CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > ANSYS > ANSYS Meshing & Geometry

[ANSYS Meshing] meshing the 3d u-pipe in ansys

Register Blogs Members List Search Today's Posts Mark Forums Read

Like Tree12Likes

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   October 8, 2014, 12:45
Question meshing the 3d u-pipe in ansys
  #1
Member
 
Join Date: May 2014
Posts: 31
Rep Power: 12
reza67 is on a distinguished road
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
reza67 is offline   Reply With Quote

Old   October 9, 2014, 20:23
Default
  #2
Senior Member
 
Join Date: Mar 2014
Posts: 375
Rep Power: 13
hwet is on a distinguished road
whatever you do dont forget inflation, atleast 10 layers
hwet is offline   Reply With Quote

Old   October 10, 2014, 06:05
Default
  #3
Senior Member
 
Gweher's Avatar
 
Gwenael H.
Join Date: Mar 2011
Location: Switzerland
Posts: 392
Rep Power: 20
Gweher will become famous soon enough
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
Gweher is offline   Reply With Quote

Old   October 12, 2014, 11:05
Default
  #4
Member
 
Join Date: May 2014
Posts: 31
Rep Power: 12
reza67 is on a distinguished road
Quote:
Originally Posted by Gweher View Post
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 ?


reza67 is offline   Reply With Quote

Old   October 12, 2014, 11:18
Default
  #5
Senior Member
 
amin.z's Avatar
 
Amin
Join Date: Oct 2013
Location: Germany
Posts: 397
Rep Power: 14
amin.z is on a distinguished road
Quote:
Originally Posted by reza67 View Post
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 likes this.
amin.z is offline   Reply With Quote

Old   October 12, 2014, 14:23
Default
  #6
Member
 
Join Date: May 2014
Posts: 31
Rep Power: 12
reza67 is on a distinguished road
Quote:
Originally Posted by amin.z View Post
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
reza67 is offline   Reply With Quote

Old   October 12, 2014, 15:52
Default
  #7
Senior Member
 
amin.z's Avatar
 
Amin
Join Date: Oct 2013
Location: Germany
Posts: 397
Rep Power: 14
amin.z is on a distinguished road
Quote:
Originally Posted by reza67 View Post
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!
f.kh likes this.
amin.z is offline   Reply With Quote

Old   October 20, 2014, 04:43
Default
  #8
Senior Member
 
Gweher's Avatar
 
Gwenael H.
Join Date: Mar 2011
Location: Switzerland
Posts: 392
Rep Power: 20
Gweher will become famous soon enough
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.

Quote:
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.
famon likes this.
Gweher is offline   Reply With Quote

Old   October 20, 2014, 05:02
Default
  #9
Senior Member
 
amin.z's Avatar
 
Amin
Join Date: Oct 2013
Location: Germany
Posts: 397
Rep Power: 14
amin.z is on a distinguished road
Quote:
Originally Posted by Gweher View Post
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!
amin.z is offline   Reply With Quote

Old   October 20, 2014, 06:26
Default
  #10
Senior Member
 
Gweher's Avatar
 
Gwenael H.
Join Date: Mar 2011
Location: Switzerland
Posts: 392
Rep Power: 20
Gweher will become famous soon enough
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.
Attached Images
File Type: jpg Half_Pipe_Geometry.jpg (43.3 KB, 328 views)
File Type: jpg Upper_Ogrid_Slice.jpg (42.6 KB, 313 views)
File Type: jpg Sweep_Slice_Upper_Ogrid.jpg (44.5 KB, 313 views)
File Type: jpg Half_Pipe_Geometry_Final_Ogrid.jpg (50.4 KB, 315 views)
k.farnagh, Baden and Teso like this.
Gweher is offline   Reply With Quote

Old   October 20, 2014, 06:45
Default
  #11
Senior Member
 
Gweher's Avatar
 
Gwenael H.
Join Date: Mar 2011
Location: Switzerland
Posts: 392
Rep Power: 20
Gweher will become famous soon enough
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
Attached Images
File Type: jpg Mapped_Face_Method.jpg (52.5 KB, 266 views)
File Type: jpg Manual_Source_and_Target.jpg (55.7 KB, 219 views)
File Type: jpg Manual_Source_and_Target_Selection.jpg (56.0 KB, 221 views)
File Type: jpg Final_Mesh.jpg (68.5 KB, 294 views)
Gweher is offline   Reply With Quote

Old   October 28, 2014, 05:22
Default
  #12
Member
 
Join Date: May 2014
Posts: 31
Rep Power: 12
reza67 is on a distinguished road
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 is offline   Reply With Quote

Old   November 2, 2014, 21:54
Default element boundaries
  #13
Senior Member
 
Join Date: Mar 2014
Posts: 375
Rep Power: 13
hwet is on a distinguished road
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?
Attached Images
File Type: jpg mesh.jpg (78.2 KB, 181 views)
hwet is offline   Reply With Quote

Old   November 3, 2014, 06:18
Default
  #14
Senior Member
 
Gweher's Avatar
 
Gwenael H.
Join Date: Mar 2011
Location: Switzerland
Posts: 392
Rep Power: 20
Gweher will become famous soon enough
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).
Attached Images
File Type: jpg Interface_Mesh_Issue.jpg (70.0 KB, 173 views)
File Type: jpg Interface_Mesh_Issue_Part.jpg (77.8 KB, 169 views)
Gweher is offline   Reply With Quote

Old   November 3, 2014, 06:20
Default
  #15
Senior Member
 
Gweher's Avatar
 
Gwenael H.
Join Date: Mar 2011
Location: Switzerland
Posts: 392
Rep Power: 20
Gweher will become famous soon enough
Quote:
Originally Posted by reza67 View Post
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.
Gweher is offline   Reply With Quote

Old   November 3, 2014, 12:12
Default
  #16
New Member
 
Farzad Montazery
Join Date: Oct 2014
Location: Iran, Tabriz
Posts: 21
Rep Power: 11
famon is on a distinguished road
Thanks for useful guides, I loved the method
famon is offline   Reply With Quote

Old   November 3, 2014, 14:43
Default
  #17
New Member
 
Farzad Montazery
Join Date: Oct 2014
Location: Iran, Tabriz
Posts: 21
Rep Power: 11
famon is on a distinguished road
Quote:
Originally Posted by amin.z View Post
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
famon is offline   Reply With Quote

Old   November 3, 2014, 17:23
Default
  #18
Senior Member
 
Join Date: Mar 2014
Posts: 375
Rep Power: 13
hwet is on a distinguished road
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
Attached Images
File Type: jpg sweep.jpg (15.1 KB, 88 views)

Last edited by hwet; November 3, 2014 at 19:39. Reason: attachement
hwet is offline   Reply With Quote

Old   November 18, 2014, 03:46
Default
  #19
Senior Member
 
amin.z's Avatar
 
Amin
Join Date: Oct 2013
Location: Germany
Posts: 397
Rep Power: 14
amin.z is on a distinguished road
Quote:
Originally Posted by Gweher View Post
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...
amin.z is offline   Reply With Quote

Old   May 23, 2016, 19:29
Default
  #20
New Member
 
Awais
Join Date: Mar 2016
Posts: 15
Rep Power: 10
ayousaf is on a distinguished road
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

Last edited by ayousaf; May 23, 2016 at 22:31.
ayousaf is offline   Reply With Quote

Reply

Thread Tools Search this Thread
Search this Thread:

Advanced Search
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are Off
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
[ICEM] Simple pipe meshing - problems with y+ in CFX Keizers ANSYS Meshing & Geometry 23 January 15, 2015 08:00
[Workbench] Meshing for perforated pipe buried in porous zone Tanjina ANSYS Meshing & Geometry 0 September 24, 2014 09:41
Using ICEM CFD to repair/edit ANSYS Meshing Kaaji1359 ANSYS 2 July 30, 2013 10:28
[ANSYS Meshing] Migrating from GAMBIT to ANSYS Meshing David-CFD ANSYS Meshing & Geometry 1 April 1, 2011 05:22
[ANSYS Meshing] Ansys meshing with extended meshing jsm ANSYS Meshing & Geometry 6 January 10, 2011 12:09


All times are GMT -4. The time now is 06:03.