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

Inject flow by nodes

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

Reply
 
LinkBack Thread Tools Display Modes
Old   January 14, 2010, 08:19
Exclamation Inject flow by nodes
  #1
New Member
 
Carlos
Join Date: Oct 2009
Posts: 18
Rep Power: 7
Carlitos is on a distinguished road
Hi everybody,

I'm trying to simulate a kind of mixing vessel and i have to inject a fluid inside the vessel. The problem is how to modelate or create that inlet. Is it possible to indicate to a group of nodes a mass-flow or you must have a 2d region in order to create a boundary condition?. I've created a solid inside the vessel to inject there the flow but it doesnīt work, there isn`t interaction between the vessel and the nozzle.

What do you suggest to me?

Thank you in advance

Carlitos
Carlitos is offline   Reply With Quote

Old   January 14, 2010, 13:10
Default
  #2
Senior Member
 
Join Date: Apr 2009
Posts: 516
Rep Power: 12
stumpy is on a distinguished road
If you are ignoring the details of the injection geometry, then add a continuity source term to a subdomain, where the subdomain is scoped to your solid inside the vessel.
stumpy is offline   Reply With Quote

Old   January 14, 2010, 15:07
Exclamation
  #3
New Member
 
Carlos
Join Date: Oct 2009
Posts: 18
Rep Power: 7
Carlitos is on a distinguished road
Thank you for reply stumpy, but could you explain a little more please?.

You advise me to create a subdomain with a continuity total source but then, i have to put a boundary condition, type inlet, in one side of the domain in order to get a flow? or it's enough with the total source?

Thanks in advance

Carlitos
Carlitos is offline   Reply With Quote

Old   January 14, 2010, 15:49
Default
  #4
Senior Member
 
Join Date: Apr 2009
Posts: 516
Rep Power: 12
stumpy is on a distinguished road
If you add a continuity source to a subdomain, then some mass flux of fluid is introduced evenly over the entire subdomain volume. So there's no boundary condition to define, but you do have to define the properties at which the fluid is introduced (temperature, turbulence, velocity etc). If this isn't a suitable approach then yes, you do need a 2d region to define a boundary condition and it must be an external 2d region.
stumpy is offline   Reply With Quote

Old   January 18, 2010, 07:02
Default
  #5
New Member
 
Carlos
Join Date: Oct 2009
Posts: 18
Rep Power: 7
Carlitos is on a distinguished road
Dear stumpy,

First at all, thanks for reply.

These days I've tried to create a subdomain with a source term but it doesn' work: i didnīt manage at injecting external flow inside the vessel. In order to overcome the problem i've created some source points which seem to work but i canīt understand the following: when i define the source point i must specify a total source mass flow (kg/s) and a velocity (m/s), so with these two values ANSYS is capable of calculate an area for that point?. Why is it necessary to give two values instead of one if it is only a point?

And i have another question. I realise when you define a boundary condition you can also specify a source term. I`ve tried to create a 2D region inside the vessel and define it as an outlet with a source term but it doesn`t work. Could you help me with the source terms, please?

Thank you in advance

Carlitos
Carlitos is offline   Reply With Quote

Old   January 18, 2010, 12:13
Default
  #6
Senior Member
 
Join Date: Apr 2009
Posts: 516
Rep Power: 12
stumpy is on a distinguished road
Source points, boundary sources and subdomain sources are really all the same. There are all actually 3D sources. For a source point the source is introduced in the element in which the point lies. For boundary sources the elements touching the boundary are used. For subdomains all the elements in the subdomain are used. In all cases a mass flow will be needed. For the source point you provide the mass flow that is introduced in that element - so you you have introduced some mass - but at what velocity is that mass introduced? Does it just appear with no initial momentum, or is it shooting into the domain? Hence you need to specify the velocity.
stumpy is offline   Reply With Quote

Old   January 19, 2010, 05:09
Default
  #7
New Member
 
Carlos
Join Date: Oct 2009
Posts: 18
Rep Power: 7
Carlitos is on a distinguished road
Thank you stumpy for the explanation.

Now itīs clear source points, but just the last question about this issue. If i've understood correctly you can create a subdomain, define their sides as wall boundary condition type and then include a source term in one of those sides. Thus it's possible to create a particular geometry for the nozzle inside the vessel. what do you think about this?

Regards

Carlitos
Carlitos is offline   Reply With Quote

Old   January 20, 2010, 23:08
Default
  #8
Senior Member
 
Join Date: Apr 2009
Posts: 516
Rep Power: 12
stumpy is on a distinguished road
Those are two separate things. The only reason to create the subdomain is to add a volumetric source over the entire subdomain. If you want internal wall BC's then these would be thin surfaces, then you can add a source to those walls, but no need for a subdomain (but your geometry/mesh would need to be created with this in mind so that you have internal 2D mesh regions).
stumpy is offline   Reply With Quote

Old   January 23, 2010, 08:23
Default
  #9
New Member
 
Carlos
Join Date: Oct 2009
Posts: 18
Rep Power: 7
Carlitos is on a distinguished road
Thanks Stumpy.

Now the idea of creating a subdomain is clear. I also understand the idea of wall BC`s as thin surfaces but what i can't really now understand, it's the following question: when you define a 2d region as an inlet you may include a source term but why?, i mean, in which case is necessary a source term instead of using a single inlet bc's?. you can create an inlet with a mixing of several materials and every material will have its own properties and initial conditions.which advantages or disadvantages have every option?.

Sorry for being a pain in the neck, but for me this issue have a lot of food for thought.

Carlitos
Carlitos is offline   Reply With Quote

Reply

Thread Tools
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 On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Flow meter Design CD adapco Group Marketing CD-adapco 3 June 21, 2011 08:33
mass flow in is not equal to mass flow out saii CFX 2 September 18, 2009 08:07
What is the difference between liquid reactive flow and gas reactive flow? James Main CFD Forum 6 May 15, 2009 12:14
reversed flow at velocity inlet / mass flow inlet ib FLUENT 1 March 26, 2007 13:11
potential flow vs. Euler flow curious ... Main CFD Forum 23 July 21, 2006 07:40


All times are GMT -4. The time now is 18:39.