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

review of the results about rotation

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

Like Tree1Likes
  • 1 Post By ghorrocks

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   May 23, 2022, 22:17
Default review of the results about rotation
  #1
Member
 
Jin Seok Lee
Join Date: Aug 2021
Posts: 51
Rep Power: 4
jins9158 is on a distinguished road
I simulated about fan assy's simulation

The fan is sirroco fan which use in ventilation system.

I used below conditons.

1. Inlet condition
-99[Pa]
(because of loss about filters)

2. outlet condtion
80[CMH]

3. rotation condition
1) 1240[RPM]
2) Frozen rotor
3) Full blade

4. solver conditon
1) steady state
2) 1500 iteration, 700 iteration
3) time scale 7.7e -04, 7.7e-03

I simulated 1500 iteration and the time scale 7.7e-04. After that, I additionally simulated 700 iteration by using 7.7e-3 time scale becasue simulation time is short.

In short,
1500 iteration & 7.7e-04 time scale >> 1.15s
700iteration & 7.7e-03 time scale >> 5.39s
So total time is 6.54s
that means 134 rotation and I think that is enough about flow development.

When I simulated, I thought that the result is not good.
(I attached the picture of result)

I want to get some advice.

Please help me.
Attached Images
File Type: png 1.PNG (148.5 KB, 15 views)
Attached Files
File Type: zip 220520_huvenW_80_case6_cutoff_increase1_003.zip (63.9 KB, 1 views)
jins9158 is offline   Reply With Quote

Old   May 24, 2022, 03:43
Default
  #2
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,641
Rep Power: 142
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
That geometry is almost certainly not steady state. The exit jet is going to flap around, so no steady state solution exists.

See this FAQ for some tips: https://www.cfd-online.com/Wiki/Ansy...gence_criteria

But you are almost certainly going to have to simulate this transient.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.
ghorrocks is offline   Reply With Quote

Old   May 24, 2022, 04:32
Default
  #3
Member
 
Jin Seok Lee
Join Date: Aug 2021
Posts: 51
Rep Power: 4
jins9158 is on a distinguished road
Quote:
Originally Posted by ghorrocks View Post
That geometry is almost certainly not steady state. The exit jet is going to flap around, so no steady state solution exists.

See this FAQ for some tips: https://www.cfd-online.com/Wiki/Ansy...gence_criteria

But you are almost certainly going to have to simulate this transient.

Thank you for replying my question

I also thought I need to simulate transient simulation in my situation.

But, Many researchers has used steady state such as me becasue unsteady require more CPU a lot.

So Are there antoher method for me? I just can use 36 core for simulation because of license limit.

I tried to use local time scale and outlet condition change mass to pressure...
jins9158 is offline   Reply With Quote

Old   May 24, 2022, 07:59
Default
  #4
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,641
Rep Power: 142
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
The only way to reduce a transient simulation to a steady state one is to introduce so much diffusion into it that it all gets smeared out. Then it will be steady state - and horribly inaccurate. If the other researchers got steady state results on a configuration like that then I would be seriously doubting the accuracy of their results.

If there was a way to reduce a transient result to steady state the FAQ would say so. The FAQ really does describe the best path forwards, so please read 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   May 24, 2022, 10:33
Default
  #5
Senior Member
 
Join Date: Jun 2009
Posts: 1,775
Rep Power: 31
Opaque will become famous soon enough
Quote:
Originally Posted by jins9158 View Post
Thank you for replying my question

I also thought I need to simulate transient simulation in my situation.

But, Many researchers has used steady state such as me becasue unsteady require more CPU a lot.

So Are there antoher method for me? I just can use 36 core for simulation because of license limit.

I tried to use local time scale and outlet condition change mass to pressure...
What is the goal of your simulation? Flow features around the non-symmetric area? or just the overall performance of the device?

There are 3 approaches commonly used in the industry to model this device:

1 - Mixing plane between the rotor (cage) and the casing (volute)
2 - Frozen rotor approximation instead of mixing plane, and study the different orientations of the rotor (cage) with respect to the non-symmetric section. For this specific case, it seems any orientation will do since there are some many "blades" in the cage that a minor rotation will look the same as the previous configuration.
3 - Full unsteady simulation (perhaps a 4th one will be transient blade row with pitch change, but never done it myself with this use case)

Despite the crude approximations of 1 and 2, the quick solutions (hours) allow engineers to make quick design decisions (helped with additional experimental data) instead of waiting days/weeks for an unsteady solution for a single operating condition. Unsteady is only used when detailed flow features are essential (no modeling error accepted) to make the next decision.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.
Opaque is offline   Reply With Quote

Old   May 24, 2022, 22:18
Default
  #6
Member
 
Jin Seok Lee
Join Date: Aug 2021
Posts: 51
Rep Power: 4
jins9158 is on a distinguished road
Quote:
Originally Posted by ghorrocks View Post
The only way to reduce a transient simulation to a steady state one is to introduce so much diffusion into it that it all gets smeared out. Then it will be steady state - and horribly inaccurate. If the other researchers got steady state results on a configuration like that then I would be seriously doubting the accuracy of their results.

If there was a way to reduce a transient result to steady state the FAQ would say so. The FAQ really does describe the best path forwards, so please read it.

Thank you for your concern.

Now, I am simulating transient simulation by inital value using steady state result. I just set total time 0.05s because I want to one rotate the impeller. simulation time are going to need about 3days.

I know the rotation is short, but it spend much time to simulate transient.

Thank you.
jins9158 is offline   Reply With Quote

Old   May 24, 2022, 22:26
Default
  #7
Member
 
Jin Seok Lee
Join Date: Aug 2021
Posts: 51
Rep Power: 4
jins9158 is on a distinguished road
Quote:
Originally Posted by Opaque View Post
What is the goal of your simulation? Flow features around the non-symmetric area? or just the overall performance of the device?

There are 3 approaches commonly used in the industry to model this device:

1 - Mixing plane between the rotor (cage) and the casing (volute)
2 - Frozen rotor approximation instead of mixing plane, and study the different orientations of the rotor (cage) with respect to the non-symmetric section. For this specific case, it seems any orientation will do since there are some many "blades" in the cage that a minor rotation will look the same as the previous configuration.
3 - Full unsteady simulation (perhaps a 4th one will be transient blade row with pitch change, but never done it myself with this use case)

Despite the crude approximations of 1 and 2, the quick solutions (hours) allow engineers to make quick design decisions (helped with additional experimental data) instead of waiting days/weeks for an unsteady solution for a single operating condition. Unsteady is only used when detailed flow features are essential (no modeling error accepted) to make the next decision.

Thank you for your concern.

Where is the vortex, and based on this, we are trying to reduce the noise by improving the inside of the fan case.

So I now simulating transient simulation although one roation.
jins9158 is offline   Reply With Quote

Old   May 25, 2022, 09:06
Default
  #8
Senior Member
 
Join Date: Jun 2009
Posts: 1,775
Rep Power: 31
Opaque will become famous soon enough
Quote:
Originally Posted by jins9158 View Post
Thank you for your concern.

Where is the vortex, and based on this, we are trying to reduce the noise by improving the inside of the fan case.

So I now simulating transient simulation although one roation.
Modeling one rotation will do nothing for you. It may take more than one rotation for the solution to "converge" to its final unsteady state. Unfortunately, you have to run it until a repeatable pattern of some kind can be identified; otherwise, it is just a snapshot of something in development
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.
Opaque is offline   Reply With Quote

Old   May 25, 2022, 21:42
Default
  #9
Member
 
Jin Seok Lee
Join Date: Aug 2021
Posts: 51
Rep Power: 4
jins9158 is on a distinguished road
Quote:
Originally Posted by Opaque View Post
Modeling one rotation will do nothing for you. It may take more than one rotation for the solution to "converge" to its final unsteady state. Unfortunately, you have to run it until a repeatable pattern of some kind can be identified; otherwise, it is just a snapshot of something in development
When I see my processing result about sovle manager, It seems like convergence althoght the impeller rotatate one.

As your advice, I'll see if the convergence goes well.

Thank you for your concern
jins9158 is offline   Reply With Quote

Old   May 26, 2022, 03:46
Default
  #10
Senior Member
 
Gert-Jan
Join Date: Oct 2012
Location: Europe
Posts: 1,815
Rep Power: 27
Gert-Jan will become famous soon enough
Quote:
Originally Posted by jins9158 View Post
Thank you for your concern.

Where is the vortex, and based on this, we are trying to reduce the noise by improving the inside of the fan case.

So I now simulating transient simulation although one roation.



Do you know what the source is for the noise? Does the spectrum tell you anything?
Gert-Jan is offline   Reply With Quote

Old   May 26, 2022, 06:36
Default
  #11
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,641
Rep Power: 142
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
If you are trying to reduce the noise then the transient flow might be the source of it. If the frequency of the flow flapping about in your transient analysis is the same as an important frequency in the noise spectrum then you know that you are modelling an important source of the noise.
Opaque likes this.
__________________
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 Off
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
bad heat transfer results with low y+ me45 OpenFOAM Running, Solving & CFD 0 April 29, 2020 12:56
Workbench results not matching CFD-Post newbietocfd ANSYS 1 December 4, 2019 12:55
Error Interpolating Results onto New Mesh nammeh CFX 1 March 26, 2019 13:08
Simultaneous rotation and translation yields strange results with gmsh BPeters Mesh Generation & Pre-Processing 2 November 19, 2018 03:52
Creating a tool to interpolate results Luis Batista OpenFOAM Running, Solving & CFD 2 April 11, 2013 09:15


All times are GMT -4. The time now is 22:44.