[Keizers]

Hi all,

I am new to CFX and the meshing programs (I've used, or tried to use let's say, ICEM and Ansys Workbench Meshing), so I am trying to do something I think should not be too complicated, but I am failing quite badly. Sorry if it is something very basic. I hope someone can help!

Also, apologies if I should be posting this in the CFX forum and not here, I wasn’t sure where to post it since it is a bit of both!

Basically, I want to create a mesh for a circular pipe to run it in CFX using the k-epsilon model. The pipe I want to use is of the same dimensions than the Butterfly valve tutorial in CFX (it is a pipe with diameter 0.04m and length 0.2m), but without the valve. I am using half a pipe because of symmetry (I could be using a quarter really, but I wanted to keep it the same as the model with the valve in)

I started using Ansys Workbench (I have version 14.0). I have no issues using the design modeller. For the Meshing, I tried following a tutorial I found for creating the mesh for a Fluent simulation (using sweep). I was able to create a mesh (see first picture), and then use it in CFX. However, I did something wrong because after running the simulation (water, inlet given by Cart. Vel. components [approx. Re=10^5], outlet set to average static pressure and set to 0 Pa) the y+ values along the pipe wall are in excess of 150,000!!! (it started at 150,000 and then carried on increasing to around 300,000)

I tried to refine the inflation layers, but if I made them much smaller, CFX solver would give errors and not be able to get a solution.

Therefore I tried using ICEM. I followed another tutorial that showed you how to make a hexa meshing (and also included an O-grid). The mesh (see second picture) looked quite different to the one I had created in Workbench (I didn’t think it looked very promising), but after running it in CFX with the same conditions, I got again y+ values of over 150,000.

I then tried to use ICEM to create a mesh as similar as possible to the one used in the butterfly valve tutorial (but without valve), the 3rd image is what I got. It made no (major) difference when running it, the y+ was around 140,000 at the inlet at the wall, increasing to about 300,000 at the end of the pipe.

What am I doing wrong? I assume I am not setting something right in the mesh, as in CFX I am doing exactly the same as in the tutorial. Let me know if you think having the ICEM project files would make it easier to know what I've done wrong.


Please help!

Many thanks,

K

[diamondx]

RE=10^5, the height for the first element should be very very small use the y+ calculator

[Far]

150,000 ! Check the units of your model.

[Keizers]

Ali,

I’ve used the y+ estimator (you mean this one: http://www.cfd-online.com/Wiki/Dimensionless_wall_distance_%28y_plus%29). I’ve tried setting the mesh so that the first layer is small enough (the calculator gave me a wall distance of 8.3e-5m, although I’m not sure if it’s completely applicable as it seems to be for flat plates, so I had to input the diameter of the pipe in the BL length box). If I try to set it too small (I used 25 layers and tried to set it so that the first one was 8.3e-5m), the solver crashes (I think this message that appears during the run has something to do with it):

****** Notice ****** |
| A wall has been placed at portion(s) of an OUTLET |
| boundary condition (at 35.1% of the faces, 6.2% of the area) |
| to prevent fluid from flowing into the domain. |
| The boundary condition name is: outlet. |
| The fluid name is: Water. |
| If this situation persists, consider switching |
| to an Opening type boundary condition instead.

I reduced the number of layers to 15 (still trying to keep the estimated wall distance, I’ve attached a picture), and it run (the same notice appeared, but it went away after 100 iterations or so). It made no difference, my y+ is still huge as before.


Far,

I think my units are correct, I’ve created the model from scratch and have been using meters all the way through. I might have missed something, but I’ve looked around and found nothing. I cannot really find a way to find which units are being used in ICEM, but the STEP file I imported was in meters.


I don’t think changing the outlet (to solve the notice shown above) will help as I had no problems with it when running the tutorial (in which I got y+ values of around 500 even at Re=10^5, and the inflation layers are considerably larger). This is why I think there is something I am not setting up right in the mesh, something I am missing…

Any ideas?

[flotus1]

This is not a crash notice from your solver, just a warning.
Read the FAQ

What boundary condition do you have at the inlet? If you use a constant velocity, it is natual that you have high Yplus-values here, no matter what cell height at the wall.
Use a velocity profile instead, or even better, use periodic bondary conditions.

With very thin cells at the walls, it is also recommended to run the solver in double precision. Good luck.

[Far]

What the difference in using the velocity inlet or pressure inlet? you set the pressure inlet so that you get the correct velocity at the inlet and vice-verca.

If this proposition is correct (which seems logical but same also hold with pressure inlet condition) then this should be problem only at inlet, once the boundary layer is developed this problem should disappear. In other words at inlet region there should be high Y+ then y+ should gradually change.

By the way did you notice that the velocity used in the Y+ formula is not the inlet velocity !!! Do you have idea what is the value of velocity gradient in normal direction in the inlet region?

http://www.cfd-online.com/Wiki/Dimen...tance_(y_plus)
http://www.cfd-online.com/Wiki/Friction_velocity

[Keizers]

Hi flotus1,

I know it was just a warning, but the solver crashed eventually, I think because it could not get away from the problem of having to blo0ck part of the outlet. I've had that warning in other simulations, but it eventually goes away and although the solver takes more iterations to finish, it does work.

At the inlet I have zero velocity for y and x components (i.e., in the plane perpendicular to the pipe axis) and a velocity profile (one-seventh power law) for the z-axis velocity component (w).

I'm just trying to simulate fully developed turbulent flow, no time varying effects, not sure how would periodic BC help?

Far,

For the formula I have used the free-stream velocity (average velocity of the profile), as the calculator tool asks (http://www.cfd-online.com/Tools/yplus.php).

I have read somewhere that the 1/7 power law has an unrealistic velocity gradient at the wall (it's one of its limitations), but the same profile worked fine with the mesh provided by CFX for the tutorial with the valve, so I do not think the problem is to do with the conditions in the CFX simulation, I think the problem is with the mesh. I've tried to strip the CFX tutorial mesh from the bit of the valve, but the way it has been created, I can't find a way.

I think my problem is: if you want to create a mesh for a simple pipe of 0.04m diameter, 0.2m length (or any other dimension in that sort of ballpark), for Re=10^5 with water, fully developed turbulent flow right from the inlet, what do you do to get sensible y+ values? It's only a pipe, no strange features or anything like that...

Thanks,

K

[flotus1]

For a fully developed flow in a pipe, I would definitely recommend periodic boundary conditions.
Just to make sure (please dont get this the wrong way) when you say jau have a power-law velocity profile for the "z-axis", is your "z-axis" defined as the wall-distance?

As far as the Yplus-values are concerned: The estimations from the tool mentioned above are only a starting point.
From here on, you can iteratively improve your mesh. If you want a Yplus-value of 1, but get a value of 50 in the first run, make the first cell thinner by a factor of 50. After 1 or 2 loops the values will be pretty close.


Edit: Keep in mind that Yplus is not the only parameter to watch here. The volume jump between the prism layers and the rest of the mesh shouldn't be too high either. This is likely to cause the error message with the backflow.

[Far]

Hey pipe is very short (L/D = 5!) . You should use periodic bc as suggested by flotus1

[Far]

yplus is around 7, when used 0.01 mm spacing in ICEM. Velocity is 5 m/sec. Y+ increased to 11 when spacing is 0.1 mm. For 1 mm spacing, Y+ is 4500.


Mesh with 0.01 mm spacing is shown in pic.


PS : Solver is Fluent 14

[Keizers]

Far,
I assume the mesh creation process is the same for Fluent than for CFX?
Would you be willing to send me the ICEM project files so that I can see if there is something you are setting up different (other than using Fluent) that makes it work? Alternatively, I could send you mine, if you are not happy sending yours. Thanks!
I haven't been able to find information on periodic BC in the CFX help file, as I say, the tutorial itself works fine without them from what I know.
Yeah I know the pipe is very short, I wanted to solve a short pipe first and then move on to a longer one.

[Far]

Here you go ....

PS . I have used the dimensions in mm in ICEM. ,Proper scaling was done in Fluent and same is true for the CFX ( 0.001, 0.001, 0.001)

[Far]

@ flotus1

If we use the periodic boundary condition in the stream wise direction then how to make sure that the velocity at inlet is 5 m/sec?

Should we define the pressure gradient in periodic bc panel? If yes, how we will calculate the pressure gradient for velocity = 5 m/sec?

[flotus1]

You will have to calculate the pressure gradient or the volume force from some analytic formula (Re=10^5 is in the middle between Blasius and Nikuradse)

[Keizers]

Hi Far, many thanks! Sorry I haven't been able to reply until today. The zip file does not contain the mesh file, could you send it? (I feel bad asking again, I promise I'll only use it to see what I have missed creating my own mesh. I cna give you my email if you prefer it to posting it here)

[Far]

Right click on the premesh and choose option " convert to unstructured mesh"

[Keizers]

A bit stupid of me. I knew how to do that, I had done it with one of the meshes I made, and completely forgot. Anyways, many thanks Far.
CFX doesn't like it too much though, peak y+ value is now 1.6e6. It had problems with the outlet though (the warning where it says it's blocking part of it), which hadn't gone away when the solver went below the residual error I had specified and stopped. It took almost 20min to run, so I might reduce the residual error to make it run fo longer and see if the outlet issue goes away, but I don't think that is a very sensible way of doing it. I will let you know if I get anywhere!
Thanks,
K

[Far]

Do you mean CFX behaves differently than the Fluent? Why?

[Far]

CFX Results :

Yplus is same as Fluent almost.

Solver : ................ Yplus.................. Solver Yplus (Y*)

CFX : ..................0.26 ................. 11.225 (scalable wall functions)

Fluent : .................. 7.89................ 11.225 (scalable wall functions)



What type of boundary conditions you are using in CFX?

I have provided following:

Wall = no slip

In = velocity inlet with 5 m/sec

out = pressure outlet with average static pressure = 0

Pipe length = 0.2 m

[Keizers]

Hi Far, sorry again for the delay, I have too many other things going on and can't dedicate as much time as I would like to to this. From Monday/Tuesday I should be working on it much more.

I sincerely don't know why my results are so different. I have the same boundary conditions, except that the velocity I had used was 6.7m/s (to get Re=3x10^5), and this velocity is set as a profile, so U and V are zero and W (velocity component z-axis) is the one seventh power law:
w=Wmax(1-r/R)^(1/7) (where Wmax is about 8m/s since Wave/Wmax=0.8167)
but I don't see how can that make a difference. I will try to use 5m/s and see what comes out (I don't have Ansys in this computer unfortunately won't have access to it until Monday).
Another thing I recall I may have different is the blending factor in the outlet (is it called that? sorry, I can't remember). There are two values you need to fill when you choose average static pressure as BC, the pressure itself and a factor. I have that as 0.05, as it is in the tutorial of the valve.
And finally, I have noticed you are doing it from within workbench, whereas I was doing it directly in CFX. But surely there is no difference there?

Thanks a lot for your help in this. I hope we get to the bottom of it (and I hope I don't find out it was just sheer incompetence from me, although maybe that would make the solution easy!) I will let you know as soon as I can run it with 5m/s.

K