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

Heat transfer and insulated walls

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

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   January 30, 2020, 02:38
Default Heat transfer and insulated walls
  #1
New Member
 
Join Date: Aug 2019
Posts: 5
Rep Power: 6
cos2pi is on a distinguished road
Hey

I'm trying to make a calculation of heat loss from a certain geometry. Parts of my geometry is insulated and the rest is steel.

I can't figure out if what I have done is correct, since my results are so non consistent.

On the curved surface (part of a cylinder) i have a flow flowing with a certain temperature (390 deg C) and through convection heating up my geometry.

I have put this in by convection film coefficient of 200 and the temperature.

Further I have drawn the free stream air which cools my geometry by convection and radiation (haven't put in radiation - wont work).

Inlet conditions 20 deg C and 1 m/s, pressure outlet.

I have attached a photo. https://imgur.com/a/AW0nKZP
cos2pi is offline   Reply With Quote

Old   January 30, 2020, 03:37
Default The issue?
  #2
Senior Member
 
vinerm's Avatar
 
Vinerm
Join Date: Jun 2009
Location: Nederland
Posts: 2,946
Blog Entries: 1
Rep Power: 36
vinerm will become famous soon enough
Hi

You have mentioned that the results are not consistent. But that doesn't explain much about the problem you are facing except that you are not getting good outcome. Could you please be more elaborate?
__________________
Regards,
Vinerm

PM to be used if and only if you do not want something to be shared publicly. PM is considered to be of the least priority.
vinerm is offline   Reply With Quote

Old   January 30, 2020, 03:55
Default
  #3
New Member
 
Join Date: Aug 2019
Posts: 5
Rep Power: 6
cos2pi is on a distinguished road
Firstly my model doesn't converge.

And I don't seem to have the heat transfer that I expected.

I have a lot of heat going into the system, but I'm not sure if it gets "lost" from the curved face or the rest where it would by in real life.

https://imgur.com/a/tjkO6RE
cos2pi is offline   Reply With Quote

Old   January 30, 2020, 09:14
Default Flow description
  #4
Senior Member
 
vinerm's Avatar
 
Vinerm
Join Date: Jun 2009
Location: Nederland
Posts: 2,946
Blog Entries: 1
Rep Power: 36
vinerm will become famous soon enough
If I rephrase the scenario, it is like this

1. You have a solid object that has heat coming in from a certain surface or a group of surfaces where you have applied HTC and T
2. There is a fluid zone around it where you are simulating the flow, which is supposed to cool it.

Am I right about the above two statements? If not, no need to read further and provide more clarity. If yes, then please check the following

How are solid and fluid cell zones connected? Is it a conformal mesh or non-conformal one with interface(s)? If it has interface(s), are they of coupled nature?
__________________
Regards,
Vinerm

PM to be used if and only if you do not want something to be shared publicly. PM is considered to be of the least priority.
vinerm is offline   Reply With Quote

Old   January 30, 2020, 09:39
Default
  #5
New Member
 
Join Date: Aug 2019
Posts: 5
Rep Power: 6
cos2pi is on a distinguished road
I have meshed it with ansys meshing - indeed the mesh could be better but looks somewhat okay.

For the interfaces I'm not really sure, it has been awhile since making CFD. I have posted some pictures

https://imgur.com/a/EfGbJcQ

https://imgur.com/a/atuVLdl
cos2pi is offline   Reply With Quote

Old   January 30, 2020, 10:04
Default Not good
  #6
Senior Member
 
vinerm's Avatar
 
Vinerm
Join Date: Jun 2009
Location: Nederland
Posts: 2,946
Blog Entries: 1
Rep Power: 36
vinerm will become famous soon enough
That's what I was worried about. You have interfaces that are not coupled. I would suggest going back to DM or SCDM or whichever modeling tool you use to ensure that all bodies belong to same assembly. If it is DM, then select all bodies and form a new part. If it is SpaceClaim, then go to Workbench tab in SpaceClaim and click on Share. This will ensure that at the Meshing stage there is only one assembly containing all bodies. Consequently, you will have conformal mesh and you would not have to worry about the interfaces, which in my view is very bad idea until and unless interface is the only solution, such as in moving mesh.

If you do not want to do that, then delete the interfaces and recreate them. While creating, ensure that coupled is selected and not mapped.
__________________
Regards,
Vinerm

PM to be used if and only if you do not want something to be shared publicly. PM is considered to be of the least priority.
vinerm is offline   Reply With Quote

Old   January 31, 2020, 09:18
Default
  #7
New Member
 
Join Date: Aug 2019
Posts: 5
Rep Power: 6
cos2pi is on a distinguished road
Hi

Thank you for using your time on my problem.

I have made the geometry one part, and imported again.

Should I do something to let the faces know that there is convection from them.
cos2pi is offline   Reply With Quote

Old   January 31, 2020, 09:30
Default Partial Overlap may exist
  #8
Senior Member
 
vinerm's Avatar
 
Vinerm
Join Date: Jun 2009
Location: Nederland
Posts: 2,946
Blog Entries: 1
Rep Power: 36
vinerm will become famous soon enough
Fluent will create solid-fluid or solid-solid coupled walls where the overlap exists. If there are portions of the boundary where overlap does not exist, those are treated as external walls. At those walls, you may apply a thermal boundary condition. Default, as you may know, would be adiabatic
__________________
Regards,
Vinerm

PM to be used if and only if you do not want something to be shared publicly. PM is considered to be of the least priority.
vinerm is offline   Reply With Quote

Reply

Tags
conduction, convection, heat losses

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
Insulated pipe heat transfer gundy STAR-CCM+ 3 May 12, 2014 21:41
Heat transfer in rooms: laminar or turbulent? ghost82 FLUENT 2 February 13, 2014 08:47
Pipe Flow Heat Transfer Saima CFX 5 January 30, 2011 16:41
Heat Transfer in a pipe flow(hot air) Saima Main CFD Forum 0 January 17, 2011 07:08
Modelling the heat transfer during compression and cooling of natural gas pano Main CFD Forum 0 December 10, 2010 15:53


All times are GMT -4. The time now is 00:12.