|
[Sponsors] |
[ANSYS Meshing] Ansys meshing result very high skewness |
|
LinkBack | Thread Tools | Search this Thread | Display Modes |
March 10, 2012, 21:28 |
Ansys meshing result very high skewness
|
#1 |
Senior Member
mohamed khedr emam
Join Date: Oct 2011
Location: Egypt
Posts: 121
Rep Power: 15 |
My Geometry is a wind turbine blade in a huge Air enclosure (1000m depth x 300m height)
I built it in Solidworks then select the enclosures in DesignModeler and started AnsysMeshing,I had tried many mesh types and reduce sizing BUT the skewness alawys is very high as below: Element 11088617 skewness Min 2.136 E-10 skewness Max 0.99999498 Any suggestion (I think to try ICEM CFD but iam not professional) |
|
March 11, 2012, 01:29 |
|
#2 | ||
Senior Member
|
Quote:
Quote:
|
|||
March 11, 2012, 06:10 |
|
#3 | |
Senior Member
mohamed khedr emam
Join Date: Oct 2011
Location: Egypt
Posts: 121
Rep Power: 15 |
Quote:
1-could you tell me how to spot the max skewness area? 2- When I tried ICEM by import the geometry From DM , the domains (Enclosures) looks different that in AM I didn't know why , iam still beginner in ICEM thanks again |
||
March 11, 2012, 08:44 |
|
#4 |
Senior Member
Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,663
Blog Entries: 1
Rep Power: 47 |
In ANSYS Meshing, left click on the mesh branch of the tree...
In the resulting details panel, expand the statistics branch... Under Mesh metric, choose "Skewness" from the pulldown. A histogram will appear below the graphics window. Left click on the bar of the histogram and its elements will appear. If the bar you want to see is too small to click easily, click on the "controls" button and adjust the X and Y axis to zoom in on the bad cells. When you click on a bar, you will see those elements on the screen...
__________________
----------------------------------------- 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 |
|
March 11, 2012, 08:49 |
|
#5 |
Senior Member
Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,663
Blog Entries: 1
Rep Power: 47 |
Oh yea, what to do with what you find...
Look to see where the skewness is coming from. 9 times out of 10, it is due to over constrained geometry forcing the mesh into awkward configurations... If the over-constrained geometry is just surface patches (like a sliver surface forcing the mesh to conform) you could try the patch independent tetra or you could try virtual topologies to merge the surface patches together... If it is between regions, such as between your turbine and the boundary of the rotating region... That second boundary is arbitrary... and you could just increase the size of that disk to allow for more space (flexibility) for the mesh... If it is something else, post the pic. Best regards, Simon
__________________
----------------------------------------- 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 |
|
March 11, 2012, 10:43 |
|
#6 |
Senior Member
mohamed khedr emam
Join Date: Oct 2011
Location: Egypt
Posts: 121
Rep Power: 15 |
I reached to bad elements , I will try to repair them
Many thanks Last edited by m5edr; March 11, 2012 at 11:41. |
|
March 12, 2012, 08:52 |
|
#7 |
Senior Member
mohamed khedr emam
Join Date: Oct 2011
Location: Egypt
Posts: 121
Rep Power: 15 |
Dear simon
I reached to bad elements in My geometry (attached photo) It is because "Inflation" that used around the blade (this "Inflation" is nessary due to Boundary Layer consideration) Without Inflation >>> Max Skewness is 0.87 (prefect) With Inflation>>>> Max Skewness is 0.9999 I tried many types of inflation that result in same High Skewness any change. Any suggestion, Thanks |
|
March 12, 2012, 09:03 |
|
#8 |
Senior Member
Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,663
Blog Entries: 1
Rep Power: 47 |
You would have to zoom in to get a better idea of what is going on...
My guess is that the inflation at the top of the blade is meeting the inflation from the other side... Since they meet at a trailing edge, you get a sharp angle between them. No amount of smoothing or other "mesh" fixes will solve this problem because when you make one side better, the other side gets worse. Some people fix this problem by putting a zero thickness baffle behind the trailing edge. This splits the angle (prism grows from both sides) and solves the problem... However, where the thin prism baffle ends, you may have other problems if you can't taper it out. (I know how to taper it out in ICEM CFD, but I don't know how in ANSYS Meshing, maybe someone else knows). But you could also just try sending it to the solver as it is. The solver can often handle these sorts of poor quality prisms much better then it would handle poor tetras...
__________________
----------------------------------------- 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 |
|
March 12, 2012, 11:13 |
|
#9 |
Senior Member
mohamed khedr emam
Join Date: Oct 2011
Location: Egypt
Posts: 121
Rep Power: 15 |
Many thanks for replay , i am really appreciated that
I attached more closer image , any change in your replay after this images Note: there is no inflation at the top of the blade (Inflation at both sides of the blade) thanks again |
|
March 12, 2012, 11:15 |
|
#10 |
Senior Member
Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,663
Blog Entries: 1
Rep Power: 47 |
I had expected they were just along the trailing edge...
I guess the wing tip could be a similar problem where the prisms are tilting to miter around the tip...
__________________
----------------------------------------- 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 |
|
March 12, 2012, 11:37 |
|
#11 |
Senior Member
mohamed khedr emam
Join Date: Oct 2011
Location: Egypt
Posts: 121
Rep Power: 15 |
||
March 16, 2012, 13:06 |
try advanced size function and adjusting your max/min sizes
|
#12 |
New Member
Join Date: Dec 2010
Posts: 8
Rep Power: 15 |
It looks like either your advanced size function is off or your are not setting the correct max/min sizes. Try setting the physics preference to CFD.
|
|
March 16, 2012, 13:17 |
|
#13 |
Senior Member
Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,663
Blog Entries: 1
Rep Power: 47 |
@m5edr, by "wing tip", I just meant the tip of the airfoil shown in your images... I guess it may not actually be a wing...
__________________
----------------------------------------- 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 |
|
March 16, 2012, 22:09 |
|
#14 | |
Senior Member
mohamed khedr emam
Join Date: Oct 2011
Location: Egypt
Posts: 121
Rep Power: 15 |
Quote:
My advance size function is ON and also i tried many size function !! Any way i started ICEM , May it comes new News |
||
March 16, 2012, 22:13 |
|
#15 | |
Senior Member
mohamed khedr emam
Join Date: Oct 2011
Location: Egypt
Posts: 121
Rep Power: 15 |
Quote:
I started ICEM , it provide many tools to fix the mesh Till now I face same problem but i think solution is close and maybe i need your help if i stopped thanks again |
||
January 5, 2014, 17:11 |
Very high skewness within two cell zone.
|
#16 |
Senior Member
Tanjina Afrin
Join Date: May 2013
Location: South Carolina
Posts: 169
Rep Power: 13 |
Hi Simon,
I am modeling a 3D object. I found very high skewness in between two cell zone using workbench meshing. Before starting the "run Calculation" , I checked " check case" and it gives me this warning that 696 cell exceed 0.98 skewness. I found a way using Fluent 14.5 to repair the face mesh, but couldn't find any way how can I repair this skewness within the cell zone. Please find the attached image for details. My model's mesh has high aspect ratio also i.e. 14.3, but Fluent didn't give any warning regarding this. Any suggestion for lowering the skewness will be highly appreciated. Thanks in advance. Regards, Tanjina |
|
March 31, 2015, 05:11 |
best way to reduce skewness and its successful, i tried
|
#17 |
New Member
S.Frank Richarrd
Join Date: Mar 2015
Posts: 1
Rep Power: 0 |
by using inflation> use auto inflation> programmed controlled and i generated my mesh. it shown the skewness value as 0.8999.
then i tried inflation> use auto inflation> none then i got the skewness value as 0.822 |
|
February 3, 2020, 12:30 |
|
#18 |
New Member
Andy
Join Date: Oct 2019
Posts: 4
Rep Power: 7 |
Where is this option auto-inflation?
I am unable to find it. Please help. Thanks |
|
February 3, 2020, 12:35 |
|
#19 |
New Member
Andy
Join Date: Oct 2019
Posts: 4
Rep Power: 7 |
Never mind. I found it. It is set to none already.
It is under mesh details> inflation. Is there any other way to reduce the maximum skewness? |
|
Thread Tools | Search this Thread |
Display Modes | |
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
[ANSYS Meshing] ANSYS Meshing hangs at "Preparing to model boundary for part" | jonny_b | ANSYS Meshing & Geometry | 12 | June 12, 2012 02:55 |
[ANSYS Meshing] ANSYS Meshing vs GAMBIT | aerospain | ANSYS Meshing & Geometry | 0 | September 28, 2011 07:05 |
Parallel Meshing in ANSYS 13 | makkks | ANSYS Meshing & Geometry | 1 | September 5, 2011 13:34 |
Interface between meshes and high skewness | Danny | FLUENT | 0 | September 13, 2005 12:23 |
Multicomponent fluid | Andrea | CFX | 2 | October 11, 2004 06:12 |