Learning Forum

[Losiola]

Hello Evryone

HOpe you are all doing good

 

I have a problem with fluent meshing where i am trying to mesh a wind turbine blade so for the first step (surface mesh ) evrything works good but unfortunatlly for the filling it gets me this error :

 

Please note that i get this errot for certain settings in the mesh (certain sizes) but for some other sizing values it doesn't show this error

Can anyone please help me? Also if anyone can help me mesh a wind turbine blade i'll be so Thankfull

 

Kind regards

[Karthik Remella]

How do those sizes (which work) compare with the overall size of the blade (perhaps, blade thickness)? Are you prescribing them such that you have a sufficient number of elements? Also, is your blade curved? If so, are you using curvature or proximity settings?

Thanks

Karthik

[Losiola]

Hi ,

My blade is a 2.04m it has 3types of airfoils shapes and also  twisted . the cord of the airfoils(blade section) starts from 0.240 m at about 10% span with 16° angle  and gets to 0.01m profile cord at the tip of the blade with 0° twist angle .

Thickness : on the  tip side like from 70%-100% span wise , the trailing edge thikness is very small about 0.1mm or less

for the sizing: i currently used for local sizing :curvature with 1mm-3mm on the blade surface  with 10° angle and the same minimum setting and angle for the surface siziing Min=1mm  and 10° angle ....>these settings gave good  mesh on the surface and lots of elements on the blade surface too .

but when i change the minimum value of curvature and surface sizing to 0.5mm it guives me that error ?.

Do you have any idea about what's the problem ?

 

Also  i forgot to mention one more  issue last Time , iN the mesh that worked there are zones were the BL mesh collapsed as you can see  the difference in the pics . How Can i Fix This Problem ? (Please Note that i used the waterTight Workflow)

Many Thanks

 

 

[Karthik Remella]

Yeah, this is not good at all. Have you tried to provide a local refinement around the airfoil? Perhaps, a Body of Influence around the airfoil might help. 

If I'm to take a guess, you might be seeing a sudden jump from your inflation layers to the rest of the mesh and it could potentially be the issue.

Also, what settings are you using to create the Boundary Layer Mesh? Could you please try the 1st layer thickness?

Regarding the error message: Could you please try to leave the angle to default and change only the local size to 0.5 mm and try? 

Also, I'm assuming that there are no errors in the geometry. I'm sure you have done this, but for completeness - I'd still say it out here - Could you please open the geometry in SpaceClaim, right-click on the part, and perform 'Check-Geometry' on your part. There should not be any errors.

Thank you.

Karthik

[Losiola]

Hi,

For the Geometry check i did it there is no errors i also cleaned the Geometry .

for the Boundary layer  i use Last-ration with first cell hight 0.01mm and 20 layers 

for the Boi i used one  i selected size of 8mm and another bigger one with size of 16 mm and i got total elements of about 4.5M elements

Thanks

 

[Karthik Remella]

Thank you for the update. Could you try my other suggestion about using the default curvature angle (but with a different local size)?

Thanks.

[Keyur Kanade]

i guess, you have not selected those boundary zones / labels for prism generation. 

please cross check boundary layer step in workflow. 

if required, delete old boundary layer controls and create new one by selecting correct boundary zones. 

Regards,

Keyur

 

If this helps, please mark this post as 'Is Solution' to help others.

Guidelines on the Student Community

How to access ANSYS help links

 

[Losiola]

Hi Kremella,

I ve did that also for the default curvature angle and i still get the same issue.

 

[Losiola]

Hi Kkanade,

I am so positive i ve selected the correct label which is blade that i defined earlier in SCDM  otherwise i wouldnt get a boundary layer mesh from the first place

 

Regards

[Keyur Kanade]

i suggest cross check the selected labels for boundary layer. 

it must be missing atleast one label at the trailing edge. 

Regards,

Keyur

 

If this helps, please mark this post as 'Is Solution' to help others.

Guidelines on the Student Community

How to access ANSYS help links

 

 

[Losiola]

Hi kkanade

 

I really did the checking and the labels are correct and there is no missing label.

 

My sense is telling me it's failing because of the very sharp  Trailing edge but i am not sue , is it possible that there is some parameter that controles this?

 

Many thanks

[Karthik Remella]

If this is the case, could you try and make a small straight cut at the trailing edge so instead of a sharp corner, you have a small straight edge. Could you please test this and let us know?

Thanks.

Karthik

[Losiola]

Hi Karthik

I did as you told me i cut just little bit of the Trailing edge and....IT WORKED  Thank you very much

 

Thank you all for the Support

Regards

[Karthik Remella]

Good to know that it answered you question. 

Good luck!