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

Pressure ratio calculation in a transient run

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

Like Tree2Likes

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   February 5, 2019, 07:22
Default
  #21
Senior Member
 
Join Date: Aug 2012
Posts: 178
Rep Power: 8
Julian121 is on a distinguished road
Quote:
Originally Posted by Opaque View Post
You are specifying the pitch angles on both sides of every rotor-stator interface, correct? Therefore, I assume you had problems with those interfaces and you are forcing the pitch, correct?

If you run with Pitch Angle/Option = Automatic only for the CT to Rotor interface, what kind of result are you getting? Same non-overlap issue?

Or more radical approach (assuming the machine can work w/o the CT component) is to remove the CT from the model, and run with a wall on that part of the rotor domain. Does the model behave sensibly?
As CFX-Pre shows a warning if automatic pitch change is selected, I always specify pitch angles on both sides of an interface.

CT to Rotor interface = Automatic
There was no effect in the reported non-overlap area fraction on side 2.
Domain interface: CT to Rotor
Time step 1 Non-overlap area fraction on side 1 = 1.70E-05
Non-overlap area fraction on side 2 = 4.58E-02
Time step 2 Non-overlap area fraction on side 1 = 9.02E-06
Non-overlap area fraction on side 2 = 4.58E-02
Time step 3 Non-overlap area fraction on side 1 = 1.70E-05
Non-overlap area fraction on side 2 = 4.58E-02
Time step 4 Non-overlap area fraction on side 1 = 1.72E-05
Non-overlap area fraction on side 2 = 4.58E-02
Time step 5 Non-overlap area fraction on side 1 = 1.63E-05
Non-overlap area fraction on side 2 = 4.58E-02
Time step 20 Non-overlap area fraction on side 1 = 1.71E-05
Non-overlap area fraction on side 2 = 4.58E-02

w/o the CT domain
Still no repeating pattern is seen even after removing the CT in the pressure ratio and the mass flow at the inlet. The images show the pressure ratio and the mass flow w/o the CT component.
So far, the rotor blade has rotated 200 degrees. Is it enough to have periodic behaviour?

it seems not having periodic behaviour is not due to non-overlap warning in CFX-Solver manager.
Attached Images
File Type: jpg pressure ratio without the CT.jpg (135.5 KB, 8 views)
File Type: jpg mass flow at the inlet without the CT.jpg (134.0 KB, 5 views)
File Type: jpg convergence history without the CT.jpg (123.3 KB, 6 views)
Julian121 is offline   Reply With Quote

Old   February 5, 2019, 10:23
Default
  #22
Senior Member
 
Join Date: Jun 2009
Posts: 949
Rep Power: 17
Opaque is on a distinguished road
From the signal pattern so far, I think the simulation must be run a lot longer. I do not think it has converged yet

I would add a monitor point for Pressure on the IGV side of the IGV/Rotor domain interface. That signal must become periodic with the period of the rotor.

Based on the number of passages in the rotor and IGV, the solution will not become periodic the rotor passes several times. For your setup seems like a full turn of the machine.

In addition, your time step value of 10 per passing period is extremely coarse. The time step for a sliding mesh should never be larger than the time required to traverse the pitch of the faces at the interface. Otherwise, the solution is skipping faces as it marches through.
Julian121 likes this.
Opaque is offline   Reply With Quote

Old   February 7, 2019, 07:18
Default
  #23
Senior Member
 
Join Date: Aug 2012
Posts: 178
Rep Power: 8
Julian121 is on a distinguished road
Quote:
Originally Posted by Opaque View Post
From the signal pattern so far, I think the simulation must be run a lot longer. I do not think it has converged yet

I would add a monitor point for Pressure on the IGV side of the IGV/Rotor domain interface. That signal must become periodic with the period of the rotor.

Based on the number of passages in the rotor and IGV, the solution will not become periodic the rotor passes several times. For your setup seems like a full turn of the machine.

In addition, your time step value of 10 per passing period is extremely coarse. The time step for a sliding mesh should never be larger than the time required to traverse the pitch of the faces at the interface. Otherwise, the solution is skipping faces as it marches through.
Thank you Opaque.

I have increased the number of time steps to 40 per passing period.

A pressure monitor was added on the IGV side of the IGV/Rotor interface.

So far 12 passing periods have passed. 16 more passing periods are needed to reach a full turn.

Do you think there is a hope to reach a periodic pattern?
Attached Images
File Type: jpg mass flow at the inlet.jpg (148.2 KB, 11 views)
File Type: jpg pressure monitor at the igv rotor interface.jpg (148.5 KB, 7 views)
File Type: jpg pressure ratio.jpg (148.1 KB, 5 views)
Julian121 is offline   Reply With Quote

Old   February 11, 2019, 08:13
Default
  #24
Senior Member
 
Join Date: Aug 2012
Posts: 178
Rep Power: 8
Julian121 is on a distinguished road
Quote:
Originally Posted by Opaque View Post
From the signal pattern so far, I think the simulation must be run a lot longer. I do not think it has converged yet

I would add a monitor point for Pressure on the IGV side of the IGV/Rotor domain interface. That signal must become periodic with the period of the rotor.

Based on the number of passages in the rotor and IGV, the solution will not become periodic the rotor passes several times. For your setup seems like a full turn of the machine.

In addition, your time step value of 10 per passing period is extremely coarse. The time step for a sliding mesh should never be larger than the time required to traverse the pitch of the faces at the interface. Otherwise, the solution is skipping faces as it marches through.
I have run the simulation a full turn so far and It has not converged yet.

Do you think it will converge soon?

After a full turn, I realized that I should have used more coefficient loops to reach convergence below 1e-5.

Can I use larger time step to speed up the convergence?
Attached Images
File Type: jpg pressure igvrotor.jpg (164.8 KB, 7 views)
File Type: jpg convergence.jpg (147.8 KB, 7 views)
File Type: jpg mass flow.jpg (170.7 KB, 10 views)
File Type: jpg pressure ratio.jpg (162.3 KB, 8 views)
Julian121 is offline   Reply With Quote

Old   February 12, 2019, 01:24
Default
  #25
Senior Member
 
Join Date: Aug 2012
Posts: 178
Rep Power: 8
Julian121 is on a distinguished road
I know that transient simulations are very lengthy and I have to be patient, but I am afraid that it might not converge after many revolutions!

Has anyone got experience with such transient simulation?

How many revolutions would be necessary to reach repeating periodic pattern?
Attached Images
File Type: jpg Pressure ratio.jpg (167.5 KB, 14 views)
Julian121 is offline   Reply With Quote

Old   February 12, 2019, 17:05
Default
  #26
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 15,569
Rep Power: 118
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
Correct, the transient simulation may not converge. But it might. Don't know until you try it. But that is one of the interesting things about fluid mechanics - you can trigger instabilities and chaotic flows depending on what regime you are in.

How long to run it for? Long enough that you are confident that it is representative. So if you are looking for the average flow, then run it until it is just jiggling about an obvious average value.

How long will this take? Again, you cannot tell in advance. It could be short, it could be long. Run it and monitor it.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.
ghorrocks is offline   Reply With Quote

Old   February 13, 2019, 10:19
Default
  #27
Senior Member
 
Join Date: Aug 2012
Posts: 178
Rep Power: 8
Julian121 is on a distinguished road
Based on these results, although they are not converged yet (for example pressure ratio), can one conclude that the flow is transient in the compressor under investigation and no steady state solution exists?
As I wrote in my previous posts, I tried to obtain a steday solution for a long time but no convergence was achievable below 1e-4 .
Julian121 is offline   Reply With Quote

Old   February 13, 2019, 16:30
Default
  #28
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 15,569
Rep Power: 118
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
It appears highly likely no steady state exists. You can only be completely sure if you run it long enough to see a repeating pattern, or to convince yourself that the result is chaotic.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.
ghorrocks is offline   Reply With Quote

Old   February 14, 2019, 10:39
Default
  #29
Senior Member
 
Join Date: Aug 2012
Posts: 178
Rep Power: 8
Julian121 is on a distinguished road
The operating point I am simulating is 1.8 kg/s and the last measured experimental point (stalling side) is 1.5 kg/s.

If the transient simulation does not converge after many turns of the rotor which seems so, shouldn’t the problem be caused by numerical reasons?

I am concerned that the reason why I have not been able to find either steady or transient solution would be something other than physical instability.

At first of the simulation with CFX, I was using a wrong interface between the Rotor and the CT domains. I did not divide the shroud due to the difficulty in using ICEM and assigned an interface between the CT and the whole shroud surface but I had better results than now! Pressure ratio had small oscillations or even did not change but the RMS residuals did not drop.

After I learned ICEM, I divided the shroud surface into two surfaces and assigned correct BCs as an interface between the Rotor and the CT and the shroud (wall boundary) which does not rotate in global coordinate system.

It is not clear for me why the modified rotor which is representative of the correct experiment should not reach a solution, though.

The attached images are the mass flow at the inlet of the compressor and the pressure ratio after nearly 73 passing periods.
In addition, the images of the rotor before and after creating the separation of the shroud surface have been attached.
Attached Images
File Type: jpg mass flow at the inlet.jpg (169.9 KB, 7 views)
File Type: jpg pressure ratio.jpg (164.6 KB, 6 views)
File Type: jpg modified rotor.jpg (94.7 KB, 9 views)
File Type: jpg first rotor.jpg (152.6 KB, 6 views)
Julian121 is offline   Reply With Quote

Old   February 14, 2019, 16:50
Default
  #30
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 15,569
Rep Power: 118
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
If you want to be sure what you are seeing is physical or numerical then you need to do a validation and verification exercise. The FAQ is on a different topic but effective describes a V&V: https://www.cfd-online.com/Wiki/Ansy..._inaccurate.3F
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.
ghorrocks is offline   Reply With Quote

Old   February 16, 2019, 02:45
Default
  #31
Senior Member
 
Join Date: Aug 2012
Posts: 178
Rep Power: 8
Julian121 is on a distinguished road
Here I have not defined an interface between the IGV and the CT.

They have nothing in common except a curve.

Is it correct?
Julian121 is offline   Reply With Quote

Old   February 16, 2019, 03:02
Default
  #32
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 15,569
Rep Power: 118
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
GGI interfaces on some settings can account for a mismatch across the interface due to periodicity. So it might be OK. But it might not, depending on what you are doing.

Have a look at the streamlines and flow to see if it is correctly crossing the interface.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.
ghorrocks is offline   Reply With Quote

Old   February 16, 2019, 06:13
Default
  #33
Senior Member
 
Join Date: Aug 2012
Posts: 178
Rep Power: 8
Julian121 is on a distinguished road
For some reason the flow is not continious even when all the domains are selected but I can see the streamlines in each domain individually.

There is a depression area in the streamlines of the rotor (image3). Isn't it suspicious?

In addition, there exists some flow reversal in the trailing edge of the IGV (image4) which doesn't seem right.

Should I change the interface default settings to account for any possible mismatch?

Should I glue the domains in CFX-Pre?
Attached Images
File Type: jpg image1.jpg (64.3 KB, 8 views)
File Type: jpg image2.jpg (70.2 KB, 8 views)
File Type: jpg image3.jpg (81.6 KB, 7 views)
File Type: jpg image4.jpg (128.3 KB, 8 views)
Julian121 is offline   Reply With Quote

Old   February 17, 2019, 05:17
Default
  #34
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 15,569
Rep Power: 118
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
You need to do a careful study what connects to what and whether it seems to be working correctly. This is not a suitable issue to sort out on the forum as it will require you to do careful use of the post processor and possibly run some additional simulations to test things.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.
ghorrocks is offline   Reply With Quote

Old   February 17, 2019, 07:14
Default
  #35
Senior Member
 
Join Date: Aug 2012
Posts: 178
Rep Power: 8
Julian121 is on a distinguished road
I think the reason why the streamlines were not shown in all domains was because the rotor was not in front of the IGV/Stator due to the transient simulation.

I have not merged any mesh since I have defined an interface between the domains.

Following my last question there is no common interface between the IGV/CT domains as shown by a red circle but a curve. Should I define an interface here?
Attached Images
File Type: jpg image.jpg (131.1 KB, 6 views)
Julian121 is offline   Reply With Quote

Old   February 17, 2019, 16:38
Default
  #36
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 15,569
Rep Power: 118
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
If those domains only share an edge in common then there is no common face to put an interface on. So there is no reason to put an interface there.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.
ghorrocks is offline   Reply With Quote

Old   February 18, 2019, 07:27
Default
  #37
Senior Member
 
Join Date: Aug 2012
Posts: 178
Rep Power: 8
Julian121 is on a distinguished road
Dear Glenn, thank you for your clear explanation.

So, after 97 passing periods (38 passing periods are equal to one full turn in my transient simulation) no periodic pattern has been observed and I have decided to monitor the number of inner loops to check whether 5 inner coefficients are sufficient.

According to the attached images which show the mass flow and the pressure ratio, is it safe to use 5 inner coefficients?

How can I deactivate the coefficient convergence monitor during a run temporarily? Once it is on, I cannot check whether a periodic behaviour is created!
Attached Images
File Type: jpg residuals.jpg (160.9 KB, 7 views)
File Type: jpg pressure ratio.jpg (131.3 KB, 8 views)
File Type: jpg mass flow.jpg (137.1 KB, 8 views)
Julian121 is offline   Reply With Quote

Old   February 18, 2019, 16:27
Default
  #38
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 15,569
Rep Power: 118
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
It is not normal to run with fixed coefficient iterations. The normal way of defining convergence is by using a residual tolerance. Then the number of coefficient loops can get bigger and smaller as required to give the accuracy you define. So do a sensitivity study on residuals convergence tolerance, not number of coefficient loops.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.
ghorrocks is offline   Reply With Quote

Old   February 19, 2019, 07:00
Default
  #39
Senior Member
 
Join Date: Aug 2012
Posts: 178
Rep Power: 8
Julian121 is on a distinguished road
Maybe this is the reason why the simulation has not converged yet.

There is some imbalance of the order of 0.001. Is it big?

I have been using 40 time steps per passing period since the start until now (105 passing periods). Should I increase it?
Attached Images
File Type: jpg imbalance.jpg (126.7 KB, 4 views)
Julian121 is offline   Reply With Quote

Old   February 19, 2019, 16:50
Default
  #40
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 15,569
Rep Power: 118
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
0.001% imbalances are pretty small for most cases. But you should do a sensitivity analysis to see if it is OK in your case.

Is 40 time steps OK? Do a time step sensitivity analysis and find out!
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.
ghorrocks 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 On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Wind tunnel Boundary Conditions in Fluent metmet FLUENT 5 September 19, 2017 00:09
Problem with an old Simulation FrankW CFX 3 February 8, 2016 04:28
transient pressure and temperature boundary condition profile inicialization Aurora23 FLUENT 2 April 21, 2015 16:01
Get the maximum and minimum pressure in the domain(In parallel calculation) xh110120 Fluent UDF and Scheme Programming 4 October 10, 2014 08:06
Warning 097- AB Siemens 6 November 15, 2004 04:41


All times are GMT -4. The time now is 20:28.