# In CFX workbench, which surface, i have to select

 User Name Remember Me Password
 Register Blogs Members List Search Today's Posts Mark Forums Read

 May 28, 2010, 11:59 In CFX workbench, which surface, i have to select #1 New Member   sendhil Join Date: May 2010 Posts: 11 Rep Power: 14 Dear CFX user, I am using ANSYS CFX workbench. I am trying to find surface temperature for a given value of heat flux. The structure of the problem is explained below. “Consider a square of 3 cm x3 cm. Divide the square into three rows and three columns. The width of the each cell is 1 cm”. From the bottom of the square, I want to give heat flux value in between the cells (1, 1) and (2, 1). The heater is placed at the top of the first cell. Like that, I want to give heat flux value at the interface of (1, 2) and (2, 2). Similarly at (1, 3) and (2, 3). While selecting the surface in the workbench before meshing, it shows two surfaces at the lower left corner of the window. Which surface, I should select? If I select upper surface to give the heat flux, the other surface automatically takes adiabatic boundary condition. And vice versa is happening, if I select lower surface. Or Should I give same heat flux value on both surfaces? Or Half value of the heat flux, should I give on both surfaces? If anyone comes across such problem, please clarify me. Thanks, SEN

 May 28, 2010, 13:17 #2 New Member   Jordi Join Date: May 2010 Posts: 26 Rep Power: 14 If you could link a picture it would be much clearer... First, you start with a square (a surface) with cells, then the inteface between them should be lines, not surfaces, unless what you mean is a cross section of a prism. Second, as far as I know, you can specify boundary conditions (temp, heat flow, adiabatic wall, etc.) at the boundaries, not between cells of continuous medium. When you need to select for a body, surface, line or point, check first the buttons in the tool bar and the icon next to the pointer, to select what you want. Whenever you click and select an item, the closest one is selected, but you have the possibility of selecting 'hidden' items behind by clicking or CTRL+Click on the parallel small planes at the lower left corner of the screen. It is sometimes useful, to select and click 'hide faces' for the items behind to be accesible.

May 28, 2010, 14:39
#3
New Member

sendhil
Join Date: May 2010
Posts: 11
Rep Power: 14
Hai Jordi,

Here I attached image related to my exact geometry. It consists of different solids domain. I put black circle to mark the heat flux value , where i want to give.

In the left corner of the screen, i marked black line to the two surfaces indication.

Please clarify me which surface, i should select for giving heat flux value.
Attached Images
 CFX.JPG (14.8 KB, 52 views)

May 28, 2010, 16:12
#4
New Member

Jordi
Join Date: May 2010
Posts: 26
Rep Power: 14
First, I suppose any of these bodies would be a fluid (gas or liquid), otherwise (all solids) I would use ANSYS for thermal simulation.
If you create different domains, each has their own boundaries, every interface is made of two boundaries in contact. You have to create 'domain interface' and tell what faces are connected (I use to write down the face's numbers of each domain, like F86.121 for example)

[IMG]file:///C:/CFX.jpg[/IMG]

I created this simplified test, it's a box (1x1x1 m) with a rectangular bar in the center. There are 2 domains. I created 2 domain interfaces: Interface 1 links the upper face of the bar to the outside domain. Interface 2 links the other 3 faces (sides and bottom) of the bar to the outside body. A thermal resistance of 0 is defined.

Then a surface heat source is defined for interface 1, but in the domain faces (there are 2). For the interface 1 side 1 (outer body) I defined a heat flow of 1e4 W/m2 and -1e4 W/m2 for the corresponding side of inner bar.

These interface sides are automatically created when you define a domain interface.

Other faces are in the default state (adiabatic wall)

The result (temperature) is shown. Heat flow from the upper face of the bar to the outer body and reflows back. It's like an electric circuit with a current source.

I think this is the point you need: defining domain interfaces and heat flows for each pair of faces in contact (+ is heat in and - is heat out)
Attached Images
 CFX.jpg (17.0 KB, 25 views)

May 29, 2010, 08:21
#5
Super Moderator

Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,321
Rep Power: 138
Quote:
 I would use ANSYS for thermal simulation.
If you are referring to ANSYS Mechanical then this sounds like a bad idea. CFX can run thermal stuff just fine, so forget about ANSYS Mech - especially on this forum, we are CFX fans here!

Jordi - you seem to have fundamentally misunderstood how CHT modelling is done. Why specify a + and - heat source at the interface? This is not physically real. If there is some external heating (maybe radiative or electrical heating) then just apply the single heat source. The coupling between the two domains and the +/- components which this creates is all taken care of in the interface boundary.

 May 29, 2010, 08:31 #6 New Member   Jordi Join Date: May 2010 Posts: 26 Rep Power: 14 If there are two faces in close contact, the heat received by one of them is given by the other, that's the reason. But I agree it's simpler and physically closer to reality to set up just one heat flux and a domain interface with proper thermal resistance. Probably, by setting these + and - heat flows i'm actually doubling it.

May 29, 2010, 18:54
#7
Super Moderator

Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,321
Rep Power: 138
Quote:
 by setting these + and - heat flows i'm actually doubling it.
Precisely. So don't do it, it is wrong.

If there is a thermal resistance then put it in as a thermal resistance on the surface. CFX V12 supports thermal resistances on interfaces.

 June 2, 2010, 09:26 Dear CFX uSER, #8 New Member   sendhil Join Date: May 2010 Posts: 11 Rep Power: 14 hI Ghorrocks, Thanks your reply, I am using ANSYS 11, Can i include Thermal resistance in the ANSYS 11?

 June 2, 2010, 09:34 #9 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,321 Rep Power: 138 Not easily, best option is to model in a thin layer and give it a thermal conductivity designed to give the right thermal resistance. It is quite easy in V12 and does not require additional mesh so a good excuse to upgrade to the latest version.

 June 2, 2010, 10:16 #10 New Member   sendhil Join Date: May 2010 Posts: 11 Rep Power: 14 Dear Ghorrocks, We tried V12 to install in our machine, we could not able to do. So we started using V11. Can u tell me procedure how to do thin layer with mesh in between the two surfaces in V11.? or except V12, iS THERE any other way to solve this kind of problem?

 June 2, 2010, 19:33 #11 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,321 Rep Power: 138 As I said, the easiest way is to insert a thin layer of mesh and define it as a solid body, with a thermal conductivity chosen to give the right resistance for the thickness.

 June 3, 2010, 06:24 #12 New Member   sendhil Join Date: May 2010 Posts: 11 Rep Power: 14 Dear Ghorrocks, Thanks for your suggestion.

 December 17, 2011, 03:44 Please Help me #13 New Member   Unuruu Join Date: Dec 2011 Posts: 4 Rep Power: 13 Dear all CDX experts I am trying to simulate temp analysis inside the weighing chamber. Suppose there is mass measurement using very precise balance which is inside the glass chamber. weight temp assumed always bigger than fluid temperature. I use ANSYS13.0 CFX, but I didn;t know how to set boundary cond. there should be 2inlet from 2 sides and 1 outlet at top of box. should I insert fuid/solid interface or thin layer mesh? If I should How all these thns done ? Pls, help me it is very urgent to compete my FEM course next week PLease I begging all of you

 December 17, 2011, 06:31 #14 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,321 Rep Power: 138 What are you trying to achieve with your model? I do not understand what you are trying to do.

December 17, 2011, 20:45
#15
New Member

Unuruu
Join Date: Dec 2011
Posts: 4
Rep Power: 13
Thanks u very much for reply.
My goal is to evaluate the effect of convective force on standard weight.
So I put hot cylindrical weight inside the weighing chamber/ box/ want to see
temp and velocity distribution around the surface of cyl weight.
I just tried to follow heatingcoil tutorial example. but I am confused to create domain and domain interface and set boundary cond.

I attached my result in txt. file.
Please explain there is some notice.
Thanks very mush
Attached Files
 weight2.txt (58.3 KB, 4 views)

 December 18, 2011, 06:19 #16 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,321 Rep Power: 138 Can you post an image? What do you mean by the "convective force"? The convection on the body is going to result in a microscopic force on the bodies weight. This would only be of interest to extremely high precision weight measurements. If this is so, why are you doing such a precision weight measurement? Some other comments - you have the flow set to laminar. Do you know it is laminar? How have you checked? Also you have lots of back flow at your outlet. This usually means your outlet is too close and needs to be moved further away.

December 18, 2011, 08:10
#17
New Member

Unuruu
Join Date: Dec 2011
Posts: 4
Rep Power: 13
Vertical drag force/ same as convective/ prodused a change in measurement of mass which is given by m= -F/g , because of temp change around surface of weight we have to consider velocity and temp. boundary layer around surface of weight on which I want to calculate Navier Stokes equation. Env.condition is well controlled so assume air is laminar. Newtonian, imcompressible, steady state.
Actually i don't know how to create this thin boundary layer around surface of weight and make mesh and apply bound.cond.
I attach my geometry.
Thanks for helping me.
Attached Images
 Figure001.jpg (45.8 KB, 12 views)

December 18, 2011, 17:50
#18
Super Moderator

Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,321
Rep Power: 138
Quote:
 Env.condition is well controlled so assume air is laminar.
How well controlled it is has nothing to do with laminar or turbulent. It is quite possible the convective plume coming off the body trips to turbulent flow. Have you calculated the Rayliegh number on the body?

Quote:
 Actually i don't know how to create this thin boundary layer around surface of weight
If you have set up a simulation where a boundary layer will form then it will form as a result of the simulation. You do not "create" it.

You still have not explained what you are trying to do. Are you doing precision measurements of the weight of this body? Why? Why is it hot? Please explain what you are trying to do.

 December 18, 2011, 22:14 #19 New Member   Unuruu Join Date: Dec 2011 Posts: 4 Rep Power: 13 Yes, in mass measurement this convective effect due to the temp. gradient is one effect which should include in uncertainty account. In order to intensify this effec,t body is pre-heated and loaded on the balance. How I set up a boundary layer that is very close to surface of body /during mesh / or during CFX-pre setup process/ ? Thanks for reply. Unuruu

 December 19, 2011, 02:31 #20 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,321 Rep Power: 138 The temperature gradient does not cause the mass error. It would be shear of the flow rising from the body. If you stop the flow you should stop the mass error. You do not set up boundary layers in simulation. You prescribe a flow and the boundary layer forms as a result of the simulation.

 Thread Tools Search this Thread Search this Thread: Advanced Search Display Modes Linear Mode

 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 OffTrackbacks are Off Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post justincase ANSYS Meshing & Geometry 4 February 24, 2020 04:22 MiXaNiK CFX 0 May 29, 2009 09:33 venugopal FLUENT 0 September 18, 2004 10:47 Alan CFX 7 June 5, 2003 13:19 Michael Rasmussen CFX 3 October 5, 2001 14:24

All times are GMT -4. The time now is 03:12.

 Contact Us - CFD Online - Privacy Statement - Top