Induced Flow through Rotation of Solid

marcel_jay · February 25, 2016, 11:04

Hello Community,

I am quite confused about how to model a Rotation. I have a solid body (consisting of like 5 solid domains) which is hot and should be cooled through rotation.
The Solids are surrounded by a cylindrincal enclosure, with inlets on the top and bottom an outlet on the cycldrincal wall with relative pressure of zero (i tried openings as well, but didnt converge very well).
Attached is a picture from the ANSYS Power Point Manual "Chapter 12 Moving Zones", which kind of shows what I'm modelling.

At first I tried to set the solid to rotate and the fluid to be stationary which did nothing. Then I gave the surrounding domain around it a rotation, and the solid stationary,
which kind of worked, seeing these swirling streamlines. I already thought that approach might be strange, as in Reality, the solid is hitting the air and causing the flow.
But then I saw that in my very large cylindrical domain, that the air-velocities becomes greater to the outside of the enclosure. Hence, I assume the fluid motion is caused by centrifugal forces only.

CFX Tutorial 17 "Flow in a Mixing Vessel" says, in accordance with the power point slide that you need Multiple Frames of Reference when you have baffles.
I Don't have baffles though. In realitiy, it's just this rotating fan in a huge room of air.

There a nice swf-file tutorial I found which models something similar:
https://www.researchgate.net/file.Po...01442282409241

In this video the "solid propeller" is only a Wall boundary in the flow field. In my case though it's an interface for the CHT, but should still be treated as a wall if I'm right.
But then again, why isn't the velocity close to the solid highest and gradually becomes lower to outer cylinder-wall?

This kind of practice with a flow domain in a larger flow domain seems like an odd trick to me, which still can't be very realistic.
If anybody could tell what I need to do or what's wrong in my way of thinking, I would be thankful.

Best regards
Marcel

ghorrocks · February 25, 2016, 18:22

The swf you linked to is modelling a propeller spinning in a free-field, that is there is no nearby walls. So it is only applicable if your rotor spins in open space. If it was modelling a pump then it would need to include the shroud, diffuser, volute and all the other bits to make it work.

You can do CHT simulations of rotating bodies. This has been supported since CFX v15 I think. If you are on a version of CFX earlier than V15 this will be quite hard - a good excuse to upgrade.

Milsey · February 26, 2016, 00:24

You could set your model up with your rotating components as an immersed solid as a separate domain if you have ANSYS 17. Alternatively you can use a boolean operation to make a cut where your solid bodies are and rotate the cuts as your rotating domain.

Didn't have the downloads to watch the video sadly so you may already be trying these.

marcel_jay · February 26, 2016, 07:20

First of all, thank you both for you answer.

Quote:

Originally Posted by ghorrocks

The swf you linked to is modelling a propeller spinning in a free-field, that is there is no nearby walls. So it is only applicable if your rotor spins in open space.

The only defined boundaries are the interface (through which massflow is apparently possible) and the propeller, which are defined as walls.
I am modelling a free field, which is cylindrical and not cubic, so why the need for an extra domain?

If I model air in a cylinder which i gave rotation, every fluid-particle would be set to motion even without a "propeller wall" in the middle. So even with the propeller, particles that are already in the domain would start rotating without touching the propeller. This wouldn't match reality.

Quote:

Originally Posted by Milsey

Alternatively you can use a boolean operation to make a cut where your solid bodies are and rotate the cuts as your rotating domain.

Yes, I think that's what is shown in the video, the cuts are represented as walls that rotate with the rotating domain.

Quote:

Originally Posted by Milsey

You could set your model up with your rotating components as an immersed solid as a separate domain if you have ANSYS 17.

I saw this approach in a video before, but since I modelled an enclosure, I would have to remodel. Neither I am sure what will happen with the interfaces I need for heat transfer.
As seen in this youtube video, no connections in meshing are created. https://youtu.be/qJyJhz4bEQI

ghorrocks · February 26, 2016, 07:27

Quote:

I am modelling a free field, which is cylindrical and not cubic, so why the need for an extra domain?

Very good

. You are correct, it is not required. You can just use a single rotating domain in that case and no need for interfaces.

Quote:

If I model air in a cylinder which i gave rotation, every fluid-particle would be set to motion even without a "propeller wall" in the middle. So even with the propeller, particles that are already in the domain would start rotating without touching the propeller. This wouldn't match reality.

Oops, I think you missed the point on this one. The rotating frame of reference is just that - a frame of reference. It does not influence the fluid, it is just the coordinate system you measure the fluid relative to. So if you have a rotating frame of reference but the fluid is really stationary, then the fluid is counter-rotating at the same velocity as the rotating frame of reference such that its velocity in the global frame of reference is zero.

So you use frames of reference to define mesh motion, not fluid motion.

Immersed solids - for any surface which you want good boundary layer accuracy you should not consider immersed solids. Most blade style rotating machines require accurate boundary layer modelling, so that means immersed solids is not a good option.

Your device looks like a ship's propeller, so I would think immersed solids is not a good choice for that.

marcel_jay · February 29, 2016, 08:56

Quote:

Originally Posted by ghorrocks

Oops, I think you missed the point on this one. The rotating frame of reference is just that - a frame of reference. It does not influence the fluid, it is just the coordinate system you measure the fluid relative to. So if you have a rotating frame of reference but the fluid is really stationary, then the fluid is counter-rotating at the same velocity as the rotating frame of reference such that its velocity in the global frame of reference is zero.

Yes maybe I missed the point completely

So I set up quickly this test simulation with a cylinder with nothing in it and all faces are openings. Velocity in Post shows me movements.
What you are suggesting is that those are just relative velocities and therefore in the middle they are low, since the tangential velocity of the frame in the middle is zero? (Picture is attached)

So then I was thinking, if Glenn was right, maybe I need to just plot another variable? Cause I really want to see the absolute velocities to comprehend the flow of my model.
When I plotted "Velocity in stationary frame" in my dirty test simulation there is some radial flow, which also confuses me... numerical error?

Cheers
Marcel

ghorrocks · February 29, 2016, 17:48

If the outside walls are free slip walls then "Velocity in Stationary Frame" should go straight through, with a small allowance for numerical error. This error can often be reduced using the "Alternate Rotation Model" - have a look in the documentation if you want an explanation of what this option means.

If the walls are no slip walls rotating with the frame of reference (which is the default condition) then this will generate secondary flows and cause vorticies to form. I suspect this is what you are seeing.

The outside walls need to be either free slip walls or Counter-rotating walls (this means they will be stationary in the absolute frame of reference).

marcel_jay · March 8, 2016, 07:45

Quote:

Originally Posted by ghorrocks

If the walls are no slip walls rotating with the frame of reference (which is the default condition) then this will generate secondary flows and cause vorticies to form. I suspect this is what you are seeing.

The funny thing is, the shown setup had an opening condition, which is not likely to cause any friction or am I wrong? So it's a flow leaving the domain. A quick CFD Post analysis showed it's only about 12 nanograms out of the domain (in a 20 liter volume cylinder).

As we are at this point there is something I haven't understood yet: does it make a difference if you set the boundaries opening, inlet and outlet to rotate?

Cheers and thank you for you help
Marcel

ghorrocks · March 8, 2016, 18:56

Try it and find out.

marcel_jay · March 10, 2016, 09:40

In this simple setup there seems to be no difference in the results, however I really wonder why the option in the Basic Settings even exists.

Glenn I'm very thankful for your time and help. I appreciate it a lot.

Cheers
Marcel

Opaque · March 10, 2016, 10:52

May I ask which Basic Settings you are referring to ?

If you are referring to the Frame Type setting, you may have misinterpreted the setting. If it is set to Rotating, it indicates that the information given on the boundary conditions is interpreted in the Rotating Frame, not that the boundary is rotating.

For certain variables like Pressure, or Temperature it does not mean much, but for Velocity, Total Pressure or Total Temperature it is meaningful.

Hope the above helps,

February 25, 2016, 11:04	Induced Flow through Rotation of Solid	#1
marcel_jay Member Marcel Jay Join Date: Jun 2014 Location: Berlin Posts: 52 Rep Power: 12	Hello Community, I am quite confused about how to model a Rotation. I have a solid body (consisting of like 5 solid domains) which is hot and should be cooled through rotation. The Solids are surrounded by a cylindrincal enclosure, with inlets on the top and bottom an outlet on the cycldrincal wall with relative pressure of zero (i tried openings as well, but didnt converge very well). Attached is a picture from the ANSYS Power Point Manual "Chapter 12 Moving Zones", which kind of shows what I'm modelling. At first I tried to set the solid to rotate and the fluid to be stationary which did nothing. Then I gave the surrounding domain around it a rotation, and the solid stationary, which kind of worked, seeing these swirling streamlines. I already thought that approach might be strange, as in Reality, the solid is hitting the air and causing the flow. But then I saw that in my very large cylindrical domain, that the air-velocities becomes greater to the outside of the enclosure. Hence, I assume the fluid motion is caused by centrifugal forces only. CFX Tutorial 17 "Flow in a Mixing Vessel" says, in accordance with the power point slide that you need Multiple Frames of Reference when you have baffles. I Don't have baffles though. In realitiy, it's just this rotating fan in a huge room of air. There a nice swf-file tutorial I found which models something similar: https://www.researchgate.net/file.Po...01442282409241 In this video the "solid propeller" is only a Wall boundary in the flow field. In my case though it's an interface for the CHT, but should still be treated as a wall if I'm right. But then again, why isn't the velocity close to the solid highest and gradually becomes lower to outer cylinder-wall? This kind of practice with a flow domain in a larger flow domain seems like an odd trick to me, which still can't be very realistic. If anybody could tell what I need to do or what's wrong in my way of thinking, I would be thankful. Best regards Marcel

Similar Threads
Thread	Thread Starter	Forum	Replies	Last Post
About Some Concepts:Laminar flow, turbulent flow, steady flow and time-dependent flow	Jing	Main CFD Forum	8	October 5, 2018 18:02
Review: Reversed flow	CRT	FLUENT	1	May 7, 2018 06:36
Flow over a flat plate as an immersed solid	hamed.majeed	CFX	4	September 8, 2016 15:40
gas solid flow in circulating fluidized bed with different gas velocity	kongl1986	FLUENT	2	April 5, 2012 23:23
gas solid flow in a pipe	Pandu	CFX	0	July 30, 2001 17:53

February 25, 2016, 18:22		#2
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,870 Rep Power: 144	The swf you linked to is modelling a propeller spinning in a free-field, that is there is no nearby walls. So it is only applicable if your rotor spins in open space. If it was modelling a pump then it would need to include the shroud, diffuser, volute and all the other bits to make it work. You can do CHT simulations of rotating bodies. This has been supported since CFX v15 I think. If you are on a version of CFX earlier than V15 this will be quite hard - a good excuse to upgrade.

February 26, 2016, 00:24		#3
Milsey New Member Millen Join Date: Jan 2016 Posts: 7 Rep Power: 10	You could set your model up with your rotating components as an immersed solid as a separate domain if you have ANSYS 17. Alternatively you can use a boolean operation to make a cut where your solid bodies are and rotate the cuts as your rotating domain. Didn't have the downloads to watch the video sadly so you may already be trying these.

February 29, 2016, 17:48		#7
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,870 Rep Power: 144	If the outside walls are free slip walls then "Velocity in Stationary Frame" should go straight through, with a small allowance for numerical error. This error can often be reduced using the "Alternate Rotation Model" - have a look in the documentation if you want an explanation of what this option means. If the walls are no slip walls rotating with the frame of reference (which is the default condition) then this will generate secondary flows and cause vorticies to form. I suspect this is what you are seeing. The outside walls need to be either free slip walls or Counter-rotating walls (this means they will be stationary in the absolute frame of reference).

March 8, 2016, 18:56		#9
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,870 Rep Power: 144	Try it and find out.

March 10, 2016, 09:40		#10
marcel_jay Member Marcel Jay Join Date: Jun 2014 Location: Berlin Posts: 52 Rep Power: 12	In this simple setup there seems to be no difference in the results, however I really wonder why the option in the Basic Settings even exists. Glenn I'm very thankful for your time and help. I appreciate it a lot. Cheers Marcel

March 10, 2016, 10:52		#11
Opaque Senior Member Join Date: Jun 2009 Posts: 1,880 Rep Power: 33	May I ask which Basic Settings you are referring to ? If you are referring to the Frame Type setting, you may have misinterpreted the setting. If it is set to Rotating, it indicates that the information given on the boundary conditions is interpreted in the Rotating Frame, not that the boundary is rotating. For certain variables like Pressure, or Temperature it does not mean much, but for Velocity, Total Pressure or Total Temperature it is meaningful. Hope the above helps,