CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > Siemens > STAR-CCM+

temperature correction limited- Star ccm+

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

Like Tree1Likes
  • 1 Post By ping

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   August 26, 2020, 15:13
Default temperature correction limited- Star ccm+
  #1
New Member
 
Lovepreet Singh
Join Date: Aug 2020
Posts: 15
Rep Power: 4
LpSingh is on a distinguished road
Hello everyone,
I'm trying to simulate the flow of R12 in a pipe 5 meters long and heated for a length of 3.5 meters. The heating occurs after 1 m of the pipe and ends at 4.5 m so I have divided the pipe in 3 regions with the central region heated by outside. Now, while the simulation is going I have these messages:
Temperature corrections limited on 15 cells in fluid 1
Minimum Temperature limited to 100 on 12 cells in fluid 1
I have tried to refine the mesh but I cannot get ta better result.
I have attached two screenshots about these messages and the residuals.
Thanks in advance.
L. Singh
Attached Images
File Type: jpg message 1.JPG (127.1 KB, 38 views)
File Type: jpg residuals.jpg (74.3 KB, 33 views)
LpSingh is offline   Reply With Quote

Old   September 4, 2020, 06:14
Default
  #2
Senior Member
 
Ping
Join Date: Mar 2009
Posts: 556
Rep Power: 18
ping is on a distinguished road
do some tests on simplified versions:
does it run well when temperature/energy is removed from the physics?
then add temperature in again but with no heating applied.
add a very small amount of heat
etc
LpSingh likes this.
ping is offline   Reply With Quote

Old   September 5, 2020, 05:32
Default
  #3
New Member
 
Lovepreet Singh
Join Date: Aug 2020
Posts: 15
Rep Power: 4
LpSingh is on a distinguished road
Quote:
Originally Posted by ping View Post
do some tests on simplified versions:
does it run well when temperature/energy is removed from the physics?
then add temperature in again but with no heating applied.
add a very small amount of heat
etc
Thanks for your reply.
I tried to run it with no energy equations and the residuals are just fine as the residuals on the continuity, X-momentum and Y-momentum are only 10^-2. (Screenshot attached)
Then I simulated the adiabatic case and even this time I have the same two errors. In particular, I have observed that the bounary heat flux at the pipe entrance has an abnormal behavior along with having the hot zones. I am not able to solve these issues.
Attached Images
File Type: jpg Residuals no energy.jpg (71.0 KB, 16 views)
File Type: jpg Residuals adiabatic.JPG (97.5 KB, 15 views)
File Type: jpg T adiabatic.JPG (37.5 KB, 19 views)
File Type: jpg BHF adiabatic.jpg (47.3 KB, 13 views)
LpSingh is offline   Reply With Quote

Old   September 6, 2020, 03:57
Default
  #4
Senior Member
 
Ping
Join Date: Mar 2009
Posts: 556
Rep Power: 18
ping is on a distinguished road
firstly i notice you might have a solid pipe in your setup and wonder if this is really needed since it is rare to need to add the actual solid and you can instead accurately allow for it in the wall boundary settings including thermal resistance. solids slow the solution especially if the energy u.r.f. is not set very close to 1 ie 0.99999. i doubt this is you problem but it might be causing slow convergence and the temperature issue might go away after some time. so remove the physics from the solid and run again.
what does your mesh look like? hope your using a more efficient extruded meshing method to keep cell numbers down.
what are your boundary conditions?
ping is offline   Reply With Quote

Old   September 6, 2020, 05:43
Default
  #5
New Member
 
Lovepreet Singh
Join Date: Aug 2020
Posts: 15
Rep Power: 4
LpSingh is on a distinguished road
Quote:
Originally Posted by ping View Post
firstly i notice you might have a solid pipe in your setup and wonder if this is really needed since it is rare to need to add the actual solid and you can instead accurately allow for it in the wall boundary settings including thermal resistance. solids slow the solution especially if the energy u.r.f. is not set very close to 1 ie 0.99999. i doubt this is you problem but it might be causing slow convergence and the temperature issue might go away after some time. so remove the physics from the solid and run again.
what does your mesh look like? hope your using a more efficient extruded meshing method to keep cell numbers down.
what are your boundary conditions?
Actually for this project it is mandatory to use also the solid so we can't remove it.
I put here the screenshots about the mesh. The only problem I can identify in the mesh is the skewness angle for the rest the diagonistic report is fine.

The mesh is of directed type. For the solid part the mesh is a polygonal type and for the fluid I have used also the prism layers.
The boundary conditions for the pipe are:
pipe 1: the inlet of the pipe and the outer wall have boundary of type wall that are adiabtic; the inner wall is interfaced with the fluid wall with an interface of type contact interface and has a boundary of type wall which is adiabatic; the outlet of the pipe is interfaced with the inlet of pipe 2 with an interface of type contact interface and has a boundary of type wall which is adiabatic.
pipe 2 : the inlet of the pipe interfaced with the outlet of pipe 1 and have boundary of type wall that are adiabtic; the outer wall is heated with an imposed heat flux with a wall boundary type; the inner wall is interfaced with the fluid wall with an interface of type contact interface and has boundary of type wall that is adiabtic; the outlet of the pipe is interfaced with the inlet of pipe 3 with an interface of type contact interface and has boundary of type wall that is adiabtic.
pipe 3: the inlet of the pipe interfaced with the outlet of pipe 2 and has boundary of type wall that is adiabtic; the outer wall has a boundary type of wall which is adiabatic; the inner wall is interfaced with the fluid wall with an interface of type contact interface and has boundary of type wall that is adiabtic; the outlet of the pipe is again adiabatic of type wall.
fluid 1: the inlet of the fluid has an imposed mass flow rate; the wall is interfaced with the inner wall of pipe 1 and has a boundary of wall type which is adiabatic; the oulet is interfaced with the inlet of fluid 2 with an interface of type internal interface and has a boundary of symmetry plane type.
fluid 2: the inlet of the fluid has a boundary of symmetry plane type; the wall is interfaced with the inner wall of pipe 2 and has a boundary of wall type which is adiabatic; the oulet is interfaced with the inlet of fluid 3 with an interface of type internal interface and has a boundary of symmetry plane type.
fluid 3: the inlet of the fluid has a boundary of symmetry plane type; the wall is interfaced with the inner wall of pipe 3 and has a boundary of wall type which is adiabatic; the oulet has a boundary of outlet type.


I had to divide the 3 parts because only the pipe 2 is heated.
Attached Images
File Type: jpg mesh1.JPG (126.5 KB, 39 views)
File Type: jpg mesh2.JPG (107.2 KB, 30 views)
File Type: jpg mesh3.JPG (113.7 KB, 23 views)
LpSingh is offline   Reply With Quote

Old   September 6, 2020, 23:13
Default
  #6
Senior Member
 
Ping
Join Date: Mar 2009
Posts: 556
Rep Power: 18
ping is on a distinguished road
i worry about two aspects of your mesh - the poly mesh in the pipe is wrong since the gradients are all radial and so should be just 3-4 hexa layers using the thin mesher or you could use directed if you manually patch the annulus.

and it looks like you have a very fine prism layer and this can cause issues occasionally so i would be starting with a simple 2-3 layer wall function type prism layer rather than a low Rn prism layer and much coarser volume mesh to get the case working then think about refining the mesh.

did you try the case with the solid physics removed since this will also give you useful info about where the problems are?

silly to have the complication of 3 sections of pipe etc and if your interfaces are not perfect then you introduce problems. all you need is one fluid and one solid region and to have the central outer wall of the pipe as a separate wall boundary with its own conditions.

also have you considered doing it as a 2d axisymmetric case?
ping is offline   Reply With Quote

Old   September 16, 2020, 12:15
Default
  #7
New Member
 
Lovepreet Singh
Join Date: Aug 2020
Posts: 15
Rep Power: 4
LpSingh is on a distinguished road
Quote:
Originally Posted by ping View Post
i worry about two aspects of your mesh - the poly mesh in the pipe is wrong since the gradients are all radial and so should be just 3-4 hexa layers using the thin mesher or you could use directed if you manually patch the annulus.

and it looks like you have a very fine prism layer and this can cause issues occasionally so i would be starting with a simple 2-3 layer wall function type prism layer rather than a low Rn prism layer and much coarser volume mesh to get the case working then think about refining the mesh.

did you try the case with the solid physics removed since this will also give you useful info about where the problems are?

silly to have the complication of 3 sections of pipe etc and if your interfaces are not perfect then you introduce problems. all you need is one fluid and one solid region and to have the central outer wall of the pipe as a separate wall boundary with its own conditions.

also have you considered doing it as a 2d axisymmetric case?

Sorry for the late reply. I hope you still want to help me. First of all, I would like to work on your last comment about having only a one solid region and 1 fluid one but I don't know then how to specify the boundary conditions on the central part.
LpSingh is offline   Reply With Quote

Old   September 17, 2020, 03:20
Default
  #8
Senior Member
 
Ping
Join Date: Mar 2009
Posts: 556
Rep Power: 18
ping is on a distinguished road
i think you are referring to my second last comment and so all you need to do is divide the outer solid region wall into 3 sections - you can do this in your native cad software or in star's 3d-cad
- read this help Pre-Processing > Modeling Geometry > Using 3D-CAD > Working with Bodies > Imprinting Sketches onto Bodies
or in the surface repair tools in the parts area but this is hard work
ping is offline   Reply With Quote

Old   September 17, 2020, 12:42
Default
  #9
New Member
 
Lovepreet Singh
Join Date: Aug 2020
Posts: 15
Rep Power: 4
LpSingh is on a distinguished road
Quote:
Originally Posted by ping View Post
i think you are referring to my second last comment and so all you need to do is divide the outer solid region wall into 3 sections - you can do this in your native cad software or in star's 3d-cad
- read this help Pre-Processing > Modeling Geometry > Using 3D-CAD > Working with Bodies > Imprinting Sketches onto Bodies
or in the surface repair tools in the parts area but this is hard work
We have built our geometry using this function, like after creating the first section of the solid body we designed a sketch on its outlet then imprinted them while using Extrude.So the problem may not be here.
LpSingh is offline   Reply With Quote

Old   September 17, 2020, 12:45
Default
  #10
New Member
 
Lovepreet Singh
Join Date: Aug 2020
Posts: 15
Rep Power: 4
LpSingh is on a distinguished road
Quote:
Originally Posted by ping View Post
i worry about two aspects of your mesh - the poly mesh in the pipe is wrong since the gradients are all radial and so should be just 3-4 hexa layers using the thin mesher or you could use directed if you manually patch the annulus.
I apologize for asking you back to back explnations but can yo explain more widely this concept. I have tried to not use Polygonal mesh for the pipe but the other options are the triangular mesh and quadrilateral one that doesn't fit well.
LpSingh is offline   Reply With Quote

Old   September 18, 2020, 02:51
Default
  #11
Senior Member
 
Ping
Join Date: Mar 2009
Posts: 556
Rep Power: 18
ping is on a distinguished road
see help topics:
Pre-Processing > Meshing > Volume Meshers > Thin Mesher - the easier way
or
Pre-Processing > Meshing > Directed Meshing - quite a bit of learning involved
ping is offline   Reply With Quote

Old   September 18, 2020, 02:57
Default
  #12
Senior Member
 
Ping
Join Date: Mar 2009
Posts: 556
Rep Power: 18
ping is on a distinguished road
Quote:
Originally Posted by LpSingh View Post
We have built our geometry using this function, like after creating the first section of the solid body we designed a sketch on its outlet then imprinted them while using Extrude.So the problem may not be here.
this is the way that i would create this geometry and it will create 3 bodies and 3 sets of surface faces - one set for each body which can then be used as separate or combined boundaries later in parts and regions.

you can label the central outer surface with a name in 3d-cad and then ensure once you are in parts and create the region(s) that you keep the surfaces as separate boundaries - then you can place special physics properties on it.
ping is offline   Reply With Quote

Old   September 18, 2020, 15:56
Default
  #13
New Member
 
Lovepreet Singh
Join Date: Aug 2020
Posts: 15
Rep Power: 4
LpSingh is on a distinguished road
Quote:
Originally Posted by ping View Post
this is the way that i would create this geometry and it will create 3 bodies and 3 sets of surface faces - one set for each body which can then be used as separate or combined boundaries later in parts and regions.

you can label the central outer surface with a name in 3d-cad and then ensure once you are in parts and create the region(s) that you keep the surfaces as separate boundaries - then you can place special physics properties on it.
I tried to do it, but I don't know how to imprint on a cylindrical body. Like I followed the star ccm+ tutorial for the rectangular body and I was able to complete it because I was able to design a sketch on a face of the body, but having a cylinder body I can design a sketch only at the inlet and outlet and this would become the case of my current configuration.
LpSingh is offline   Reply With Quote

Old   September 19, 2020, 02:41
Default
  #14
Senior Member
 
Ping
Join Date: Mar 2009
Posts: 556
Rep Power: 18
ping is on a distinguished road
if you understood my previous answer you don't need to imprint because the separate faces already exist due to the way you contructed your cad
ping is offline   Reply With Quote

Old   September 29, 2020, 11:59
Default
  #15
New Member
 
Lovepreet Singh
Join Date: Aug 2020
Posts: 15
Rep Power: 4
LpSingh is on a distinguished road
Quote:
Originally Posted by ping View Post

did you try the case with the solid physics removed since this will also give you useful info about where the problems are?
We tried this case now. We have done 700 iterations and there are some problems related to the velocity and themperature. I put the shots below.
Attached Images
File Type: jpg error.JPG (27.6 KB, 16 views)
File Type: jpg error 1.JPG (24.9 KB, 11 views)
LpSingh is offline   Reply With Quote

Old   September 29, 2020, 12:06
Default
  #16
New Member
 
Lovepreet Singh
Join Date: Aug 2020
Posts: 15
Rep Power: 4
LpSingh is on a distinguished road
Also the skewness angle shows a strange behavior.
Attached Images
File Type: jpg error 2.jpg (23.6 KB, 12 views)
LpSingh 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
temperature correction limited- Star ccm+ LpSingh Main CFD Forum 4 August 30, 2020 05:40
limited temperature in X cells Bücherknopf STAR-CCM+ 3 June 27, 2016 02:29
Change the Mass flux formulation in Star ccm Xuekun STAR-CCM+ 0 January 24, 2016 09:14
importing ducted fan from catia to star ccm Daniel4 STAR-CCM+ 0 November 3, 2014 10:34
error in star ccm maurizio Siemens 3 October 16, 2007 06:17


All times are GMT -4. The time now is 07:04.