# (AutoGRID 5) Problem in Geometry definition of propeller

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

 June 14, 2012, 13:10 (AutoGRID 5) Problem in Geometry definition of propeller #1 Member   venkatesh Join Date: May 2012 Posts: 93 Rep Power: 12 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

 June 15, 2012, 11:18 #2 Senior Member   Hamid Zoka Join Date: Nov 2009 Posts: 282 Rep Power: 17 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

 June 17, 2012, 08:58 #3 Member   venkatesh Join Date: May 2012 Posts: 93 Rep Power: 12 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.

 June 17, 2012, 13:55 #4 Senior Member   Hamid Zoka Join Date: Nov 2009 Posts: 282 Rep Power: 17 Dear Venkatesh; please leave an image of your blade and curves you have defined in Autogrid5. regards Hamidzoka

 June 17, 2012, 17:59 #5 Member   venkatesh Join Date: May 2012 Posts: 93 Rep Power: 12 Dear Hamidzoka, Since my laboratory is closed today, I will post the image of the propeller blade tomorrow. Thank you, Venkatesh

June 18, 2012, 15:25
#6
Member

venkatesh
Join Date: May 2012
Posts: 93
Rep Power: 12
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.

Thank you,
Venkatesh
Attached Images
 BladeZOOM.jpg (66.5 KB, 300 views) DOMAIN.jpg (65.4 KB, 218 views) zoom contra_rotors.jpg (40.4 KB, 180 views) CONTRA_ROTOR.jpg (41.3 KB, 160 views)

June 21, 2012, 05:26
#7
Senior Member

Hamid Zoka
Join Date: Nov 2009
Posts: 282
Rep Power: 17
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.
please chack and let me knoe the result.

regards
Attached Files
 Drawing.pdf (6.9 KB, 232 views)

 June 21, 2012, 05:52 #8 Member   venkatesh Join Date: May 2012 Posts: 93 Rep Power: 12 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

June 21, 2012, 12:42
#9
Member

venkatesh
Join Date: May 2012
Posts: 93
Rep Power: 12
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
Attached Images
 Capture.jpg (53.4 KB, 163 views)

 June 23, 2012, 00:13 #10 Senior Member   Hamid Zoka Join Date: Nov 2009 Posts: 282 Rep Power: 17 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 Last edited by Hamidzoka; June 23, 2012 at 12:35.

June 23, 2012, 21:49
#11
Member

venkatesh
Join Date: May 2012
Posts: 93
Rep Power: 12
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
Attached Images

 July 17, 2012, 06:06 #12 Member   venkatesh Join Date: May 2012 Posts: 93 Rep Power: 12 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.

 July 18, 2012, 00:10 #13 Senior Member   Hamid Zoka Join Date: Nov 2009 Posts: 282 Rep Power: 17 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

 July 31, 2012, 15:05 FineTurbo #15 Member   venkatesh Join Date: May 2012 Posts: 93 Rep Power: 12 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. John1956 likes this.