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

Inlet Velocity in CFX

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

Reply
 
LinkBack Thread Tools Display Modes
Old   August 5, 2009, 10:08
Default Inlet Velocity in CFX
  #1
New Member
 
Join Date: Jul 2009
Posts: 22
Rep Power: 8
aeroman is on a distinguished road


OK..I've been through the documentation and believe I have exhausted all other references and I have a question.

I am wanting to have an initial constant inlet velocity for a given time and then have the inlet velocity change with respect to the net forces acting on an obstruction in the x direction in the domain.

To expand, I have water entering an air domain with a velocity of say 10 m/s. Then, when the water reaches the obstruction, I am wanting to implement v=dtstep(g-(netforce/mass))-Vold. Essentially, I am describing the movement of the obstruction by varying the inlet flow.

I have tried to carry this out a few ways with no success. First, I defined an initial inlet velocity of 10 m/s and then specified the velocity at the inlet as Vnew, where Vnew was Vnew=dtstep(g-(force_x()@wall)/Mass)-probe(u)@monitorpoint. The mass is the mass of the obstruction defined by the volume and density. I put the monitorpoint in line with the obstruction in the farfeild (i.e. far enough away so as not to pick up velocity fluctuations due to the obstruction). Further, I tried putting the obstruction right at the inlet and at a distance from the inlet. Where the obstruction was right at the inlet, I put the monitor point at the inlet. Rather than using a monitor point, I have also tried using areaave and found that because the velocity fluctuates about the obstruction, average velocity at the inlet is affected.

I have also tried splitting up the domain into subdomains, whereby I have an inlet domain and a domain with the obstruction in it. I had hoped that I could use the inside()@subdomain to maintain a constant velocity until the water reached the obstruction domain, but it would appear that I was mistaken in the correct usage of this function (I think).

Because I am interested in large relative displacements and an accurate solution at the wall and thereafter, I am unable to just move the obstruction by deforming the mesh (and hence, use the mesh displacement for Vold, like in the FSI valve tutorial). I suspect that the CFX expression language can be used for this, I'm just lost as to how I can implement it. Any suggestions would be greatly appreciated.
aeroman is offline   Reply With Quote

Old   August 5, 2009, 10:13
Default whoops
  #2
New Member
 
Join Date: Jul 2009
Posts: 22
Rep Power: 8
aeroman is on a distinguished road
Note: I put the equations in backwards they are Vold+dtstep(g-(f/m)).

Sorry about that.
aeroman is offline   Reply With Quote

Old   August 5, 2009, 12:33
Default
  #3
Senior Member
 
ckleanth's Avatar
 
George
Join Date: Mar 2009
Location: Birmingham, UK
Posts: 257
Rep Power: 9
ckleanth is on a distinguished road
what if you use the subdomain to freeze the velocity of your phase at a spesified location (a bounding box with x,y,z relations)? you can write the ccl to have this freezing effect to capture your moving obstruction

(that is if I understood what you want to do...) why you change the inlet velocity anyway? whats the physical problem?
__________________
Top 4 tips
1. Knowledge is everything and Ignorance is dangerous.
2. Understand your limitations and try to eliminate them.
3. Get yerself a bike and hoon the chuffer. You will soon learn why dogs like to hang their heads out the car window.
4. Please before asking any questions on how to run simulations in CFX, go though all the tutorials
ckleanth is offline   Reply With Quote

Old   August 5, 2009, 12:48
Default hmmm
  #4
New Member
 
Join Date: Jul 2009
Posts: 22
Rep Power: 8
aeroman is on a distinguished road
Thanks for your reply!!

I'm not sure what you mean however. Lets say I have two subdomains 1 is an inlet domain and the other has the obstruction at the interface between the two domains. If I give the inlet domain a constant fluid velocity I can somehow freeze the inlet domain and begin recalculating flow velocity as the fluid enters the obstruction domain?
aeroman is offline   Reply With Quote

Old   August 5, 2009, 12:59
Default
  #5
Senior Member
 
ckleanth's Avatar
 
George
Join Date: Mar 2009
Location: Birmingham, UK
Posts: 257
Rep Power: 9
ckleanth is on a distinguished road
i still dont get what you want to do.. have any pics/schematic of the problem?
__________________
Top 4 tips
1. Knowledge is everything and Ignorance is dangerous.
2. Understand your limitations and try to eliminate them.
3. Get yerself a bike and hoon the chuffer. You will soon learn why dogs like to hang their heads out the car window.
4. Please before asking any questions on how to run simulations in CFX, go though all the tutorials
ckleanth is offline   Reply With Quote

Old   August 5, 2009, 13:01
Default physical problem
  #6
New Member
 
Join Date: Jul 2009
Posts: 22
Rep Power: 8
aeroman is on a distinguished road
I got a little trigger happy with the submit button and didn't answer your question. The physical problem is an object entering the water with a given velocity. I want to change the inlet velocity since the velocity of the object will decay with time due to the net forces acting on it. It is important to the body entry dynamics that I model this velocity accuratly.
aeroman is offline   Reply With Quote

Old   August 5, 2009, 13:11
Default Model
  #7
New Member
 
Join Date: Jul 2009
Posts: 22
Rep Power: 8
aeroman is on a distinguished road
Please find attached a picture of the CAD model. the circular region is modeled as a no slip wall. the left wall is the inlet, the upper and lower walls are free slip walls. and the right wall is the opening.
Attached Images
File Type: jpg Part1.jpg (43.8 KB, 54 views)
aeroman is offline   Reply With Quote

Old   August 5, 2009, 18:55
Default
  #8
Senior Member
 
ckleanth's Avatar
 
George
Join Date: Mar 2009
Location: Birmingham, UK
Posts: 257
Rep Power: 9
ckleanth is on a distinguished road
well why not using the immersed solids?

if the mesh movement is not imposed and using mesh deformation the only forces acting on the object for example on x direction is: mass * X dot = fluid force X ;cant you do something similar as shown in the example found in the cfx manual?

if the mesh movement is imposed its pretty easy
__________________
Top 4 tips
1. Knowledge is everything and Ignorance is dangerous.
2. Understand your limitations and try to eliminate them.
3. Get yerself a bike and hoon the chuffer. You will soon learn why dogs like to hang their heads out the car window.
4. Please before asking any questions on how to run simulations in CFX, go though all the tutorials
ckleanth is offline   Reply With Quote

Old   August 5, 2009, 20:58
Default
  #9
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,941
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
Hi,

Yes, I would consider using immersed solids with the 6DOF solver for this. Also in your original approach be careful about specifying a varying inlet velocity to model the body motion. This approach means you are using an accelerating frame of reference but the acceleration terms are not in the model - this can potentially cause errors.

Glenn Horrocks
ghorrocks is offline   Reply With Quote

Old   August 6, 2009, 13:42
Default Thanks
  #10
New Member
 
Join Date: Jul 2009
Posts: 22
Rep Power: 8
aeroman is on a distinguished road
I will have acess to V12 this tuesday and will use the immersed solids model as you recommend. This has been advised to me in a previous thread (thanks Glen). I see what you mean about the errors, I managed to fix the problem for the tme being, but am looking forward to using the 6dof solver in V12 (no doubt you will be hearing from me when I open that can of worms!!)

Thanks again

P.S. I now have a deep and profound interest in "hooning the chuffer"...
aeroman is offline   Reply With Quote

Old   August 6, 2009, 14:13
Default one more question
  #11
New Member
 
Join Date: Jul 2009
Posts: 22
Rep Power: 8
aeroman is on a distinguished road
Just one more quick question. In version 12 cfx mesh movement is carried out by compressing and stretching the mesh about the body. In fluent, the cells are removed and replaced as the body translates. For my problem, it would be a massive help if the cells could be removed and replaced since I need to travel many diameters to capture the physics of interest. I know I need to read up on this, and I will, but does V 12 CFX handle dynamic meshing like in fluent?
aeroman is offline   Reply With Quote

Old   August 6, 2009, 14:24
Default
  #12
New Member
 
Join Date: Jul 2009
Posts: 22
Rep Power: 8
aeroman is on a distinguished road
ok, I answered my own question. immersed solids does not need to deform the mesh. I knew I should have read before writing.

But now I have another (less ignorant) question, for my ball moving from air into water the resolution of seperation at the wall and downstream turbulance is what I am wanting to model (mostly). From what I have read immersed solid solver does not solve near wall turbulant conditions. I'm not sure if I am understanding this correct, but it would seem that if I need an accurate simmulation of the seperation and turbulance aft of the ball/cylinder/obstruction, a solution of near wall turbulant conditions is important .
aeroman is offline   Reply With Quote

Old   August 6, 2009, 18:42
Default
  #13
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,941
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
Yes, you are correct. The immersed body model is not good at capturing accurate boundary layer flows. If the details of the boundary layer flow is important then immersed solids is not a good approach and you need to look at the moving mesh approaches.

Glenn Horrocks
ghorrocks 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
nonuniform velocity at the inlet sambatra OpenFOAM Running, Solving & CFD 5 June 17, 2014 17:39
ATTENTION! Reliability problems in CFX 5.7 Joseph CFX 14 April 20, 2010 15:45
inlet velocity BC ahsan FLUENT 3 July 22, 2009 04:17
How to read a file with inlet velocity data? dorin CFX 13 July 20, 2007 02:16
inlet velocity profile in Polyflow srinu Main CFD Forum 0 January 16, 2003 21:27


All times are GMT -4. The time now is 21:55.