Rigid Bodies (Immersed Solids) Boundary Interaction & FSI

ghorrocks · October 19, 2015, 02:50

Please post a cross section of your mesh so we can see the mesh distortion.

But If you have modelled this as a single deformable mesh domain - that is never going to work. You have to put the paddle in a rotating frame and join it to the rest of the mesh with a GGI and a transient rotor/stator interface.

Mohammad80 · October 19, 2015, 04:57

Quote:

Originally Posted by ghorrocks

Please post a cross section of your mesh so we can see the mesh distortion.

But If you have modelled this as a single deformable mesh domain - that is never going to work. You have to put the paddle in a rotating frame and join it to the rest of the mesh with a GGI and a transient rotor/stator interface.

Thank you for your collaboration.
I used a sliding mesh technique as you mentioned and shown in the attached pictures, the mesh before and when the simulation was stopped (I tried different mesh properties but I got same problem).
I have another question, what about the mass moments I must use? is it just the Izz as the rotation is about z axis? or shall I give a values of the three mass moments Ixx, Iyy and Izz? I just want to check that.

Mohammad80 · October 19, 2015, 04:58

and this is zoom in

ghorrocks · October 19, 2015, 20:16

It looks like the outer boundary of the rotor is not rotating and this is causing the deformation.

Have a look at the floating buoy tutorial example for how this sort of rotating sub domain should be set up.

-Maxim- · October 20, 2015, 05:15

---
sorry didn't see the second page

Mohammad80 · October 21, 2015, 06:24

Quote:

Originally Posted by ghorrocks

It looks like the outer boundary of the rotor is not rotating and this is causing the deformation.

Have a look at the floating buoy tutorial example for how this sort of rotating sub domain should be set up.

There is no accessible mesh file or geometry file for that tutorial to go through it in detail. However, thank you at all.

stumpy · October 27, 2015, 15:55

Cut out a cylinder around your wheel, then assign a subdomain to that cylinder. You can set the cylinder/subdomain mesh motion based on the rigid body solution, so the mesh for the whole cylinder will rotate as a rigid body. That will avoid mesh folding problems.
You'll have a Domain Interface between the cylinder and the rest of the mesh. The outer side of the interface should be stationary, while the inner side of the interface will pick up the motion from the subdomain automatically.

Mohammad80 · November 3, 2015, 05:39

Quote:

Originally Posted by stumpy

Cut out a cylinder around your wheel, then assign a subdomain to that cylinder. You can set the cylinder/subdomain mesh motion based on the rigid body solution, so the mesh for the whole cylinder will rotate as a rigid body. That will avoid mesh folding problems.
You'll have a Domain Interface between the cylinder and the rest of the mesh. The outer side of the interface should be stationary, while the inner side of the interface will pick up the motion from the subdomain automatically.

Thank you very much for your help. I did as you advised me and the simulation is going well.
I did a modification to the geometry and added a weir before the wheel, as shown in the attached picture, to compare the results with the first case, but the solution progress stopped after few iterations, when the water starts flowing at the downstream side of the weir and the wheel starts rotating. I don't know if I have a problem with the mesh (I used the multi zone method) or in the CFX problem setup?
Last thing, is it possible to take the fluid as "non-buoyant" to get the same result (the same upstream water profile) that is shown in the following link?

https://www.youtube.com/watch?v=jk6veeHE8To

Frankly, I tried this case but I couldn't get any result and the solution stops after few iterations.
I will be very thankful if you can help me with that.
Thank you again for your message. Best regards.

ghorrocks · November 3, 2015, 18:32

What error message are you getting?

Mohammad80 · November 6, 2015, 03:45

Quote:

Originally Posted by ghorrocks

What error message are you getting?

First of all, I would like to thank you all for your help.
I solved the first problem regarding to the weir added to the geometry.
But I tried to make the simulation close to the reality as that shown in this movie but I couldn't get it.

https://www.youtube.com/watch?v=jk6veeHE8To

The following link shows the animation I got from the simulation:

https://www.youtube.com/watch?v=dW2BzkXd-C4

You can compare the both animations and see the problem with my animation ( I mean the flowing water profile).
The question is how can I improve my simulation analysis to get exactly the same animation as the first one? Best regards.

ghorrocks · November 6, 2015, 05:30

The problems are pretty obvious.

1) Your water level is too low. You need to make the water deeper.
2) Your mesh is too coarse. You need a finer mesh to get the resolution of the interface finer.

Mohammad80 · November 6, 2015, 13:12

Quote:

Originally Posted by ghorrocks

The problems are pretty obvious.

1) Your water level is too low. You need to make the water deeper.
2) Your mesh is too coarse. You need a finer mesh to get the resolution of the interface finer.

I did not give any water level to the setup. I just divided the inlet face into two parts and used the lower part as inlet and I gave only the inlet water velocity as a boundary condition and the outlet was of zero pressure. The question is haw can I specify the water level and make it deep along the channel using the CFX? Regards.

ghorrocks · November 8, 2015, 06:08

The water level is a function of the inlet flow rate, the outlet conditions and any resistances along the way. You adjust these parameters to change the water level.

Mohammad80 · November 9, 2015, 04:05

Quote:

Originally Posted by ghorrocks

The water level is a function of the inlet flow rate, the outlet conditions and any resistances along the way. You adjust these parameters to change the water level.

Thank you for your reply. I will try to change the inlet and the outlet boundary conditions to get the deep water level. Best regards.

Mohammad80 · November 16, 2015, 04:52

Quote:

Originally Posted by Mohammad80

Thank you for your reply. I will try to change the inlet and the outlet boundary conditions to get the deep water level. Best regards.

Good morning
I am sorry because of my too many questions. I faced another problem and I don't know what is the reason. The problem I faced is clearly shown in the attached movies that I got from the simulation that I did. When the water hits the wheel and the wheel starts rotating, the wheel gets upset. I hope you can help me with this problem. Regards.

https://www.youtube.com/watch?v=_jMD...ature=youtu.be

https://www.youtube.com/watch?v=3mK1...ature=youtu.be

ghorrocks · November 16, 2015, 06:15

Looks like divergence. Use a higher quality mesh, smaller time steps, double precision numerics and tighter residuals convergence.

Mohammad80 · November 18, 2015, 04:39

Quote:

Originally Posted by ghorrocks

Looks like divergence. Use a higher quality mesh, smaller time steps, double precision numerics and tighter residuals convergence.

Is there any tips about getting an optimum mesh for the wheel geometry? Frankly, I used a multi zone method for the mesh of the stationary and rotating domains.

ghorrocks · November 18, 2015, 06:52

Based on your images posted before:

* Your mesh is way too coarse. You will need a far finer mesh.
* A hex mesh will be marginally better for free surface flows. If this is a problem don't worry about it, but if you can do hex mesh it will run a little better.
* The key things to think about in meshing are:
** No rapid changes in mesh size. Avoid mesh size transitions greater than about 1.2. Your interface currently has a much larger size ratio than that.
** Aspect ratio close to one. So elements are as close to squares or equilateral triangles as possible.

Mohammad80 · November 23, 2015, 04:30

Quote:

Originally Posted by ghorrocks

Based on your images posted before:

* Your mesh is way too coarse. You will need a far finer mesh.
* A hex mesh will be marginally better for free surface flows. If this is a problem don't worry about it, but if you can do hex mesh it will run a little better.
* The key things to think about in meshing are:
** No rapid changes in mesh size. Avoid mesh size transitions greater than about 1.2. Your interface currently has a much larger size ratio than that.
** Aspect ratio close to one. So elements are as close to squares or equilateral triangles as possible.

Thank you very much for all your notes. Is it possible to discuss something about the wheel?
1. If we suppose that the wheel is a water wheel turbine, Is it possible to predict the electrical power that can be extracted from the spinning wheel? and how?

2. The attached picture shows the solution convergence of the motion and the torque on the rigid body. Do you think the resulted curve of the torque is logical? Is it possible to say that the solution progress is going well and the simulation is good?
If not, how can I improve the simulation setup to get the torque convergence? Regards.

ghorrocks · November 23, 2015, 06:15

1. If you have a model of the mechanical link from the wheel to the generator with all the losses and efficiencies then yes.

2. It looks like a horribly coarse mesh to me, causing it to jiggle around everywhere. The results are bound to be very inaccurate. See my post #38.

October 20, 2015, 05:15		#25
-Maxim- Senior Member Maxim Join Date: Aug 2015 Location: Germany Posts: 413 Rep Power: 13	--- sorry didn't see the second page Last edited by -Maxim-; October 20, 2015 at 05:15. Reason: sorry didn't see the second page

October 27, 2015, 15:55		#27
stumpy Senior Member Join Date: Apr 2009 Posts: 531 Rep Power: 21	Cut out a cylinder around your wheel, then assign a subdomain to that cylinder. You can set the cylinder/subdomain mesh motion based on the rigid body solution, so the mesh for the whole cylinder will rotate as a rigid body. That will avoid mesh folding problems. You'll have a Domain Interface between the cylinder and the rest of the mesh. The outer side of the interface should be stationary, while the inner side of the interface will pick up the motion from the subdomain automatically. Mohammad80 likes this.

Similar Threads
Thread	Thread Starter	Forum	Replies	Last Post
mass flow in is not equal to mass flow out	saii	CFX	12	March 19, 2018 06:21
Difficulty in calculating angular velocity of Savonius turbine simulation	alfaruk	CFX	14	March 17, 2017 07:08
Error finding variable "THERMX"	sunilpatil	CFX	8	April 26, 2013 08:00
Rigid Body State Variables in Solid Immersed Simulation	Hamidreza	CFX	1	October 19, 2009 07:14
how to extend FSI 2D codes to 3D, need advises	abouziar	Main CFD Forum	1	May 30, 2008 05:08

October 19, 2015, 02:50		#21
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,854 Rep Power: 144	Please post a cross section of your mesh so we can see the mesh distortion. But If you have modelled this as a single deformable mesh domain - that is never going to work. You have to put the paddle in a rotating frame and join it to the rest of the mesh with a GGI and a transient rotor/stator interface.

October 19, 2015, 20:16		#24
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,854 Rep Power: 144	It looks like the outer boundary of the rotor is not rotating and this is causing the deformation. Have a look at the floating buoy tutorial example for how this sort of rotating sub domain should be set up.

November 3, 2015, 18:32		#29
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,854 Rep Power: 144	What error message are you getting?

November 6, 2015, 05:30		#31
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,854 Rep Power: 144	The problems are pretty obvious. 1) Your water level is too low. You need to make the water deeper. 2) Your mesh is too coarse. You need a finer mesh to get the resolution of the interface finer.

November 8, 2015, 06:08		#33
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,854 Rep Power: 144	The water level is a function of the inlet flow rate, the outlet conditions and any resistances along the way. You adjust these parameters to change the water level.

November 16, 2015, 06:15		#36
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,854 Rep Power: 144	Looks like divergence. Use a higher quality mesh, smaller time steps, double precision numerics and tighter residuals convergence.

November 18, 2015, 06:52		#38
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,854 Rep Power: 144	Based on your images posted before: * Your mesh is way too coarse. You will need a far finer mesh. * A hex mesh will be marginally better for free surface flows. If this is a problem don't worry about it, but if you can do hex mesh it will run a little better. * The key things to think about in meshing are: No rapid changes in mesh size. Avoid mesh size transitions greater than about 1.2. Your interface currently has a much larger size ratio than that. Aspect ratio close to one. So elements are as close to squares or equilateral triangles as possible.

November 23, 2015, 06:15		#40
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,854 Rep Power: 144	1. If you have a model of the mechanical link from the wheel to the generator with all the losses and efficiencies then yes. 2. It looks like a horribly coarse mesh to me, causing it to jiggle around everywhere. The results are bound to be very inaccurate. See my post #38.