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

Boundary Conditions for Axial Flow Fan

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

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   August 29, 2020, 05:44
Default Boundary Conditions for Axial Flow Fan
  #1
New Member
 
Zero_g
Join Date: May 2020
Posts: 12
Rep Power: 3
petrosdd is on a distinguished road
Hi. I'm trying to simulate a small axial fan that is placed in a duct, so the whole setup looks kind of like a small wind tunnel (see picture below). The problem is that I've tried multiple boundary conditions, but both total and static pressure always drop after the fan, which is not physically possible. The fan has a diameter of 78mm, rotates at 20000 rpm and has a modified inlet and outlet for better flow characteristics. I've seen suggestions at other threads, but nothing seems to work, except if i set 0 Pt at the inlet and 0 Ps at outlet, then i get a pressure increase but i don't know if this is a valid approach.



Any help would be appreciated.



Thanks in advance.
Attached Images
File Type: png Untitled.png (33.1 KB, 27 views)
petrosdd is offline   Reply With Quote

Old   August 29, 2020, 10:36
Default
  #2
Senior Member
 
Gert-Jan
Join Date: Oct 2012
Location: Europe
Posts: 1,330
Rep Power: 20
Gert-Jan will become famous soon enough
Need more info to be able to help. Please share your output file.
And show where inlet and outlet are.
Gert-Jan is offline   Reply With Quote

Old   August 29, 2020, 14:16
Default
  #3
New Member
 
Zero_g
Join Date: May 2020
Posts: 12
Rep Power: 3
petrosdd is on a distinguished road
Quote:
Originally Posted by Gert-Jan View Post
Need more info to be able to help. Please share your output file.
And show where inlet and outlet are.

Inlet is at the left of the image. The concept is that i need to design a small scale fan (fitted in a 8x8cm casing) in order to replace the one currently used (a CPU fan of the same size) in a small wind tunnel that is used for multiple experiments. In CFX I've imported 4 domains; the inlet duct, the fan, the fan hub, and the outlet duct. For the fan domain, i simulated one blade passage in turbogrid and then did a turbo rotation in CFX pre in order to get the whole domain. I used turbogrid for the fan meshing, mainly to get a good quality hexa mesh. The rest are meshed in ICEM. Also the hub is the only solid domain. Finally, there are 5 interfaces; 2 for the connection of the fan with the ducts (inlet/outlet), same for the hub and one for the hub/fan connection. As i said, I've tested multiple cases, mainly changing the boundary conditions but the results always show a drop in pressure after the fan. Inlet domain is 0.2m long and outlet 0.4m. Longer outlet lengths have been tested but there is no difference in the results.

Last edited by petrosdd; August 30, 2020 at 03:43. Reason: removed link
petrosdd is offline   Reply With Quote

Old   August 29, 2020, 18:18
Default
  #4
Senior Member
 
Gert-Jan
Join Date: Oct 2012
Location: Europe
Posts: 1,330
Rep Power: 20
Gert-Jan will become famous soon enough
Please don't use links to other software. We don't know what's behind. Just keep the output on this forum. Use "Go advanced:" to up load text files.
Also, I am not going to open results files. We're not helpdeks employees. Just share your results in figures like streamlines, velocities, pressure, total pressure, etc.
Gert-Jan is offline   Reply With Quote

Old   August 31, 2020, 04:41
Default
  #5
New Member
 
Zero_g
Join Date: May 2020
Posts: 12
Rep Power: 3
petrosdd is on a distinguished road
Quote:
Originally Posted by Gert-Jan View Post
Please don't use links to other software. We don't know what's behind. Just keep the output on this forum. Use "Go advanced:" to up load text files.
Also, I am not going to open results files. We're not helpdeks employees. Just share your results in figures like streamlines, velocities, pressure, total pressure, etc.



Ok sorry for the link, it's my first time asking and i thought you needed the .res file as well.



The figures below, are from a previous run, with the only difference being the lower rpm of the fan, lower inlet speed and the absence of the modified fan inlet/outlet. So, it's just a straight duct, with a fan and its case in the middle. The flow always moves from left to right in the pictures. Axis of rotation of the fan is Z and ω is negative (-7000rpm). As an inlet BC I've specified the total pressure knowing the inlet velocity (reference pressure is 1 atm so Pt is just 1/2*ρ*V^2, where V=11m/s, thus Pt=74Pa) and outlet BC is static pressure which is set equal to 0. Also, I'm doing a frozen rotor simulation and the SST model is used.



As i said, the fan acts like a turbine, extracting energy from the fluid instead of adding any.



I can't upload the .out file, because the size is too big.

Ps ch.jpg

Pt ch.png

Ps fig YZ.png

Ptot fig YZ.png

slines.png
petrosdd is offline   Reply With Quote

Old   August 31, 2020, 04:49
Default
  #6
Senior Member
 
karachun's Avatar
 
Alexander Karachun
Join Date: Nov 2015
Location: Mykolaiv, Ukraine
Posts: 216
Rep Power: 8
karachun is on a distinguished road
Quote:
Originally Posted by petrosdd View Post
I can't upload the .out file, because the size is too big.
Archive it or remove central part of file, with residuals converhence history.
karachun is offline   Reply With Quote

Old   August 31, 2020, 05:08
Default
  #7
Senior Member
 
Gert-Jan
Join Date: Oct 2012
Location: Europe
Posts: 1,330
Rep Power: 20
Gert-Jan will become famous soon enough
It is not necessary to upload the complete output file. Only the top part with all settings will do.

When plotting streamlines or velocity, use Velocity in Stationary Frame. This helps interpreting the results as a stationay observer standing in the laboratorium. Since streamlines will stop on the fan blades, it is best to let them start on both interfaces and use forward and backward calculation/.

Are you sure your shroud wall is counter rotating? Since it is the rotating domain, it will stand still effectively.

I would set Total pressure or Velocity on the inlet and static pressure 0 [Pa] on the outlet. Then the static pressure on the inlet should be negative. Then increase velocity or decrease total pressure on the inlet values several times to generate a fan curve. Alternatively, increase or decrease the rotational speed. Using affinity rules you can generate other points.

Mostly, my results using CFX are spot on.
Gert-Jan is offline   Reply With Quote

Old   August 31, 2020, 05:30
Default
  #8
New Member
 
Zero_g
Join Date: May 2020
Posts: 12
Rep Power: 3
petrosdd is on a distinguished road
Quote:
Originally Posted by Gert-Jan View Post
It is not necessary to upload the complete output file. Only the top part with all settings will do.

When plotting streamlines or velocity, use Velocity in Stationary Frame. This helps interpreting the results as a stationay observer standing in the laboratorium. Since streamlines will stop on the fan blades, it is best to let them start on both interfaces and use forward and backward calculation/.

Are you sure your shroud wall is counter rotating? Since it is the rotating domain, it will stand still effectively.

I would set Total pressure or Velocity on the inlet and static pressure 0 [Pa] on the outlet. Then the static pressure on the inlet should be negative. Then increase velocity or decrease total pressure on the inlet values several times to generate a fan curve. Alternatively, increase or decrease the rotational speed. Using affinity rules you can generate other points.

Mostly, my results using CFX are spot on.

Setting a total pressure value on the inlet (e.g. my 74Pa) and a static pressure of 0Pa on the outlet, always results in a pressure drop after the fan. Same happens when i set velocity. The only case where there is a pressure rise, is when i set Pt=0 at the inlet and Ps=0 at the outlet, if that's what you mean.But i don't seem to grasp the meaning of it.
petrosdd is offline   Reply With Quote

Old   August 31, 2020, 05:45
Default
  #9
Senior Member
 
Gert-Jan
Join Date: Oct 2012
Location: Europe
Posts: 1,330
Rep Power: 20
Gert-Jan will become famous soon enough
CFX is just trying to solve the case that you set. It cannot think for it self. So if you apply 74 Pa on the inlet, CFX will adapt the flow such that 74 Pa is obtained. No matter what your fan does. It can stand still, rotate clockwise or counter clock wise.

So now you have 74 Pa on the inlet. Apparently that is too much. In fact you are forcing the air through the fan, no matter what it is doing. The fan cannot add anything to it. It is more like a resistance.

Better set 0 [Pa] total pressure on inlet and 0[Pa] static pressure on the outlet. Then let the fan pick up the air by itself. The static pressure on the inlet will drop, giving you the head you are looking for. Then increase or decrease the fan speed to create a fan curve.

So your second case is correct. In that case, you let the fan do the work instead of your boundary condition.
Gert-Jan is offline   Reply With Quote

Old   August 31, 2020, 06:56
Default
  #10
New Member
 
Zero_g
Join Date: May 2020
Posts: 12
Rep Power: 3
petrosdd is on a distinguished road
Quote:
Originally Posted by Gert-Jan View Post
CFX is just trying to solve the case that you set. It cannot think for it self. So if you apply 74 Pa on the inlet, CFX will adapt the flow such that 74 Pa is obtained. No matter what your fan does. It can stand still, rotate clockwise or counter clock wise.

So now you have 74 Pa on the inlet. Apparently that is too much. In fact you are forcing the air through the fan, no matter what it is doing. The fan cannot add anything to it. It is more like a resistance.

Better set 0 [Pa] total pressure on inlet and 0[Pa] static pressure on the outlet. Then let the fan pick up the air by itself. The static pressure on the inlet will drop, giving you the head you are looking for. Then increase or decrease the fan speed to create a fan curve.

So your second case is correct. In that case, you let the fan do the work instead of your boundary condition.
Ok, thanks for the advice, this problem has been bothering me for a long time. One final thought; I get that if I change the rpm of the fan I will get different inlet speeds, because I can derive it from the equations and the velocity triangles. What I don't get, is how does cfx knows this, meaning that if I set 0 Pt at the inlet, then a head will develop. So will it be the correct head for the rpm that I set? In other words when I set 7000rpm, I expect an inlet velocity of 11m/s. Will this be the case?
petrosdd is offline   Reply With Quote

Old   September 2, 2020, 07:19
Default
  #11
Member
 
Henrique Stel
Join Date: Apr 2009
Location: Curitiba, Brazil
Posts: 79
Rep Power: 14
Stel is on a distinguished road
Let me add one thought:

Defining turbomachinery problems in terms of pressure on both the inlet and outlet (either total or static) is a very unstable setup. I would prefer a specified total pressure at the inlet and a specified mass flow rate at the outlet. You know the velocity, so why not setting the mass flow rate? I agree with Gert-Jan that your setup may be resulting in a high mass flow rate so that your fan is choking (not increasing pressure).
Stel is offline   Reply With Quote

Old   September 2, 2020, 09:23
Default
  #12
Senior Member
 
Join Date: Jun 2009
Posts: 1,369
Rep Power: 25
Opaque will become famous soon enough
Quote:
Originally Posted by Stel View Post

Defining turbomachinery problems in terms of pressure on both the inlet and outlet (either total or static) is a very unstable setup. I would prefer a specified total pressure at the inlet and a specified mass flow rate at the outlet. You know the velocity, so why not setting the mass flow rate? I agree with Gert-Jan that your setup may be resulting in a high mass flow rate so that your fan is choking (not increasing pressure).
Partially agree with it; however, we must keep in mind it is case dependent. Examples:
1 - Case where the Pressure Ratio vs Mass Flow Rate curve is nearly flat for an interval of mass flow
In such situations a Total Pressure Inlet+Static Pressure outlet is not a great combination because any mass flow in that interval is nearly a solution; therefore, the solver will wander around that solution space.

2 - Case where the Pressure Ratio vs Mass Flow Rate curve has a sharp drop/increase, i.e. narrow range of mass flow rate represents a large change in pressure.
In such situations, a Total Pressure Inlet+Mass Flow Rate outlet is not a great combination because any value of Static Pressure at the outlet will support the specified mass flow rate during convergence; therefore, the flow may converge very slow or wander around the solution space.

The only known boundary condition pair in ANSYS CFX that adjust itself to both extremes and anything in between is the Total Pressure+Exit Corrected Mass Flow Rate since the effective mass flow rate is adjusted as the solution is converging.

Hope the above helps,
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.
Opaque is offline   Reply With Quote

Old   September 2, 2020, 10:09
Default
  #13
Member
 
Henrique Stel
Join Date: Apr 2009
Location: Curitiba, Brazil
Posts: 79
Rep Power: 14
Stel is on a distinguished road
Quote:
Originally Posted by Opaque View Post
Partially agree with it; however, we must keep in mind it is case dependent. Examples:
1 - Case where the Pressure Ratio vs Mass Flow Rate curve is nearly flat for an interval of mass flow
In such situations a Total Pressure Inlet+Static Pressure outlet is not a great combination because any mass flow in that interval is nearly a solution; therefore, the solver will wander around that solution space.

2 - Case where the Pressure Ratio vs Mass Flow Rate curve has a sharp drop/increase, i.e. narrow range of mass flow rate represents a large change in pressure.
In such situations, a Total Pressure Inlet+Mass Flow Rate outlet is not a great combination because any value of Static Pressure at the outlet will support the specified mass flow rate during convergence; therefore, the flow may converge very slow or wander around the solution space.

The only known boundary condition pair in ANSYS CFX that adjust itself to both extremes and anything in between is the Total Pressure+Exit Corrected Mass Flow Rate since the effective mass flow rate is adjusted as the solution is converging.

Hope the above helps,
This is what you see in the ANSYS Help. From my experience, specifying a mass flow rate always works great (including the region with the sharp drop in pressure, in fact the solver always tends to be robust in this region since it is usually associated with a high mass flow rate so less tendency of flow separation inside the channels). Conversely, the Exit Corrected Mass Flow Rate never worked great for me.

Anyway, I guess that the guy has now some ideas to try and see what could work for him. At the end of the day if you have a bunch of possibilities all of which are physically feasible, the best should be the most stable/fast converging one. Only testing will tell which one will be them.
Stel is offline   Reply With Quote

Old   September 2, 2020, 14:58
Default
  #14
New Member
 
Zero_g
Join Date: May 2020
Posts: 12
Rep Power: 3
petrosdd is on a distinguished road
Quote:
Originally Posted by Stel View Post
Let me add one thought:

Defining turbomachinery problems in terms of pressure on both the inlet and outlet (either total or static) is a very unstable setup. I would prefer a specified total pressure at the inlet and a specified mass flow rate at the outlet. You know the velocity, so why not setting the mass flow rate? I agree with Gert-Jan that your setup may be resulting in a high mass flow rate so that your fan is choking (not increasing pressure).
I've tried specifying total pressure at inlet and mass flow rate at outlet, but the solution always gives a drop in total and static pressure, which I think is not physically possible, considering there is a fan in the setup. The only boundary conditions that give reasonable results, is Pt=Ps=0.
petrosdd is offline   Reply With Quote

Old   September 2, 2020, 15:45
Default
  #15
Senior Member
 
Join Date: Jun 2009
Posts: 1,369
Rep Power: 25
Opaque will become famous soon enough
Have you looked at the rotational velocity vector in CFD-Post?

Is the rotor speed specified correctly? For the software, a fan, a compressor or a turbine looks the same. It is the direction of rotation that defines the behavior. If you are seeing a pressure drop, sounds more like an expansion from inlet to outlet.

It is very common to get the rotation speed confused when the direction axis is specified backwards, or the angular velocity as negative.

Perhaps?
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.
Opaque is offline   Reply With Quote

Old   September 2, 2020, 15:48
Default
  #16
New Member
 
Zero_g
Join Date: May 2020
Posts: 12
Rep Power: 3
petrosdd is on a distinguished road
Quote:
Originally Posted by Opaque View Post
Have you looked at the rotational velocity vector in CFD-Post?

Is the rotor speed specified correctly? For the software, a fan, a compressor or a turbine looks the same. It is the direction of rotation that defines the behavior. If you are seeing a pressure drop, sounds more like an expansion from inlet to outlet.

It is very common to get the rotation speed confused when the direction axis is specified backwards, or the angular velocity as negative.

Perhaps?

Both rotational speeds have been tested. Obviously, when I set the wrong one, the streamlines are chaotic even before the fan.
petrosdd is offline   Reply With Quote

Reply

Tags
axial, boundary, cfx, conditions, fan

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
3D Windturbine simulation in SU2 k.vimalakanthan SU2 14 February 8, 2019 14:43
Waterwheel shaped turbine inside a pipe simulation problem mshahed91 CFX 3 January 10, 2015 11:19
Radiation interface hinca CFX 15 January 26, 2014 17:11
An error has occurred in cfx5solve: volo87 CFX 5 June 14, 2013 17:44
RPM in Wind Turbine Pankaj CFX 9 November 23, 2009 04:05


All times are GMT -4. The time now is 15:38.