[hwet]

For sweep meshing the number of cells in the cross section of the thicker part and the thinner part will remain the same. hence it reduces the cell size to put in the same number of cells in the constriction. slice vertically before and after the constriction as well, then you will be able to simply sweep the two cylinders created without any slices. for the converging part err well try meshing it separately.

[ayousaf]

Originally Posted by hwet

For sweep meshing the number of cells in the cross section of the thicker part and the thinner part will remain the same. hence it reduces the cell size to put in the same number of cells in the constriction. slice vertically before and after the constriction as well, then you will be able to simply sweep the two cylinders created without any slices. for the converging part err well try meshing it separately.

Thanks for the response hwet.

I tried that before (2 cylindrical bodies on either side and constriction in between). However, there were no other slices there to divide the cylinders. The issue there was that the mesh and inlet and outlet faces was not uniform(skewed) and at constriction I had unstructured mesh.

I think you meant to say keep the slices that I showed in my last post and add two extra vertical slices? I actually thought of that after my post, but the issue that I am having there is with the constriction.


As you can see that the cylinders are easily swept and the mesh in those regions is structured, but when it comes to the constriction, I am having a bit of an issue.

a.JPG
b.JPG

What is happening here is that I am trying to create slices (with loft function) at the constriction but as you can see from the image below that vertices on two sketches are not being associated in correct way for some reason. Hence I can not create slices here and this in turn is causing poor quality in constriction and imposing bad quality in other regions as well.

d.JPG
c.JPG


I think if I can associate the vertices correctly, that should fix the problem.
Do you know if there is a way to fix this within workbench ?

Thanks again for you help, I really appreciate this!


Cheers!
Awais

[hwet]

if you really want a structured mesh used ICEM,

but you can have a tet mesh at the constriction and a hex mesh elsewhere, a tet mesh with inflation layer is as good as a hex mesh in terms of the quality of the final results you will obtain.

[ayousaf]

9

Originally Posted by hwet

if you really want a structured mesh used ICEM,

but you can have a tet mesh at the constriction and a hex mesh elsewhere, a tet mesh with inflation layer is as good as a hex mesh in terms of the quality of the final results you will obtain.

I think I managed to fix that problem. There is a function within workbench to fix the vertices, I just found it.

I have obtained a structured mesh within workbench.

1.JPG
2.JPG

However, when I went on to inspect it, I found this butterfly like pattern
3.JPG

Any idea what might be causing this?
I think that this will significantly affect the solution.

[hwet]

when you do a cut section of a mesh, there is an icon in the same toolbar to display the whole of the cells, you are just cutting though the cells in a straight line and hence see this...

[ayousaf]

Originally Posted by hwet

when you do a cut section of a mesh, there is an icon in the same toolbar to display the whole of the cells, you are just cutting though the cells in a straight line and hence see this...

Hwet, I will check this and post the result here.

Thanks for your help throughout

[Antanas]

Originally Posted by ayousaf

Hi guys,

Try to split your geometry where cross-section changes. But IMO you shouldn't cut your geometry, but use multi-zone method with proper inflation to get O-grid.

[Omish]

Originally Posted by Gweher

Here is a step by step procedure for your half 3D pipe:

1) Create a "path" sketch in a plane (in my case "Centre_Line_Path" in the XY plane)
2) Create a "profile" sketch in a perpendicular plane (YZ plane with a half pipe geometry sketch)
3) Use the Sweep option create the geometry (see Picture 1)
4) Create a "slice sketch" in the same plane as the profile sketch, in this case you will need 2 sketches for the Ogrid slice, a "upper part" and a "lower part" (here "Ogrid_slice_1", see Picture 2)
5) Use the Sweep option, selecting the "Ogrid_slice_1" as profile and "Centre_Line_Path" as path, replacing "Add Material" by "Slice Material" under the Operation tab in order to slice the existing geometry (See Picture 3)
6) Create a second slice sketch (for the lower "Ogrid part") "Ogrid_slice_2" and repeat the point 5)
7) At the end you will obtain 4 parts, to mesh them as a single entity, select all 4 solid > rmb > Form New Part (See picture 4)

Now you're done with the geometry.

Ghewer I don't know how to thank you. Your tutorial and patience involved was very helpful. Just one simple question about it.
When we "Form a new part" and put our slices in one part, doesn't it have any problem while analizing? I mean does Fluent simply understand the whole geometry is a single pipe and not 4 parts of flow beside one another?

[arunuknome]

Thanks a lot @Gweher. You guys are doing excellent work out here.

[desmond0204]

Originally Posted by Gweher

The method Amin described is the correct one. In my previous post I've mentioned a topic with 3D pipe where I explained the sweep method Amin described.



As it's nearly the same geometry (1/2 of the model) you can use the same meshing strategy.

Hi! How do you define the multiple inlets created at boundary conditions?

[Udayraj12]

Hello Everyone,

I am trying to simulate two phase flow in horizontal pipelines. I obtained structured meshing of Pipe using ICEM. However, I realised that I need to have two inlets instead of one at circular face of pipe and this is not possible in ICEM. So, Can anyone tell me how to do structured meshing of Pipe in workbench without using ICEM?

Thank you,

Regards

[Antanas]

Originally Posted by Udayraj12

However, I realised that I need to have two inlets instead of one at circular face of pipe and this is not possible in ICEM.

Are you sure?

Originally Posted by Udayraj12

So, Can anyone tell me how to do structured meshing of Pipe in workbench without using ICEM?

MultiZone + Inflation + Mapped Face

[Udayraj12]

Thank you so much

[Udayraj12]

I am doing numerical simulation of gas and liquid two phase flow through horizontal pipelines. What criteria should be chosen for the Mesh Independence study?

[Antanas]

Originally Posted by Udayraj12

I am doing numerical simulation of gas and liquid two phase flow through horizontal pipelines. What criteria should be chosen for the Mesh Independence study?

Changes of variables of interest should asymptotically vanish

[RRT]

Hi everyone.
I have difficulties in meshing a cyclone separator , I'm beginer in Ansys .
Please can you explain me step by step

[Mounarah]

is this procedure of meshing would be good if this tube will be considered qs a serpentine inside another rectangular fluid domaim.I'm wondering on the fact if the interface between the two regions would be affected because it is sliced.thanks