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

User Variable Plot and Oscillating Convergence

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

Like Tree1Likes
  • 1 Post By ghorrocks

Reply
 
LinkBack Thread Tools Display Modes
Old   August 21, 2014, 11:11
Default User Variable Plot and Oscillating Convergence
  #1
New Member
 
Marcel Jay
Join Date: Jun 2014
Location: Berlin
Posts: 14
Rep Power: 3
marcel_jay is on a distinguished road
Hello CFD Community,

I am experience some convergence problems and that's why want to observe user variables in my simulation.
At first I just plotted pressure loss, which worked fine, but now additionally I want to plot average inlet velocity and mass flow.
The issue is, it is all plotted in one graph, so I see the velocity converging, but the other two are displayed just as a line next to the x-axis. I think it's because the values are to far from each other.
Any hint how to fix this?

Secondly, I wanted to ask what you think about a converging solution that is not monotonic, means oscillation. It reaches the residual target after about 170 timesteps though.
Is the non-monotonic behaviour inaccurate even if the result is below my residuals?

Cheers
Marcel
Attached Images
File Type: jpg 333.jpg (28.4 KB, 18 views)
File Type: jpg user points.jpg (24.3 KB, 16 views)
marcel_jay is offline   Reply With Quote

Old   August 21, 2014, 11:18
Default Found a solution
  #2
New Member
 
Marcel Jay
Join Date: Jun 2014
Location: Berlin
Posts: 14
Rep Power: 3
marcel_jay is on a distinguished road
Okay, for the first issue, I just found out you can right click the plotted graph (Monitor Properties) and deselect single variables!
marcel_jay is offline   Reply With Quote

Old   August 21, 2014, 20:52
Default
  #3
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,800
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
The residual is not a total measure of convergence. The variation on your inlet velocity suggests that in your case, even though the residuals are tight the flow has not converged. So in your case I would add imbalances to your convergence requirement. Then you will continue until the global balances are good too.

This is a sign that your physical time scale is probably too short. You would converge faster if you used a larger physical time scale.
rgd likes this.
ghorrocks is online now   Reply With Quote

Old   September 5, 2014, 11:20
Default
  #4
New Member
 
Marcel Jay
Join Date: Jun 2014
Location: Berlin
Posts: 14
Rep Power: 3
marcel_jay is on a distinguished road
First of all, thanks a lot for you answer.

I now understand my user variables as my main convergence criteria.
RMS Targets were after about 100 timesteps very close to 1E-4, but all my user variables very diverging (almost linear). And that even after 500 timesteps, whilst Momentum and Mass were oscillating at the same level.

As I think my mesh is pretty good (min orthogonal quality = 0.25 and max skewness = 0.8) I might have to fix the timescale.
Imbalances were set to 1% and the results were 0.05% to 1.7% which is not even too bad I suppose.

I used automatical timescale (conservative, factor 1.0) so far.

In the CFD-Online Tutorial it says I need the average residence time, don't know how to get that. In the streamline it tells me that 0,00013s is the max value.
Do you know how to find the right physical time scale?
Also shouldn't I use the residence time of previous converging models (similar), as with diverging velocitys the timescale changes. In my previous solutions the max residence time was 10 times higher.

An ANSYS video tutorial said you should use a physical timescale of about 1/3 of the velocity scale or 1/ω when the domain rotates. Mine rotates with 30k rpm.
As I've seen people using timescales of about 2 seconds... mine would be a million times smaller, isn't that bad?

Cheers
Marcel
marcel_jay is offline   Reply With Quote

Old   September 6, 2014, 07:48
Default
  #5
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,800
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
In a steady state simulation the exact value of the time step is not important. All the suggestions of residence time or functions of the rotation speed are really just starting guesses. You need an approximate time step just to get started.

If it diverges then restart with a smaller time step. If it converges slowly then use "edit run in progress" to increase the time step. You can probably edit it a few times as the simulation converges you should be able to use larger time steps. But if it starts to go wobbly you have gone too far so back it off again.

So all the time step sizes you quote are just a starting point, and it does not really matter which one you choose. You then run it and adjust it as you go.
ghorrocks is online now   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
Oscillating residuals and no convergence! Sherlock_1812 OpenFOAM Running, Solving & CFD 7 August 20, 2014 09:39


All times are GMT -4. The time now is 23:02.