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

Mathematics of Source Points

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

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   December 20, 2019, 20:19
Default Mathematics of Source Points
  #1
New Member
 
DhyaniBaba
Join Date: Aug 2019
Posts: 7
Rep Power: 2
pdhyani96 is on a distinguished road
hello guys, I understand that a source point acts on a single mesh element and acts a 3D source. So, If i am modelling a jet of 2 (mm^2) and the area of mesh element at point source location is 0.5 (mm^2), does the jet come out of assumed area or the area of the mesh?

Because we are required to provide mass flow rate and an injection velocity. I assume the area is calculated from that reference. In most cases the area of injection is going to be more than the area of that mesh element. Then how does the software model such an area if injection come out of a single mesh element only?
pdhyani96 is offline   Reply With Quote

Old   December 21, 2019, 02:16
Default
  #2
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 16,263
Rep Power: 125
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
Source points act on a single element only, even if the size of the implied source is bigger than a single element.

It has been a while since I looked at source points, but I am surprised you can specify both mass flow and velocity. This appears to me to over-constrain the definition. Are you sure that is correct? I cannot check as I am not at work at the moment.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.
ghorrocks is offline   Reply With Quote

Old   December 21, 2019, 03:13
Default
  #3
New Member
 
DhyaniBaba
Join Date: Aug 2019
Posts: 7
Rep Power: 2
pdhyani96 is on a distinguished road
Yes, it does ask for velocity and mass flow rate. I had the same doubt. But my professor told me that a source point needs velocity and mass flow rate based on an area that a user assumes. But that idea didnít help me in simulations

I am supposed to inject uniform flow spanwise on an airfoil. For that I have made sure that source points occupy every mesh element along the span. But my simulations show four equidistant bumps at the location on jets instead of a uniform flow across the span.

Also, if I change the number of elements spanwise, the pattern changes. But I am not able to see a uniform injection.
pdhyani96 is offline   Reply With Quote

Old   December 30, 2019, 21:30
Default
  #4
Senior Member
 
Join Date: Jun 2009
Posts: 1,217
Rep Power: 24
Opaque will become famous soon enough
May I ask what are you trying to simulate?

Are you modeling injection points on the surface of the airfoil?, i.e. film cooling
Opaque is offline   Reply With Quote

Old   January 8, 2020, 07:29
Default
  #5
Member
 
Abdullah Arslan
Join Date: Apr 2019
Posts: 87
Rep Power: 3
Goenitz is on a distinguished road
So to calculate a source/flux if you have reaction rate like mol m^-2 s^-1.. Then if we multiply this to the area (wall) at which the reaction is taking place so it will become mol s^-1. So it is correct or depends upon the number of elements or element area(which should be equal to wall area)? My case is mesh independent.
Goenitz is offline   Reply With Quote

Old   January 8, 2020, 16:33
Default
  #6
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 16,263
Rep Power: 125
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
It all depends on whether your reaction is a point, surface or volume reaction.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.
ghorrocks is offline   Reply With Quote

Old   January 8, 2020, 21:54
Default
  #7
Senior Member
 
Join Date: Jun 2009
Posts: 1,217
Rep Power: 24
Opaque will become famous soon enough
Just for clarification,

For incoming flow, the velocity vector must be specified either directly or indirectly in several ways:

1 - Velocity Vector in any coordinate system
2 - Mass flow and flow direction
3 - Pressure of some kind and flow direction

The use of mass flow and velocity vector can be used, but (big one) the product of density * Velocity * Normal Area must be identical to the specified mass flow. Therefore, the velocity vector is implying the direction. Otherwise, there is an inconsistency between the two quantities.
Opaque is offline   Reply With Quote

Old   January 10, 2020, 18:24
Default
  #8
New Member
 
DhyaniBaba
Join Date: Aug 2019
Posts: 7
Rep Power: 2
pdhyani96 is on a distinguished road
Yes, I am trying to have injection points for film cooling on a blade surface.
pdhyani96 is offline   Reply With Quote

Old   January 10, 2020, 18:26
Default
  #9
New Member
 
DhyaniBaba
Join Date: Aug 2019
Posts: 7
Rep Power: 2
pdhyani96 is on a distinguished road
Quote:
Originally Posted by ghorrocks View Post
It all depends on whether your reaction is a point, surface or volume reaction.
It is point source. I don't think there is any surface or volume reaction involved
pdhyani96 is offline   Reply With Quote

Old   January 10, 2020, 18:31
Default
  #10
New Member
 
DhyaniBaba
Join Date: Aug 2019
Posts: 7
Rep Power: 2
pdhyani96 is on a distinguished road
Quote:
Originally Posted by Opaque View Post
Just for clarification,

For incoming flow, the velocity vector must be specified either directly or indirectly in several ways:

1 - Velocity Vector in any coordinate system
2 - Mass flow and flow direction
3 - Pressure of some kind and flow direction

The use of mass flow and velocity vector can be used, but (big one) the product of density * Velocity * Normal Area must be identical to the specified mass flow. Therefore, the velocity vector is implying the direction. Otherwise, there is an inconsistency between the two quantities.
I agree with the logic. But the software does not allow me to select the normal area. I am assuming that based on given mass flow rate and velocity of injection, the software assumes an area. Correct?

But if that is true, it goes against the manual which states that the injection comes of that specified mesh element.
pdhyani96 is offline   Reply With Quote

Old   January 19, 2020, 03:31
Default
  #11
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 16,263
Rep Power: 125
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
You have misunderstood the post. The normal area in Opaque's equation is not something you set, it is implicit in the element you define to have the source point. This means it is driven by the element's cross section area. It is not something the user sets directly.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.
ghorrocks is offline   Reply With Quote

Old   January 20, 2020, 16:41
Default
  #12
New Member
 
DhyaniBaba
Join Date: Aug 2019
Posts: 7
Rep Power: 2
pdhyani96 is on a distinguished road
Quote:
Originally Posted by ghorrocks View Post
You have misunderstood the post. The normal area in Opaque's equation is not something you set, it is implicit in the element you define to have the source point. This means it is driven by the element's cross section area. It is not something the user sets directly.
Okay, this clears most of the confusion. Mass flow is for defining strength, velocity is for defining direction. But all in all, the net mass flow rate should equal rho*area*velocity. Thank you guys! I really appreciate it.
pdhyani96 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
[snappyHexMesh] Invalid Normals for source face to target face while making AMI? Sorabh OpenFOAM Meshing & Mesh Conversion 0 November 21, 2019 23:58
[foam-extend.org] Problems installing foam-extend-4.0 on openSUSE 42.2 and Ubuntu 16.04 ordinary OpenFOAM Installation 19 September 3, 2019 18:13
[foam-extend.org] problem when installing foam-extend-1.6 Thomas pan OpenFOAM Installation 7 September 9, 2015 21:53
pisoFoam compiling error with OF 1.7.1 on MAC OSX Greg Givogue OpenFOAM Programming & Development 3 March 4, 2011 17:18
OpenFOAM on MinGW crosscompiler hosted on Linux allenzhao OpenFOAM Installation 127 January 30, 2009 19:08


All times are GMT -4. The time now is 12:44.