the flow rate through mixing plane. It cannot be 0.
Fluent has some problem with mixing plane.
I've got a big tasks, so I usualy use:
- Pressure based solver
- RNG k-e
- Pressure inlet/outlet
- SIMPLIC
- Solution controls:
Pressure 0.03
Density 0.1
Body forces 0.1
Momentum 0.07
(all default / 10)
It's slow but usualy I can obtain the solution.
Pospelov Alexander

Catthan April 26, 2013 11:30

Quote:

Originally Posted by Pospelov (Post 423342)
OK. 9/2 = 4.5 degree. This angle you would have if you use that blocks.
I've tested you mesh. It's OK. I think that you use the mixing plane as rotor-stator interface. In this case the mistake in Solution Initialization. You must have the flow rate through mixing plane. It cannot be 0.
Fluent has some problem with mixing plane.
I've got a big tasks, so I usualy use:
- Pressure based solver
- RNG k-e
- Pressure inlet/outlet
- SIMPLIC
- Solution controls:
Pressure 0.03
Density 0.1
Body forces 0.1
Momentum 0.07
(all default / 10)
It's slow but usualy I can obtain the solution.
Pospelov Alexander

Thanks for checking Alexander,
it's a great relief to hear that the mesh is acceptable.

I wasn't using mixing plane, more like a rotating reference frame (and a stationary one).
But I noticed that when I switched my non-conformal periodic walls back to walls the solution progressed whereas when I recreated the non-conformal periodics it kept crashing.
So far I think the problem may have been with Fluent's auto-compute of the periodic offset (By Fluent: 59.999 etc and by me 60.00) When I set it myself to 60 it seems to work. I 'll verify during the weekend.

Thanks


All times are GMT -4. The time now is 15:54.