CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   ANSYS Meshing & Geometry (http://www.cfd-online.com/Forums/ansys-meshing/)
-   -   [ICEM] Solid wall meshing in T junction (http://www.cfd-online.com/Forums/ansys-meshing/111240-solid-wall-meshing-t-junction.html)

selvam2487 January 1, 2013 04:45

Solid wall meshing in T junction
 
1 Attachment(s)
Hello Friends,

I am currently working on fluid flows in T junction piping system. I wanted to create mesh for the solid piping part along with the fluid part inside the pipe. Can someone suggest me a blocking strategy for doing this? I have attached a picture of the T junction pipe along with this post for your reference. Thank you.

Far January 1, 2013 08:22

Draw ogrid for thickness

selvam2487 January 1, 2013 09:40

Solid pipe blocking
 
Hello Far,

You mean two O grids (one for the fluid domain and one for the solid domain)? If my understanding is wrong, kindly correct me. It would be more understandable for me if you could attach some pictures.
Also, I would like to thank you for your suggestions about meshing in a T junction pipe in my previous posts. Based on your suggestion, I am able to create a mesh with an angle of 41° and a quality of 0.62. Now I am trying to create a complete meshing of solid pipe with fluid flow inside it, which is what my work is all about.

Far January 1, 2013 09:48

If you can attach .tin I will try

selvam2487 January 1, 2013 15:39

tin file for T junction with a thickness
 
1 Attachment(s)
Hello Far,

I am attaching the tin file along with this post. Kindly have a look at it. Once again thank you very much for your help.

energy382 January 2, 2013 05:08

Why do you want to model the solid part as well? Is there any heat transfer?

If so (and if it's a thin surface), you can do it with a another, more accurate approach.

selvam2487 January 2, 2013 05:12

Solid pipe and fluid blocking
 
Yes, there is a conjugate heat transfer between the pipe and the fluid near the wall. Because of the temperature fluctuations occurring near the solid wall, the pipe fails after certain thousand hours of operation which is generally called thermal fatigue. So I am interested in modeling both fluid and solid parts. Could you kindly help me as to how to do it? Thank you very much in advance for your help.

P.S: The thickness of the cold fluid pipe (branch pipe) is 1.1 mm while the thickness of the hot fluid pipe (main pipe) is 8.2 mm

energy382 January 2, 2013 05:26

Ok, that's an easy one. I'll take a look on it as soon as I'm back in office. Any blocking so far?!

selvam2487 January 2, 2013 05:32

T junction with a thickness
 
No. I have done blocking for T junction with only fluid flow (i.e., no thickness in the pipe walls). For T junctions with wall thickness, I do not know how to implement a blocking strategy. I have attached the ANSYS ICEM file in the present thread when replying to another member in this forum.

energy382 January 2, 2013 07:09

1 Attachment(s)
your geometry is not closed at t-junction. Blank part T_P and you'll see it. Please confirm.

selvam2487 January 2, 2013 08:13

T junction with a thickness
 
1 Attachment(s)
Hello,

Thank you very much for pointing out the mistake in the geometry. I think I have corrected it and I am attaching it along with this post. Kindly have a look at it and let me know if it is ok.

energy382 January 2, 2013 10:22

1 Attachment(s)
I've attached the mesh.

You've to adjust edge paramters (especially within boundary layer => y+ should be < 1 for heat transfer )

Regards,
Christoph

selvam2487 January 3, 2013 05:14

Dear Christoph,

Thank you very much for your help. I am currently working on the mesh you sent me. It is simple and understandable.

Regards,
Karthick

selvam2487 January 3, 2013 09:10

Dear Christoph,

I have a doubt regarding a part that you have created. What does the part T_P mean? I see it on the outer surface of the cold pipe. Also, how did you do the blocking for the solid and fluid part. I think you applied three blockings (two for solid outer wall and inner wall) and one for the fluid domain along with the O grid. I tried it and it is showing me the option of merging or replacing the earlier blocking that I had done. Could you please explain me how to do the blocking strategy you have implemented?

Far January 3, 2013 10:13

1 Attachment(s)
Please find the blocking attached herewith.

I have done some more steps as compared to previous only fluid blocking

1. Made two o-grid instead of one

2. Solid blocks were defined

3. Associated edges to curves. special care was taken at the junction

4. Shared wall between solid and fluid (inner pipe)

5. Due to problems in meshing, i have manually associated the outer pipe faces to corresponding surface(s).


Hier findest du die hiermit Sperrung angebracht.;)

Ich habe einige weitere Schritte getan, um vorhergehende nur Fluidsperrvorrichtung Vergleich

Ein. Hergestellt zwei o-Grid statt einer

2. Feste Blöcke definiert wurden

3. Zugeordneten Kanten in Kurven. Besondere Sorgfalt wurde an der Kreuzung getroffen

4. Gemeinsame Wand zwischen festen und flüssigen (Innenrohr)

5. Aufgrund von Problemen in kämmendem haben i manuell die Außenrohr Gesichter zu entsprechenden Oberfläche (n) zugeordnet ist.

Mit freundlichen Grüßen
Far (Nicht zu weit)

Far January 3, 2013 10:35

I am curious to see that how you will handle the solid part in CFD solver !!!

energy382 January 3, 2013 10:43

Quote:

Originally Posted by selvam2487 (Post 399923)
Dear Christoph,

I have a doubt regarding a part that you have created. What does the part T_P mean? I see it on the outer surface of the cold pipe. Also, how did you do the blocking for the solid and fluid part. I think you applied three blockings (two for solid outer wall and inner wall) and one for the fluid domain along with the O grid. I tried it and it is showing me the option of merging or replacing the earlier blocking that I had done. Could you please explain me how to do the blocking strategy you have implemented?

Du kannst es auf zwei Arten machen:

1. du machst ein O-grid für das Fluid und machst dann nochmal ein O-grid, wobei du hier dann "arround blocking" "abstand=1" und "absolut" wählst. Dann hast du zwei verschachtelte O-grids. Das Äußere weist du dann dem Part "SOLID" zu, das innere O-grid dem Part "FLUID".
Dazu einfach Part-Create New Part-"SOLID"-und dann die Blöcke des äußeren O-grids diesem Part zuweisen.
Dann nur noch die Kanten mit den Kurven verbinden (oder face to surface falls das Netz nicht richtig projeziert wird).

2. du machst zwei getrennte Blockings. Ein 3D-Blocking FLUID und eins fürs SOLID. Dann musst du diese allerdings an den Blockgrenzen verbinden (merge nodes).

Die elegantere Methode ist sicher die Erste, aber die Zweite ist vielleicht etwas übersichtlicher.

Das Netz kannst du dann ja über die Kantenparameter steuern. Du solltest max. grow ratio von 1,2 wählen und auf dein y+ Werte achten. Bei Wärmeübergängen etc. sollten diese nahe an 1 liegen, damit auch die viskose Unterschicht der Grenzschicht aufgelöst wird. Wandfunktionen liefern hier falsche Ergebnisse. Als Turbulenzmodel SST.

Melde dich, falls noch Fragen offen sind zum Thema Vernetzung und/oder Preprocessing

Gruß Christoph


All times are GMT -4. The time now is 10:24.