[Kyriakos]

Hi again,

I'm trying to mesh a wind turbine blade and i am having some problems near the trailing and leading edge areas respectively. I've watched a tutorial (#8) with a similar geometry and although i am using the same options for perimeters spacing, i can't manage to have more nodes near the trailing or leading edge perimeters of the blade. If anyone has any ideas i would really appreciate it. And one more thing, is there a way to get the spacing options of a pre-meshed geometry, because i have saved a previous mesh, but when i open the file, ANSA does not keep the options that were used for the particular mesh.

Thanks...

[vangelis]

Hi Kyriako
May I ask which tutorial you are referring to exactly?

Have you checked your units?
How large is the model?
Have you made a measurement on the model?
What is your Min and Max length as well as sharp edge lenght
on Spacing AutoCFD?

About your second point.
If you want to "save and re-apply" your meshing strategy
you should use Batch Mesh.
Please refer to Batch Mesh tutorial under CFD category

Best regards
Vangelis

[Kyriakos]

Ηι Vangeli,

Thanks for the answer. The tutorial is titled as "Live introductory webinar on ANSA for CFD" (the one with an F1 car on the cover), which has a blade example at the end.

My model's length is close to 0,13 meters, and my settings are:
Min length 0.005
Max length 0.02
sharp edge length (convex/concave) 0.005

Anyways i think i've fixed that problem...but now i have a new one!!
The resulted mesh of the the blade's suction side is much more smoother in contrast to that of the pressure side. The problem is that the mesh at the pressure side seems to grow very fast resulting in a big number of max length elements, while at the suction side the elements size grow uniformly. So, when i try to increase the max length (and decrese the min length) , the resulted mesh at the pressure side is even worse because some nodes which are tangent to the blade's leading edge, are unable to connect with the nodes next to them resulting in big and non-uniform elements. Maybe it has something to do with the distortion angle...If you have any ideas on that it would be very helpful.

Regarding the second point, what i wanted to ask is if there is a way to retrieve the auto cfd settings of an imported mesh created in ANSA at a previous point.

Sorry for writing such a long reply but i couldn't explain the above problem in a less detailed way!!

Thanks again

[vangelis]

Hi Kyriako,

My recommendation is that you should better work with mm units and not metres.

Units are also related with the Tolerances (both accessible from settings)

Check that your units are metres, and your tolerances are medium
that is 0.05 and 0.2.

If you want to scale up your model use the function Transform>Move>Scale

Once your model is 130mm long
and you min length=5
and max length=20
i believe things will work better


About the second point, no you cannot import settings from an old meshed model, unless you meshed it with Batch Mesh.
If you use Batch mesh all your meshing strategy is saved in the ANSA file and hence you can re-apply it on a new model.



Let me know how it goes

Vangelis

[Kyriakos]

Hello Vangeli,

First of all, thank you for your reply. Although i made of your suggestions (units into mm and tolerance, max and min length) the mesh became even worse (mesh with lines instead of triangles!!). I also tried to scale my original geometry (by 0.001) and the result was that my model disappeared , and couldn't find it even with zoom window...probably i'm doing something wrong. Anyways now i'm working with meters again and i 'm having the same results as mentioned in my previous reply. So i think that maybe the problem has to do with the Distortion angle or the Sharp edges angle because it seems that the mesh elements cannot "fit" with the curvature near the leading edge.
If you have any suggestions on that i would really appreciate it.

Thanks

[vangelis]

Have you checked if you have some values for Min and Max Length in Presentation Parameters/Quality criteria window (F11 key)?

Otherwise you need to send some images of the problematic mesh and the following snapshots.
1) The model with a measurement on it visible
2) Your current Settings>Units/Tolerances
3) Your Quality criteria
3) Your Mesh Parameter settings

Best regards

Vangelis

[Kyriakos]

Hi again,

I couldn't find any Max and Min Length as options in Presentation Parameters/Quality criteria window. I took the snapshots you told me...Let me know if you need anything else.

Thanks for the help

[Kyriakos]

By the way i'm sorry for the bad quality of the uploaded images but i had to compress them due to the upload files size limit of 195 KB. If there is a different way to upload the snapshots retaining a good quality let me know...

[vangelis]

Indeed the images are blurry.
You could have sent images of the just the windows.

I am also missing the Quality Criteria Settings for Shells tab
to see what quality criteria you have (skew, min length etc)

Anyway it seems that your model is indeed in metres and your tolerances are correct respectively.

However I would like to insist that you change your Units to millimetres
Please follow these steps
1) Go to Settings>Units change the pulldown to mm, activate the
Scale model dimensions flag and press Apply and OK.
2) Now your model should be in mm, so it should have a chord length at the tip of around 100 and a span of 2000 (if I can see well from the images)
Your tolerances should now be 0.05 and 0.2
3) Now use Spacing Auto CFD with
Growth 1.2
Curvature angle 15
Min length =5
Max length =20
convex and concave sharp edge length =5
Press OK
4) Then use Shell Mesh CFD Visible
What is the result now?
post images
if you still have problems cut the blade is say 4 spanwise sections to make smaller macros to mesh

[Kyriakos]

Hey, here are some of the snapshots you asked with a better quality than before, including the Quality Criteria settings. I will apply the settings on the scaled (mm) model as you told me and i 'll let you know probably tomorrow...

Thanks for the suggestions Vangeli

[Kyriakos]

Hi Vangeli,

I did as you suggested and here are the results. The leading edge mesh is much better than before (pressure and suction side respectively) but now i am having some problems at the trailing edge (sharp mesh), which might be reduced by selecting Refine Trailing Edge Ratio i guess (i am testing it right now). I also have to mention that in order to obtain these results, besides scaling my model in mm and using the spacing settings you posted, i had to change the perimeters Length number (trailing and leading edge curves respectively) and put a much smaller one, specifically equal to 0.1. The problem is that i have a large amount of mesh elements as you can see in the images i posted (considering that my wind turnine has 3 blades), and now i need to dicrease somehow the number of them (maybe increse the Max length andGrowth rate a bit...). Anyway thanks a lot for helping me and i'll let you know about the results i am waiting for.

[vangelis]

I am glad things get better.

In order to reduce the element count you should use anisotropic meshing.
See slide 19 of
http://www.beta-cae.com/pdf/ansa_met...esentation.pdf

So you do not reduce the element length so much at the leading edge
and mesh with CFD algorithm and then you use the function Shell Mesh>Zonecut Gradual
and you set first height, growth and number of rows

Is you trailing edge sharp or curved?

[Kyriakos]

My trailing edge is curved normally, but as you can see from the last two posted images, the current mesh settings make the trailing edge sharper than the real one.

[vangelis]

You should use anisotropic mesh as I described both on leading and trailing edges
In this way you capture the curvature but you do not increase cell count dramatically

[Kyriakos]

Ok thanks, i'll give it a try and let you know about the results.

[Kyriakos]

Hey, it's me again...

Is there a tutorial or something relating to anisotropic mesh and how to use Zone Cut because i can't make it work...I have to mesh the geometry first and then use Zone cut, right?

And after this i have to choose every little edge (of each element) that belongs to the leading or trailing edge?? And then ANSA needs another edge selection again... HELP!!

[vangelis]

Please have a look at the online help
Press Ctrl+Left mouse button on Zonecut function to get more details.

Also in order to select many edges in one click activate the Corner Angle selection tool at the bottom of the GUI

[Kyriakos]

Ok thanks, i wasn't aware of that function...