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

Rotating domain vs Wall velocity

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

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   January 19, 2020, 16:55
Default Rotating domain vs Wall velocity
  #1
Senior Member
 
Jiri
Join Date: Mar 2014
Posts: 218
Rep Power: 13
Jiricbeng is on a distinguished road
Hi there,


I analyze a simple 2D model of a bearing to verify basic equations.
The issue is as follows:
The bearing domain consists of inner wall, outter wall and 2 symmetry planes. The inner wall rotates 80000 rev/min, the outer wall rotates 30000 rev/min.
1) I set stationary domain and wall velocity inner 80000 and outer 30000
2) I set rotating domain to 30000, inner wall velocity 50000 and outer is default.


When ploting the variable "Pressure" (which is scalar and invariant) around inner wall I obtain different curves in both cases. They are both perfectly converged. The Velocity in Stn Frame on inner wall is the same for both cases, which means that velocity field is the same. The question is why is the pressure different?


Btw, I modified the case 2) by swithing off rotating domain. So I kept the inner velocity 50000 and outer to be zero but domain was stationary. And I obtained the same results of the pressure around the inner wall. It looks as if the pressure was not affected whereas velocity were changed..
Jiricbeng is offline   Reply With Quote

Old   January 19, 2020, 23:57
Default
  #2
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,749
Rep Power: 143
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
Check your convergence in this comparison, and use double precision numerics. I would converge these simulations tighter than normal to reduce numerical errors caused by the large variations in velocities.
__________________
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, 04:03
Default
  #3
Senior Member
 
Jiri
Join Date: Mar 2014
Posts: 218
Rep Power: 13
Jiricbeng is on a distinguished road
Thank you very much for suggestion. I tried it with double precision but I obtained the very same results. Imbalances are also again zero..
Do you think it is still matter of convergence (e.g. try out finer mesh) or is there some other misunderstanding?
Jiricbeng is offline   Reply With Quote

Old   January 20, 2020, 04:58
Default
  #4
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,749
Rep Power: 143
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
The residuals are more important that imbalances in this case, I suspect.

Making sure your results are properly converged is just the first thing to check. There are others, such as round off errors, simulation set up, mesh resolution and so on.
__________________
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 21, 2020, 06:04
Default
  #5
Senior Member
 
Jiri
Join Date: Mar 2014
Posts: 218
Rep Power: 13
Jiricbeng is on a distinguished road
The residuals are below E-4 and monitored variables (e.g. force x,y) are very stable, several thousands iterations were done, when changing time scale no change of monitored variables occurs, this is valid for both cases. I found difference in velocity in Stn Frame across bearing thickness which likely is the reason of different "Pressure". I cannot converge more the cases, it seems there is another glitch...
Jiricbeng is offline   Reply With Quote

Old   January 21, 2020, 17:50
Default
  #6
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,749
Rep Power: 143
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
I would converge tighter than 1E-4 to check this. I would also try using double precision numerics to see if round off error affects it.

Can you post an image of what you are modelling and your output file?
__________________
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 23, 2020, 02:25
Default
  #7
Senior Member
 
Jiri
Join Date: Mar 2014
Posts: 218
Rep Power: 13
Jiricbeng is on a distinguished road
I am sending in the attachment. I am modelling a bearing with eccentricity of several microns. It is a 2D model (I cell in axial direction). I tried also refined the mesh with double precision.
Attached Images
File Type: jpg figure.jpg (40.6 KB, 20 views)
Attached Files
File Type: txt Case2_002_txt.txt (118.2 KB, 4 views)
Jiricbeng is offline   Reply With Quote

Old   January 23, 2020, 17:20
Default
  #8
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,749
Rep Power: 143
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
Your domain is 9mm across, but you are trying to resolve the effect of a few microns displacement. That is a ratio of about 1000:1, which means round-off errors will make this simulation difficult, if not impossible by the approach you are using. So I am not surprised you are getting weird results, round-off errors are limiting the simulation.

I would recommend doing some background reading to understand round-off errors in CFD better, and then you will need to revise your simulation approach to reduce round off errors. This will probably mean you model this geometry in small segments rather than one big ring.
__________________
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 25, 2020, 08:07
Default
  #9
Senior Member
 
Jiri
Join Date: Mar 2014
Posts: 218
Rep Power: 13
Jiricbeng is on a distinguished road
Thank your for advice. Do you have any documentation regrading this issue? I do not know what to improve basically, I refined the mesh, computed double precision, changed time step etc. and the results are the same.
Jiricbeng is offline   Reply With Quote

Old   January 25, 2020, 16:16
Default
  #10
Senior Member
 
Jiri
Join Date: Mar 2014
Posts: 218
Rep Power: 13
Jiricbeng is on a distinguished road
Thank your for advice. Do you have any documentation regrading this issue? I do not know what to improve basically, I refined the mesh, computed double precision, changed time step etc. and the results are the same.


In addition, I analyzed the case in Fluent (double precision, converged below E-7) and obtained basically the same results. I think it is not a round-off error.

The question therefore is, is rotating domain approach fully analogous to rotating walls, in general? Must the results be the same?
Jiricbeng is offline   Reply With Quote

Old   January 28, 2020, 05:20
Default
  #11
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,749
Rep Power: 143
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
Please attach the output file of both runs.
__________________
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 28, 2020, 07:47
Default
  #12
Senior Member
 
Jiri
Join Date: Mar 2014
Posts: 218
Rep Power: 13
Jiricbeng is on a distinguished road
Please find attached, case2 is rotating domain, case3 is wall rotation
Attached Files
File Type: txt Case3_003.txt (167.6 KB, 4 views)
File Type: txt Case2_004.txt (167.4 KB, 2 views)
Jiricbeng is offline   Reply With Quote

Old   January 28, 2020, 19:01
Default
  #13
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,749
Rep Power: 143
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
I can't see the problem. I do note that in the stationary domain case you have the inner wall rotating about axis 1.3 but the outer wall about axis 0.3. Are you sure this is correct? Also you should have a look at the results carefully and see if you can see the difference between the runs.

You appear to have a very coarse mesh on this and the residuals are very low compared to normal. This does not bode well. I recommend you try doing this with a small segment rather than the whole ring, as I said previously.
__________________
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 29, 2020, 09:48
Default
  #14
Senior Member
 
Erik
Join Date: Feb 2011
Location: Earth (Land portion)
Posts: 1,171
Rep Power: 23
evcelica is on a distinguished road
"I recommend you try doing this with a small segment rather than the whole ring, as I said previously"


I agree. This is the perfect candidate for a periodic model.
evcelica is offline   Reply With Quote

Old   January 29, 2020, 10:55
Default
  #15
Senior Member
 
Jiri
Join Date: Mar 2014
Posts: 218
Rep Power: 13
Jiricbeng is on a distinguished road
Thank you both for the reply. However, there is eccentricity as I mentioned previously hence I think segment model cannot be considered.

Therefore the inner wall rotates around axis 1.3 and outer wall around 0.3. 1.3 is axis "z" shifted in x direction by several microns. Therefore, maybe, rotating domain approach cannot be used because there are two circles of different center (axis) and giving rotation to the whole domain around one axis may cause the problems.
Jiricbeng is offline   Reply With Quote

Old   January 29, 2020, 17:39
Default
  #16
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,749
Rep Power: 143
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
Looks like you worked it out. Your two simulations are modelling different things because of the eccentricity.
__________________
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 30, 2020, 09:06
Default
  #17
Senior Member
 
Jiri
Join Date: Mar 2014
Posts: 218
Rep Power: 13
Jiricbeng is on a distinguished road
Perhaps, it might be main culprit
Jiricbeng 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
Wrong flow in ratating domain problem Sanyo CFX 17 August 15, 2015 06:20
rotation velocity of a water wheel and rotating domain Ema40 FLUENT 0 November 12, 2014 10:50
Correct velocity boundary condition for a wall in a rotating mesh zordiack OpenFOAM Running, Solving & CFD 2 March 4, 2014 10:11
injection problem Mark New FLUENT 0 August 4, 2013 01:30
what the result is negatif pressure at inlet chong chee nan FLUENT 0 December 29, 2001 05:13


All times are GMT -4. The time now is 10:47.