[Richeom]

Ok, thanks very much for your help. I needed it.

[Saima]

Hello PSYMN,

I have two question.
1. I have an airfoil (basically a section of blade), but coordinates are available in 3-dimensions then what will be steps of blaocking?

2. I have 2D airfoil and if i want to convert it in a 3D blade. What will be main steps in ICEM.


Thank you,

Originally Posted by PSYMN

I usually create a tunnel myself... In that CGrid far field case I used a pressure far field. This would be a good question for the Fluent Solver Forum...

[PSYMN]

1) There are several tutorials that will train you toward this goal... Basically, you would do what I did in 2D, but start with a 3D block and do everything on both faces... Or start with a 2D block and then extrude it. More complex methods are needed if you have an interesting wing tip or the wing tip is far from the wall (because you want to be more efficient), etc.

2) You could use extrude on the geometry and mesh (or blocking). Or you could copy the blade profile out and create a lofted surface, etc. ICEM CFD has geometry tools to get the job done, but you may also want to do it in a proper CAD program and just import the full 3D geometry. If you wing has taper or twist or various airfoils along its length, it is still topologically the same and, you could still just extrude the 2D blocking (Create blocks => 2D to 3D) and associate the new indices to the various wing sections... There is no specific tutorial for this (that I know of), but try some tutorials for general practice and look at some of the other cases (CFD-Online threads) where I already went thru specific examples in detail.

Simon

[Saima]

Hello Simon,

I have attached my 2D airfoil in x,y,z coordinates here. If i do 3D blocking that mean it gives me a box and my airfoil inside that. 4 curve on top plane and 4 curve on bottom plane. I am wondering how to do blocking in this case curve associate etc...

I did meshing (coars) which is attached here.When i try to import it it gives me error:
"Unable to import mesh: Region FLUID can only be defined in terms of elements or faces or nodes - not a combination of two or more."

Why is that?

If u have a look and suggest me some steps it will be really appreciated.

Thank you,

Originally Posted by PSYMN

1) There are several tutorials that will train you toward this goal... Basically, you would do what I did in 2D, but start with a 3D block and do everything on both faces... Or start with a 2D block and then extrude it. More complex methods are needed if you have an interesting wing tip or the wing tip is far from the wall (because you want to be more efficient), etc.

2) You could use extrude on the geometry and mesh (or blocking). Or you could copy the blade profile out and create a lofted surface, etc. ICEM CFD has geometry tools to get the job done, but you may also want to do it in a proper CAD program and just import the full 3D geometry. If you wing has taper or twist or various airfoils along its length, it is still topologically the same and, you could still just extrude the 2D blocking (Create blocks => 2D to 3D) and associate the new indices to the various wing sections... There is no specific tutorial for this (that I know of), but try some tutorials for general practice and look at some of the other cases (CFD-Online threads) where I already went thru specific examples in detail.

Simon

[PSYMN]

Samia,

The *.prj files are not enough.

The *.tin file is the geometry and mesh parameters. (I need this)

The *.blk file is the blocking (This would be nice if you have taken a first try)

The *.uns file is the mesh (I don't need that).

[Saima]

Hello Simon,

I have attached *.prj ,*.tin, *.blk here.

Regards,

Originally Posted by PSYMN

Samia,

The *.prj files are not enough.

The *.tin file is the geometry and mesh parameters. (I need this)

The *.blk file is the blocking (This would be nice if you have taken a first try)

The *.uns file is the mesh (I don't need that).

[Saima]

Hello Simon,

I need your help in the following mesh, I am making 2D airfoil in 3D coordinate system. I used 3D Blocking but when i am gng to import my mesh in CFX it gives me error.

"Unable to import mesh: Region FLUID can only be defined in terms of elements or faces or nodes - not a combination of two or more."


Kindly let me know, how can i avoid it?

Best Regards,

Originally Posted by PSYMN

Samia,

The *.prj files are not enough.

The *.tin file is the geometry and mesh parameters. (I need this)

The *.blk file is the blocking (This would be nice if you have taken a first try)

The *.uns file is the mesh (I don't need that).

[PSYMN]

A model is composed of a fluid surrounded by boundary conditions...

In your model, the volume and the shells (or the the shells and the lines if 2D) are in the same part. The solver can't separate the fluid from the bocos (it doesn't make sense to apply fluid properties to the boundary around a fluid...

You need to go back to ICEM CFD and make sure that the fluid part contains either all volume elements or all shell elements, it can't handle a combo.

Simon

[Saima]

Thank you simon i undesrtand wat u are saying but i dont know how to implement it. I am telling u my steps which i followed kindly let me know wehere i shud make chnages:


1. First i imported points for airfoil.
2. Create periodic lines + input and ouput line.
3. Generate a surfae with a name "Fluid" by taking (input+ouput+Per1+per2 lines)
4. Create a 3D "Block" by taking "Fluid" in the part option.
It generates a reactanguler box around airfoil.
5. I did association around 2D shape(Input+output+periodic lines around airfoil) with this box.
6. Split the block in length and width .
7. For meshing follow the steps as u did in airfoil (on you-tube).

Now, kindly let me know where i shud make changes?

Waiting for your reply.
Regards,

Originally Posted by PSYMN

A model is composed of a fluid surrounded by boundary conditions...

In your model, the volume and the shells (or the the shells and the lines if 2D) are in the same part. The solver can't separate the fluid from the bocos (it doesn't make sense to apply fluid properties to the boundary around a fluid...

You need to go back to ICEM CFD and make sure that the fluid part contains either all volume elements or all shell elements, it can't handle a combo.

Simon

[PSYMN]

Those steps look fine... But you need to check again if you have anything but Shells in your fluid part...

Turn off all your parts.

Turn on your Fluid Part.

Turn on points, fit to screen to see if you have any points.

Turn on curves, fit to screen to see if you have any curves...

If you have any curves or points in "fluid", you shouldn't. Put them into other parts, and then recompute the premesh, etc.

If that doesn't turn anything up, just load your mesh file... Under info, you can see mesh info. This will tell you how many elements are in each part and each type... Check the number of elements in the FLUID part. Then check the number of elements in the "Shells" part... they should be the same.

Simon

[Richeom]

Is it possible to have a 2D wind turbine blade geometry, much like the one designed in the youtube videos mentioned above, which moves with a given speed from left to right, so that the blade movement can be accounted for separately to the wind speed?

How would I go about doing this?

[PSYMN]

Maybe someone else will have a good idea, but the way I see it, wind speed is all relative.

If you want to say that the blade is moving in a certain direction, you can do that with a 2D model by setting the boundary flow velocity. Essentially, you are pretending the blade is still, but the air is moving past. This is similar to how we would check aerodynamics in a wind tunnel (car is still, air is moving). And is no different to how we would model the situation if the airfoil were moving thru still air.

If you also have wind with another vector, the only way I know to do it is to adjust the boundary condition vector so you take care of both the motion and the wind with the same boco.

Pretend the airfoil is still and add the motion and wind vectors to get the boco.


Now what if your blade is turning around the Z axis (XY plane) (like a regular wind turbine) and the wind is just moving along the XZ plane... Then you have bocos which are not 2D and you really need to model in 3D. Put the 3D turbine blades in a cylinder that you can rotate within the greater far field. This would separate the blade motion from the Far field wind boco.

You can represent this sort of thing in 2D with a vertical wind turbine because motion plane and the wind plane are the same (without the 3rd D). Is that what you are asking about?

[Richeom]

Yes, that's what I'm asking about. I'm trying to model a horizontal axis turbine, so if I understand you correctly, that would be best done in 3D.

I am hesitant to use 3D as I don't have the geometries for the specific blade.

I will model it as a still blade in a tunnel. For this I should define the upper and lower boundaries as walls and a velocity inlet on the left and an outflow on the right? (I think that at these windspeeds I can't use a far field boundary as air is being modelled as incompressible)

Given that the vector addition of the speed of the blade and the windspeed will mean that the wind is coming from, roughly speaking, NW of my blade, should I have a short distance between the blade and the inlet so as to lessen the effects of the upper wall? What is the best way to lessen the effect of this wall?

[PSYMN]

Right, to model the actual turbine, you need 3D, but to model the flow over an airfoil on that turbine, you can use 2D with some vector addition...

But actually their are more factors to consider...

It is a radial system with a particular angular velocity, so you need to consider how far from the hub your cross section is to properly calculate its velocity...

Also, most tubine blades twist (have varying angles of attack) along the blade to make the most of the increasing velocity hub to tip... Your specified airfoil will be set at a particular angle...

so, you need to figure out the airfoil velocity at a particular cross section, and combine that vector with the wind direction vector AND the angle of attack for the airfoil...

This will give you the angle to put your blade in the tunnel...

The flow thru the tunnel is always direct from inlet to outlet, parallel to the walls.

You always need to keep sufficient distance upstream and downstream of the blade... Up stream, 3 to 6X the wind tunnel width should be a good place to start. I am not sure what the official number for 2D airfoil analysis is, but I usually add a 6X diameter extension upstream to any piping assembly I am interested in to prevent any flow from trying to go back out the inlet (more than enough). Now as for your tunnel width... In an ideal world, it will be wide enough that you solution will show undisturbed free stream flow before the side wall...

Just do one and have fun with it... This should solve pretty quickly so you can afford to experiment. Check the results with the mesh visible and see if you have any oddities where the flow pattern seems to be interacting with the mesh or boundaries... Adjust as necessary. Then help out your fellow CFD-Onliners by publishing the results of what it took back here.

Simon

[neilpan]

Hi Simon,

I am doing similar research on a hydrofoil (vertical axis tidal wave turbine) and your tutorial videos are extremely helpful. Sincere thanks for taking the time to teach the rest of us

[PSYMN]

-----------------------------------------
Please help guide development at ANSYS by filling in these meshing surveys

Public ANSYS ICEM CFD Users Survey

This second one is more general (Gambit, TGrid and ANSYS Meshing users welcome)...

CFD Online Users Survey

[wangquan]

hello,all
I am a new ,recently I search for the iecm airfoil meshing,the video at www.youtobe.com/ansysinc, it is very useful to me,but I can not open the internet,meybe it is closed in my courtury.if anyone have these video,please send me by email.My email is quan_wang@foxmail.com
thank you all!

[tgrt18]

Hi all
i suggest to use chimera capability if your solver have it. basically you need a background mesh which is a global mesh around the cylinder (O grid the best way) and child grid around your airfoil. the only problem that chimera does not guaranty the conservation

thanks Simon

[spraveeng]

I am doing project on aerofoils
I have taken NACA 0012 aerofoil, meshed it in gambit, and made it to run it in fluent - it was working
then
I have taken NACA 0006 aerofoil did the same process and solution is not converging
some one please tell the reason behind this

i am trying to calculate the coefficient of lift from fluent
some one please help

[Edward!]

Hi

There are many many options...

First check the grid in fluent before run your calculation, and check the mesh, if that its ok, maybe the flow conditions are wrong; and you will have reversible flow thats way the solutions doesnt converg.

I recomend the K epsilon turbulence model
And the residuals under 1x10-3


Greetings
I hope this can help