[reza67]

hello everyones
i want to know what is the best way for meshing the 3d u-shape pipe in ansys
i'm begginer with ansys
plz explain me step by step


tnx a lot

[hwet]

whatever you do dont forget inflation, atleast 10 layers

[Gweher]

Hello Reza,

Well you're question has already been treated in various topics but I will give you the useful links. I've explained, step by step, the meshing procedure with AM for a 2D U-bend geometry. In your case you need to apply a similar approach for your 3D, you will find here a thread regarding structured mesh in a 90° bend pipe.

Have fun

[reza67]

Originally Posted by Gweher

Hello Reza,

Well you're question has already been treated in various topics but I will give you the useful links. I've explained, step by step, the meshing procedure with AM for a 2D U-bend geometry. In your case you need to apply a similar approach for your 3D, you will find here a thread regarding structured mesh in a 90° bend pipe.

Have fun

thanks Gweher
but i still couldn't find the best way to mesh my geometry
my geometry is a half u-tube like the picture shown below
could you help me ?

[amin.z]

Originally Posted by reza67

thanks Gweher
but i still couldn't find the best way to mesh my geometry
my geometry is a half u-tube like the picture shown below
could you help me ?

Hey
Maybe using sweep could help you!

[reza67]

Originally Posted by amin.z

Hey
Maybe using sweep could help you!

thanks amin
how can i decrease the mesh size in sweep method ?
what is the sweep element size ? line size? surface size ? volume size?
because it's scale is mm i think it should be line size but which line?

thanks again

[amin.z]

Originally Posted by reza67

thanks amin
how can i decrease the mesh size in sweep method ?
what is the sweep element size ? line size? surface size ? volume size?
because it's scale is mm i think it should be line size but which line?

thanks again

use this way:
first set a face size for one of the top faces of U tube

then use this setup:
mesh>insert>method

in geometry select the body
in method select sweep
in "src/trg selection" select "manual source and target"
in source select the face that apply face size
in target select another one face of top faces of tube
in "free face mesh type" choose "all quad"
and for "sweep num divs" enter an appropriate number! it's number of sweep layers!

I haven't experience in this shape but I guess this way should help you!

Good lock!

[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.

Originally Posted by Gweher; July 24, 2012, 17:36

For those who are curious, the problem was solved by selecting "manual source and target" under "sweep method" and specifying the source and target faces.

ElbowPipe90.jpg

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

[amin.z]

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.

Hooommm! So great mesh! nice job! bravo!

[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.

[Gweher]

Now the meshing part step by step:

1) rmb on mesh> Insert> Mapped Face Meshing (see Picture 1)
2) Select all faces (Using the Box select tool to select all the faces)
3) rmb on mesh> Insert> Method and select all 4 bodies
4) Change the Automatic type to Sweep (under Definition>Sweep)
5) Change Src/Trg selection from Automatic to Manual Source and Target (under Definition>Manual Source and Target - see Picture 2)
6) Select the 4 faces of one side as "source" and the 4 end faces as "target" (see Picture 3)
7) rmb on Mesh> Generate mesh (see Picture 4)
8) You can play with the mesh parameters to generate a more coarse/fine mesh

Hope this helped

[reza67]

thanks Gweher for your helpful information

could you help me to mesh the geometry which shown below

it's the grout around the pipe

[hwet]

i am doing the same thing, forming a new part from the different bodies and then meshing but for some reason my element boundaries dont fall on each other as seen from the picture. could anyone please have a look and explain why?

[Gweher]

hwet, are you sure that the 5 bodies are in the same part? As you import 5 "separated" bodies, the meshing tools meshes them in an independent way without matching the nodes at the interface (see pictures).

[Gweher]

Originally Posted by reza67

thanks Gweher for your helpful information

could you help me to mesh the geometry which shown below

it's the grout around the pipe

reza67, if you upload your .agdb file I can have a look at it.

[famon]

Thanks for useful guides, I loved the method

[famon]

Originally Posted by amin.z

use this way:
first set a face size for one of the top faces of U tube

then use this setup:
mesh>insert>method

in geometry select the body
in method select sweep
in "src/trg selection" select "manual source and target"
in source select the face that apply face size
in target select another one face of top faces of tube
in "free face mesh type" choose "all quad"
and for "sweep num divs" enter an appropriate number! it's number of sweep layers!

I haven't experience in this shape but I guess this way should help you!

Good lock!

Thanks for useful highlights, but this method doesnt support inflation, (inflation deactives in this method)
How can we use inflaton in this method?
Thanks alot

[hwet]

Thanks Gweher, I guess it was something to do with solid/fluid bodies, but just randomly ansys meshing would recognize these as sweepable bodies and at other times just wont sweep them automatically, even if i put in a method for sweeping with hex, it will say cant sweep these parts, and again at other times would just sweep these regions, see the attached picture of the same geometry but this time only the middle section is shown as sweepable
there are also some tet regions which get poor mesh quality, is it possible for you to have a look at my geometry? thanks

[amin.z]

Originally Posted by Gweher

Now the meshing part step by step:

1) rmb on mesh> Insert> Mapped Face Meshing (see Picture 1)
2) Select all faces (Using the Box select tool to select all the faces)
3) rmb on mesh> Insert> Method and select all 4 bodies
4) Change the Automatic type to Sweep (under Definition>Sweep)
5) Change Src/Trg selection from Automatic to Manual Source and Target (under Definition>Manual Source and Target - see Picture 2)
6) Select the 4 faces of one side as "source" and the 4 end faces as "target" (see Picture 3)
7) rmb on Mesh> Generate mesh (see Picture 4)
8) You can play with the mesh parameters to generate a more coarse/fine mesh

Hope this helped

Hey Gweher!
In the method you described, one simple domain is devised to 5 separate domains!
Is there any way to use some auxiliary lines without deviding domain!? One domain with various local meah! I think it's possible in gambit and ICEM...

[ayousaf]

Hi guys,

I have seen a few of the posts providing guidance for meshing pipe geometries including the ones provided in this post.


I am relatively new to this area and have a geometry which I am finding a bit difficult to discretise. I am using Ansys Workbench for everything here.
The geometry under consideration is a constricted artery, and I am trying to model the FSI between fluid and the arterial wall.

Over here, let us just consider the fluid mesh.

I first tried with a single body (revolved around a central axis) and generated mesh from that body.
1.JPG

I thought that the mesh near 4 edges within the circle was not good enough and was somewhat irregular.


So, I tried to alter the geometry to assist the sweep method for meshing. From my previous geometry, I created slices to form separate bodies and then combined then into one part. The mesh I obtained from this method is below:

a.JPG

b.JPG

d.JPG

e.JPG

When I cut the plane to inspect the mesh, the mesh at the inlet, outlet and near the constrictions does not seem to be good, you can see from the images that the division lines inside the tube are not straight and have quite high angles.
Furthermore, I am using dynamic meshing in fluent (with smoothing and re-meshing) and am getting "Update-Dynamic-Mesh failed. Negative cell volume detected" error and I don't know if that is because of these sharp angles or something else.

Is it probably because of the element size or the O-grid approach is not suitable for these types of geometries ? Is there something else that I should look into?

Any help with this will be highly appreciated.


Cheers!
Awais