CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   NUMECA (http://www.cfd-online.com/Forums/numeca/)
-   -   (AutoGRID 5) Problem in Geometry definition of propeller (http://www.cfd-online.com/Forums/numeca/103243-autogrid-5-problem-geometry-definition-propeller.html)

venkat_aero2007 June 14, 2012 12:10

(AutoGRID 5) Problem in Geometry definition of propeller
 
Hi,
I am trying to generate a structured mesh for contra-rotating Propeller using Autogrid 5. The Propeller geometry is in IGES formate.I have a problem in the geometry definition of propeller. In the case of a propeller, the shroud does not exist. In the user Manuel It has been said that shroud must be defined using a curve cutting the tip of the propeller definition. But I am not clear with the definition. I tried to define my geometry without shroud definition but it in the geometry check it gives me a warning saying that shroud has not been defined. Can some one help me to mesh my geometry.

Thanks in advance for your valuable information

Venkatesh

Hamidzoka June 15, 2012 10:18

Dear Venkatesh;
You have to define a shroud curve even if it does not intersect with the propeller blades.But you can define a shroud gap for your blades in Autogrid5. This parameter is in fact the distance between shroud wall and blade tip. In fact your blades can have a finite distance from shroud , but you cannot remove the shroud when working with Numeca!

regards

venkat_aero2007 June 17, 2012 07:58

Dear Hamidzoka,

Thanks for your information. Do you mean that "I can draw a curve (parallel to the hub) far above the tip of the propeller blade and define that curve as a shroud.

One more query, I Imported Propeller blade geometry (IGES Formate) into Autogrid5, and I defined the geometry as you said but When I did geometry check it tells me that Hub does not intersect with blade. But every thing looks perfect. Could you please tell me a method to solve this problem.

Hamidzoka June 17, 2012 12:55

Dear Venkatesh;
please leave an image of your blade and curves you have defined in Autogrid5.

regards
Hamidzoka

venkat_aero2007 June 17, 2012 16:59

Dear Hamidzoka,

Since my laboratory is closed today, I will post the image of the propeller blade tomorrow.

Thank you,
Venkatesh

venkat_aero2007 June 18, 2012 14:25

4 Attachment(s)
Dear Hamidzoka,

Have a look on the images of my propeller blade. Also I have attached the Igs file. you can click on the link below and download it.
http://jyraphe.isae.fr/file.php?h=R0...4ba790af838797. In first figure, I defined the base where the blade is attached as HUB. In The second figure shows the domain that I have created. I define the top Portion of the domain as Shroud but when I define Shroud, it say 180 degree discontinuity. When I associate blade portion to Autogrid I am not getting the exact shape of the blade (you can see that in figure1).

The full view of contra rotor can bee seen in the figure 3 &4.

I am struk up in generating mesh with with Autogrid. Please help me

Looking forward for your suggestion

Thank you,
Venkatesh

Hamidzoka June 21, 2012 04:26

1 Attachment(s)
Dear Venkatesh;
Approach of flow simulation in Numeca is different from what we see in CFX, Fluent, StarCD, etc.
in Numeca Fine/Turbo you don't need to model flow boxes. these boxes are automatically generated in the Numeca. All you need to import to numeca is just a blade geometry, hub curve and a shroud curve.
this model at its present form cannot be appied to numeca simulations.
for solving this problem I have following suggestions:

1- import your blade (just blade and not a subtracted model) in .igs format. it is important that you change the reference frame such that flow direction is Z and blade span is set to R.
2- drow and import hub and shroud as R,Z curves, your blade geometry should intersect these curves. your model at its present form needs r=cte. curves as hub and shroud. this can be easily drawn in CAD softwares and imported to Autogrid. but the only issue is that the height of the blade should be selected such that it initially intersects with the hub and shroud curves. regarding your model it is difficult to intersect your blade model with the shroud curve because of its far distance to the blade tip.
if you succeed to find such an intersection, you can define a shroud gap for the blade such that your blade finds its real height.
attached dwg may help you find a better insight.
please chack and let me knoe the result.

regards

venkat_aero2007 June 21, 2012 04:52

Dear Hamidzoka,
Thanks a lot for your reply. I was without any idea to start the problem. Through your suggestion I got an Idea to start the meshing.

"1- import your blade (just blade and not a subtracted model) in .igs format. it is important that you change the reference frame such that flow direction is Z and blade span is set to R."


Could you please exaplain me how to change the reference frame in Autogrid.

My professor told me to simulate the flow using FLUENT.

Regards,
Venkatesh

venkat_aero2007 June 21, 2012 11:42

1 Attachment(s)
Dear Hamidzoka,
Hi found the way to fix the reference frame. I imported blade, hub and shroud curves as you said. I tried with hub shroud extension but it fails. But I have a problem in intersection of blade with hub and shroud. Please have a look on the image.

Regards

Hamidzoka June 22, 2012 23:13

Dear Venkatesh;
This last fugure looks good, although it does not intersect with hub and shroud curves properly. To do so, open "row1" in "Rows Definition" column. A folder opens and there is another folder entitled as "Main Blade". right click on it and select "Expand Geometry". a window opens in which you can set the extension from hub and shroud regions.
I think this solves your problem. But since this tool applies an extrapolation on your geometry, it may lead to a twisted or maybe a discontinuous one. if it happens, try extending your blade geometry manually in your CAD software then import it to Autogrid5 for mesh generation.

Regards

venkat_aero2007 June 23, 2012 20:49

4 Attachment(s)
Dear Hamidzoka,
Using CAD software I extended the blade such that it intersect with the hub curve. but when i define the trailing edge curve, autogrid showed me a warning message "Bad Stream-wise orientation". then i proceeded to generate mesh and defined the mesh distribution parameters. when i clicked Blade to blade(B2B) preview (Figure 2and 3). it displayed me a message " overlapping detected in row1". I continued and Finally generated a 3d mesh. at the end of 3D mesh generation process, it displayed a message " optimization failed". In the mesh quality report there were huge number of negative volumes.

Could you suggest me some idea to get rid off negative volumes.

Regards

venkat_aero2007 July 17, 2012 05:06

Dear Hamidzoka,
I am I have generated a nice mesh around my propeller blade. but I have negative cells in far field. Actually I gave a tip gap of 0.25mm. I think the problem is because of the tip gap. If I increase the radius of the far field the, I get more negative cells. I tried to change the expansion ration and the grid point distribution. but all these didn't work well to solve the negative cell problem. Please suggest me some idea to solve this problem. waiting for your reply.

Hamidzoka July 17, 2012 23:10

Dear Venkatesh;
following points regarding the meshing file comes to my mind:
- mesh distribution near the trailing edge needs to be modified. the current mesh near the TE is quite distorted and needs to be changed. you can do this by this way: row mesh control > B2B mesh topology control > Blade points distribution > trial control > relative control distance.
default value is 1.0. you can redistribute the mesh at TE by changing this value.
one useful criteria for improving the mesh quality at TE is that "try changing this value so that TE finds mesh distribution similar to LE".

- number of elements at trailing edge is quite higher than number of elements assigned to outlet boundary. this causes distortion of elements. there must be a balance between these elements.

regrads

venkat_aero2007 July 18, 2012 14:57

Dear Hamidzoka,

Thanks for you information. I think for contra rotating fan wizard, there is no option called relative control distance. ( Blade points distribution > trial control > relative control distance)..

Actually In grid point distribution there are two parameter
1. Number of points in Throat
2. Number of Points in Clearance O-mesh.

Actually I tried to reduce number of optimization steps for far field to 50 then all the negative cells disappeared. But the orthogonal quality was very low - 4.2. When I increased number of optimization steps, I got huge number of negative cell in the far field ( only above the tip region of the blade). I also get more negative cells when I increase the number of control line.

with a far field radius 10, I get a mesh without negative cells (less optimation steps), with a quality of 4.2 in far field. My Should have a Far field radius of 21. So When I increase the far field radius I get huge negative cells and bad quality elements.

I have attached the mesh files. Could you please have a look on it.

Here is the link.

geomTurbo
https://www.dropbox.com/s/spgoqdz4u7...lity.geomTurbo

igg
https://www.dropbox.com/s/wpyqropt1v...ow_quality.igg

.trb
https://www.dropbox.com/s/0q0g7tmlw5...ow_quality.trb

https://dl-web.dropbox.com/get/Nouve...fig?w=4c7aa661

I am struggling hard for past one month to mesh this geomentry. It will be a great help from your side. Looking forward for your reply.

venkat_aero2007 July 31, 2012 14:05

FineTurbo
 
Dear Hamidzoka,
I have meshed my geometry. I am trying to simulate flow around Contra rotating Fan using Full Non Matching Mixing Plane. IThe flow is steady and incompressible with a blade speed of 1029 rpm. I use Spalart–Allmaras turbulence model with velocity inlet (68 m/s), pressure outlet (Radial equilibrium) as the boundary condition and I imposed Farfield velocity as 68 m/s. The Periodic angle for the front rotor is 32.7272 degree and 40 degree. There are nearly 6.5 million cells.

In the initialization of simulation, I gave 98500 pascal as inlet pressure and 90000 pascal as pressure in mixing plane. I ran simulation, after two iteration it say solution blow out, Process killed, Crashed. I tried with different boundary condition but nothing helped me. I am not able to figure out the problem.

Please Can you give me some suggestions to solve my problem.


All times are GMT -4. The time now is 08:17.