Learning Forum

[Anthony Bowers]

Hello all!

I am trying to create a good quality mesh for a pipe with two bends (85 degrees) and a flow condtioner. I want a y+ < 5 for enhanced wall function with a realizable k-e turbulent model. However, I am struggling to obtain an acceptable orthogonality and skewness quantity with the inflation layer, first cell thickness, requirement. 

Here are a few images of my flow domain.

What does the community suggest? 

[Keyur Kanade]

You will need to define mesh sizing correctly. 

Please check following link. 

https://ansyshelp.ansys.com/account/secured?returnurl=/Views/Secured/corp/v221/en/wb_msh/ds_Sizing_Group.html

Also if you want y+<5 then if your surface mesh size is 1 mm try to get first layer of inflation of 0.1mm. 

Please check following videos

Ansys Meshing Sizing:
https://www.youtube.com/watch?v=w4q6q8nKF3U

Ansys Meshing: Meshing Methods:
https://www.youtube.com/watch?v=nEOC8rDnnRo

Ansys Meshing: Inflation:
https://www.youtube.com/watch?v=lrEHXizrhC0

 

Regards,

Keyur

How to access Ansys Online Help Document

Guidelines on the Student Community

Fluids Engineering Courses | Ansys Innovation Courses

 

 

[Anthony Bowers]

Hi ! 

I have applied some of the techniques you have recommended. For the most part, they worked so thanks, but now I am getting low orthogonality where flow conditioner holes and the main pipe meet, see image below. How do you suppose I resolve this issue? 

 

[Anthony Bowers]

Hi Keyru,

 

Thanks for your response. While the first link did not work I will review the other links and post my questions here.

[Rob]

I'd be more concerned with the jump in cell size at the end of the smaller pipes. I'm sure I've seen a similar geometry recently, if so, there are some suggestions in that thread. 

[Anthony Bowers]

I have checked forums with key word of "peforated plate", "Flow conditioner", "mesh " and have not been able to find anything but I will keep looking!

 

Ideally, I'd like a mesh like this 

 

I attempt a multizone for the larger pipes but it fails to decompose.. multizone only works for the smaller holes in the flow conditioner

[Rob]

/forum/forums/topic/design-modeler-for-fluid-simulaton/

I'd be inclined to use a tet/poly mesh in the complex part and sweep/multizone in the rest of the domain. 

 

[Anthony Bowers]

I have created a tet mesh in the complex part . However, when I use multizone/sweep I am being thrown back 

[Rob]

If you tet just the small tubes the inflation layer will break and do some very interesting things as they rejoin the main tube. This is why learning about decomposition is recommended: an old skill that becomes very useful in this sort of situation. If I had to use a hybrid tet & swept mesh I'd be meshing 5 volumes in total (if I counted correctly). 

The mesh in "wanted" image looks like something I'd have built in GAMBIT 15-20 years ago. I wouldn't have used any inflation, and the refined section looks like it may have been adapted. 

The warning is because you're not using the Worksheet (inside Meshing) to record the order inwhich you mesh things. 

Finally, the tet mesh you've shown is awful. Inflation is just to get a reasonable resolution perpendicular to the wall with as few cells as possible. You also need to consider flow separation, cell aspect ratio (because the flow won't be perfectly aligned to the walls and jump in cell size: at best you've got the first cell height about right. 

[Anthony Bowers]

I understand decomposition surface level, wherein volumes are broken down accordingly to allow easier meshing capabilities. In a straight pipe, this was very simple. For this geometry, I am worried about the intersection between the holes and the larger pipe, see the image below. 

[Rob]

That's not how I'd decompose it. Sweeping the larger sections shouldn't need the splits. 

[Anthony Bowers]

How would you decompose the mesh? 

The way I originally decomposed the mesh is like this 

2 large sections and 25 small section ( flow conditioner holes)

[Rob]

Think about the advice so far. Splitting the smaller pipes at the ends makes using inflation mesh difficult. There's no need to split the long sections axially. So, how would you sweep most of the long pipe but also connect the smaller pipes so you can use inflation and tets? 

I'm not able to just tell you as that's "specialist knowledge" and I don't want another conversation with Legal.... 

[Anthony Bowers]

Okay, I will take some time to think about this. Thank you for your guidance! 

[Rob]

So, how could you use tets in some regions, swept mesh elsewhere? The image above (omitting the remainder of the model) would split into 3 bodies. 

[Anthony Bowers]

 

 

Okay, I found a good video that I think exemplifies what you are talking about (

;  Workbench Meshing Methods for CFD | ANSYS e-Learning | CAE Associates). However, this is giving me a non-conformal mesh, and with no imprints of the flow conditioners, on the pipe ends, I am unable to give the domain wall boundary condition. Should I accept that a non-conformal mesh will occur and deal with the loss of accuracy from the interpolation of domains? Again thank you Rob for your help, you are being very patient with me and I thoroughly appreciate it. 

 

P.s,In that video, the user has the part separate, part 1 (containing 1 body), but he was able to get a conformal mesh without connections. I have mimicked this tutorial but when I import the mesh i (A) still have interface connections being read in; (B) obtaining a non-conformal mesh 

 

[Rob]

The image shows exactly what I mean, thanks for finding that. You also need to use Share topology (SpaceClaim & Discovery) or form a multibody part (DesignModeler). Mesh the awkward bit first and then work away from that zone meshing one zone at a time (the order will be retained in the Worksheet if you switch that on). 

[Anthony Bowers]

So I have conducted the recording of mesh, starting the the smaller FC holes and then the top/bottom pipes. The holes were a success but when I go to mesh the top, first, I am returned this error. Also should the inflation meshing be after the recording or during? 

[Rob]

I meant the video, your image only showed up now! Splitting like you have will cause problems. The error isn't the message you've shown, that's the warning that meshing has stopped. That may well be linked to inflation settings, Sweep doesn't use inflation in the same way as the tets. 

[Anthony Bowers]

Okay, here is a huge update. I finally understood the object and decomposed the geometry as seen below. 

I am able to get a Conformal mesh between the bodies, inflation on the larger pipe, and inflation in the smaller pipes. 

This is what the section plane looks like when sliced down the middle of the FC

Now I am facing an orthogonality issue of 6e-02. 

[Rob]

OK, on the mesh slice shown look for a blue-ish triangle. That will display whole elements and make it easier to see the cut plane. As you are using tet and prism focus on skewness. In meshing find the quality graph and you want to select cells with skew over about 0.9 to 0.95 then look at what's causing the poor quality. 

Once you've fixed that I think you're sorted.