CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > OpenFOAM Running, Solving & CFD

Please help How is delta t determined in interFoam

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

Reply
 
LinkBack Thread Tools Display Modes
Old   February 23, 2005, 22:44
Default Hi, Yesterday, I ran a tes
  #1
Pei-Ying Hsieh (Hsieh)
Guest
 
Posts: n/a
Hi,

Yesterday, I ran a test case:

Cloned the damBreak case.
Axi-symmetric (so, a wedge was built).
radius = 2 mm (set to 2, with 0.001 scaling factor).
length = 5 mm (set to 5, with 0.001 scaling factor).
4 degree wedge.

inlet flow rate set o 0.001 m/sec.
Wall contact angle = 90 degree
one outlet.
fluids properties are the same as in the damBreak case (water and air?)

in FoamX, set initial delta t to 1e-5 seconds.
Set delta t to autoadjustable.

Very quickly, the delta t was adjusted automatically to about 3.7e-7 seconds. This seem a little bit small given the conditions I set. Can anyone tell me why this is so small? How is delta t determined by the code? Thanks!

Pei
  Reply With Quote

Old   February 24, 2005, 05:25
Default The deltat is determined from
  #2
Mattijs Janssens (Mattijs)
Guest
 
Posts: n/a
The deltat is determined from the max Courant number. This in turn is determined on a face by face basis using the local velocity (from the face flux) and the distance to the cell centre.
(CourantNo.H in cfdTools)

The time step is then adjusted given the ratio between wanted Co and calculated Co. The time step can decrease unlimited but the increase is limited to prevent oscillations.
(setDeltat.H in cfdTools)
  Reply With Quote

Old   February 24, 2005, 08:49
Default I can tell you with 99.9% cer
  #3
Eugene de Villiers (Eugene)
Guest
 
Posts: n/a
I can tell you with 99.9% certainty that there is a problem with your setup Pei.

Some ideas,
Do not use wedges unless you have periodic rotational flow.
Do not allow the inlet to become "dry" (i.e. use a additional pipe length.)
  Reply With Quote

Old   February 24, 2005, 08:49
Default Hi, Mattijs, Thanks! This
  #4
Pei-Ying Hsieh (Hsieh)
Guest
 
Posts: n/a
Hi, Mattijs,

Thanks! This is what I thought.

Given these BCs, a rough calculation,

delta t = CFL * delta x/ Velocity
= 0.5 * 5 mm/40 / 1 mm/sec
~ 0.06 seconds

So, I will expect delta t to be on the order of 0.01 seconds. But, OpenFOAM adjusted it to 3e-7 seconds. What could be the reason? Is there any way to print out all the courant numbers on each cell calulcated by the code?

Can anyone run a quick simple axi-symmetric (tube) calculation (20X40 cells in X-Y axis) to confirm this?

Pei
  Reply With Quote

Old   February 24, 2005, 10:27
Default Hi, Eugene, Thanks for the
  #5
Pei-Ying Hsieh (Hsieh)
Guest
 
Posts: n/a
Hi, Eugene,

Thanks for the reply. I suspect this problem could be due to my setup, but, this is such a simple problem.

Let me describe my steps again:

1. cloned the case from the damBreak case.
(so, this is a 2-phase flow problem with air/water, with surface tension and contact angle).
2. computational domain is axi-symmetric. In the user manual, it mentioned using wedge for the two side faces.
3. revised the BlockMeshDict so that domain is 2 mm by 5 mm (with 20 by 40 cells in X-dir and Y-dir).
4. generated mesh, checked using paraFoam - no obvious problem found.
5. runFoamX, set the boundary conditions, inlet velocity is set to 0.001 in Y-dir. For inlet, gamma set to 1, so that water starts to flow into the domain when simulation starts.
6. setup start time, end time, initial delta t to 1e-5.
7. at time t=0, computation domain is set to gamma = 0 (that is, no special initialized done - no setgammaDamBreak type thing).

Pei
  Reply With Quote

Old   February 24, 2005, 10:45
Default 2. The dambreak geometry is n
  #6
Eugene de Villiers (Eugene)
Guest
 
Posts: n/a
2. The dambreak geometry is not axi-symmetric. It is a very flat 3D case (move it around in paraview and you will see). So you cant use wedge BCs on the side patches unless you collapse one side of the domain to an edge. Anyway, if the problem is still 2D, there is little point in using wedge patches since they are for rotating flows.

5. That flow speed is awfully slow. Given that gravity is switched on in the dambreak case, your inlet is likely to run "dry" (fluid moves away from the inlet faster than it enters). This will cause the code to diverge, because of a surface tension-gamma gradient related problem (check old posts for details). If the inlet is from below, none of this matters of course.

To aid diagnostics, dump the results very frequently and look where the high velocities are originating.
  Reply With Quote

Old   February 24, 2005, 11:57
Default Hi, Eugene, I cloned the d
  #7
Pei-Ying Hsieh (Hsieh)
Guest
 
Posts: n/a
Hi, Eugene,

I cloned the damBreak case because I am doing 2-fluid VOF simulation. The BlockMeshDict was re-built for an axi-symmetric geometry (a tube). According to the user manual, wedge type BC should be used for the two sides (circular).

X-dir is the radial direction and Y-direction is the axial direction. Flow inlet is located below and outlet on top. In this case, gravity should have no impact on velocity because the inlet velocity was specified. Gamma = 1 was specified at the inlet, so, the inlet should never run dry.

Thanks!

Pei

PS: this is a very simple test problem. An axi-symmetric tube, initially empty (fill with air with 0 verocity everywhere). At time 0, water starts to flow into the tube (from below) at 0.001 m/s. Tube length = 5 mm and tube radius = 2 mm. Surface tension turned on (same as the damBreak case). Wall contact angle set to 90 degree.
  Reply With Quote

Old   February 24, 2005, 12:38
Default Pei, As Eugene mentioned,
  #8
Ali (Ali)
Guest
 
Posts: n/a
Pei,

As Eugene mentioned, usually, for liquid jet problem only setting gamma=1 at inlet is not enough. if you just extend the inlet and fill three or four cells with liquid (instead of just 1 cell), your problem may be resolved.

PS: A stupid question, but are you sure your scaling is right. i.e. the value of 'convertToMeters' in blockMeshDict should be in order of 1 in your case)
  Reply With Quote

Old   February 24, 2005, 12:42
Default Plus, in very small velocites
  #9
Ali (Ali)
Guest
 
Posts: n/a
Plus, in very small velocites and small scales (higher curvature), you may get spurious velocities due to surface tension) higher than jet velocity and that screws up everything.

To make sure this is not happenning, try this:

1 m/s. Tube length = 5 m and tube radius = 2 m

I know if you do this Reynolds changes a lot, but 'delta-t' again should be in the same range as you want.
  Reply With Quote

Old   February 24, 2005, 14:10
Default Hi, Ali, Great! I basical
  #10
Pei-Ying Hsieh (Hsieh)
Guest
 
Posts: n/a
Hi, Ali,

Great! I basicaly set the ConvertToMeters to 1 (so, the geometry is 2 m and 5 m, respectively).
Set inlet velocity to 1 m/s. I got qood results.

OK, so, for small ID tube (2 mm), surface tension has a strong effect on stability. I have similar simulation using Fluent and did not have the same problem. I am going to repeat exactly the same problem using Fluent today. I will report back my results.

Ali, why did you say the ConvertToMeters should be 1 in my previous case? The values were for mm, so, I set ConvertToMeters to 0.001 so that it converts to meter, correct?

Pei
  Reply With Quote

Old   February 24, 2005, 14:13
Default By the way, in the previous t
  #11
Pei-Ying Hsieh (Hsieh)
Guest
 
Posts: n/a
By the way, in the previous testing suggested by Ali ( 2 m by 5 m, and 1 m/s inlet vel), I did NOT fill any cells next to the inlet to fluid (and still got good results).

Pei
  Reply With Quote

Old   February 24, 2005, 15:37
Default HI, I just ran my original
  #12
Pei-Ying Hsieh (Hsieh)
Guest
 
Posts: n/a
HI,

I just ran my original case (2 mm by 5 mm tube) and set the surface tension constant, sigma, to 0.001 (it was 0.07), inlet vel is 0.001 m/s. In this case, the effect of surface tension force is minimized. I got 6.9e-7 detal t still. So, does it mean that the surface tension force is not the problem?

Pei
  Reply With Quote

Old   February 24, 2005, 15:50
Default Qoute from Pei:"Ali, why did
  #13
Ali (Ali)
Guest
 
Posts: n/a
Qoute from Pei:"Ali, why did you say the ConvertToMeters should be 1 in my previous case? The values were for mm, so, I set ConvertToMeters to 0.001 so that it converts to meter, correct?
"

Yeah sorry you're right I meant 1e-3 not 1.

---------------------------
1) Why don't you turn off the gravity and see if there is any difference.

2) How you tried 0 (zero) surface tension? What you get then?

3) I still think the problem decreases if you fill the inlet with some cells.

4) It may not be solely surface tension, it can be the interFoam tracking and pressure-velocity coupling. So, fill the inlet with some fluid and see what happens.

Low velocity jets are still difficult to deal with.
  Reply With Quote

Old   February 24, 2005, 22:40
Default Hi, Ali, I will try turnin
  #14
Pei-Ying Hsieh (Hsieh)
Guest
 
Posts: n/a
Hi, Ali,

I will try turning off the gravity next.

I set surface tension constant from 0.07 to 0.0001 and contact angle to 1 degree -> surface tension force should be small enough.

I will try filling few cells with water near the inlet also. How to do this the easy way?

I started a Fluent run tonight. At the early stage, it seems holding up.

Regards,

Pei
  Reply With Quote

Old   March 2, 2005, 09:09
Default Hi, Problem solved by Hen
  #15
Pei-Ying Hsieh (Hsieh)
Guest
 
Posts: n/a
Hi,

Problem solved by Henry. In the BlockMeshDict set up, I only had one wedge (I put all the wedge faces into one) BC. This needs to be paired.

Also, Ali was correct, I do need to initialize some cells close to the entrance with liquid.

Thanks!

Pei
  Reply With Quote

Old   March 2, 2005, 09:30
Default But, still the bad thing is t
  #16
Ali (Ali)
Guest
 
Posts: n/a
But, still the bad thing is that if you fill some cells with liquid but your inlet is not perpendicular to the patch (i.e. inclined inlet, say you have inlet flow from the left boundary but it is not exactly from left to right, it also makes an angle with bottom boundary), it has problems with that too. This is one of the problems to be solved.
  Reply With Quote

Old   November 23, 2005, 11:06
Default setFields: works for me every
  #17
Senior Member
 
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,763
Rep Power: 21
hjasak will become famous soon enough
setFields: works for me every time. It's worth checking whether your specification makes sense, e.g. whether the box you have given falls into the actual mesh and similar. Try it on the dam break tutorial and you will see it working.

(do you use a scaling factor in blockMesh?)


Enjoy,

Hrv
__________________
Hrvoje Jasak
Providing commercial FOAM/OpenFOAM and CFD Consulting: http://wikki.co.uk
hjasak 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
Simplefoam and Delta t ariorus OpenFOAM Running, Solving & CFD 3 January 13, 2006 05:02
relaxtion delta Andrew Hayes Main CFD Forum 0 December 7, 2005 09:45
LES delta turb Main CFD Forum 2 March 2, 2005 15:27
Delta Wings R Main CFD Forum 1 October 10, 2004 13:16
Delta wing Thomas Pettersson FLUENT 1 April 22, 2000 20:18


All times are GMT -4. The time now is 10:31.