[hikinam]

Hi, guys

Let me get some help with CFX.

I have a problem with rotating two impellers in water tank.

I did correctly 3D modelling and imported the model in CFX.

I know how to rotate one impellers but I failed to rotate two impellers.

I probably missing something to rotate two impellers in the system.

I have searched the way to solve my problem; however, I could not find it.

Please give me advice on this issue.

Thanks

[ghorrocks]

There are lots of ways to model this:
1) Use two separate rotating frames of reference, with a large stationary frame of reference joining it all up. This is the recommended approach.
2) Use immersed solids - you won't get good boundary layer resolution with this method so it is not recommended.
3) There are other ways but they are even less recommended.

[hikinam]

There are lots of ways to model this:
1) Use two separate rotating frames of reference, with a large stationary frame of reference joining it all up. This is the recommended approach.
2) Use immersed solids - you won't get good boundary layer resolution with this method so it is not recommended.
3) There are other ways but they are even less recommended.

from your suggestions I am willing to follow the way 1.

But the thing is that I don't exactly understand the way 1. It seems that I have to use interface; however, I don't know how to use it.

Can you give me some link to follow ? (eg. videos, documents and the like)

What I always do for simulating 3D modell in CFX is below:

When I run the only one impeller in the tank I just use enclosure and the impeller in the design modeller; thus, meshing, setting, solving and having a look at the result.

IS my way to simulation bad ? I just want to listen to your opinion.

Thanks!

[ghorrocks]

The approach of using 2 rotating frames of reference should work fine. I have not tried it but I know of no problems with it.

Yes, you will have to join the rotating domains to the stationary domains with a GGI. This is not difficult and is well explained in the tutorial examples. Have a look at the CFX tutorial examples for how to set up rotating frame of reference simulations. The axial rotor/stator simulations are the relevant ones to look at.

[hikinam]

I will try the tutorials that you mentioned. If I am stuck again I 'll post questions.

THANKS A LOT.

[urosgrivc]

Hi

I think Glenn was talking about this
https://drive.google.com/open?id=0Bw...nRmMm9yQ1NTWlU

The interfaces are realy simple to set up, just be sure to put the cord sistems directly in the center of rotation or errors will ocure. And when you setup the problem be sure to call the right axis of rotation.

[hikinam]

I think Glenn was talking about this
https://drive.google.com/open?id=0Bw...nRmMm9yQ1NTWlU

The interfaces are realy simple to set up, just be sure to put the cord sistems directly in the center of rotation or errors will ocure. And when you setup the problem be sure to call the right axis of rotation.

Hi, urosgrivc

I have modelled like you draw in the picture. But the thing is that I couldn't set up properly. So I want to know the way to set up before the solving. If you can give me the short cut to know about it. I will appreciate.

Cheers

[urosgrivc]

Make two cord sistems centered in the center of both rotating cilinders

Set up 3 domains
The bigest one, will be stationary.
And the other ones will be rotating. (each around its own cord sistem) with the rotational frequency you will specify.
Axis will be named diferently i think (x1,y1,z1)-> (1.1,1.2,1.3) and for the other cord sistem these will be (2.1,2.2,2.3)


Than you should specify 2 seperate (fluid-fluid) interfaces
And conect rotating domain to the stationary one.
Select the faces that touch (cilinder shaped faces)

If you are doing transient analisis select (transient rotor stator)->(pitch change-NONE)->(GGI)

If you are doing static analisis choose (frozen rotor) but be aware that you will only get results for the rotor position that was set at the beginig (rotors will not turn->frozen)

than set the same for the other interface

[hikinam]

OMG, I was almost there.

I'll try again, looking at your suggestion.

Thanks a lot!!

[hikinam]

Originally Posted by urosgrivc

Make two cord sistems centered in the center of both rotating cilinders

Set up 3 domains
The bigest one, will be stationary.
And the other ones will be rotating. (each around its own cord sistem) with the rotational frequency you will specify.
Axis will be named diferently i think (x1,y1,z1)-> (1.1,1.2,1.3) and for the other cord sistem these will be (2.1,2.2,2.3)


Than you should specify 2 seperate (fluid-fluid) interfaces
And conect rotating domain to the stationary one.
Select the faces that touch (cilinder shaped faces)

If you are doing transient analisis select (transient rotor stator)->(pitch change-NONE)->(GGI)

If you are doing static analisis choose (frozen rotor) but be aware that you will only get results for the rotor position that was set at the beginig (rotors will not turn->frozen)

than set the same for the other interface

Dear grivc

I have got an error.

I HAVE QUESTIONS BELOW:

Q:The bigest one, will be stationary.
-> HOW CAN I SET COORDINATE FOR THE BIGGEST ONE, LETS CALL IT WATER OR FLUID. USE WHICH COORDINATE? BECAUSE I SET TWO COORDINATE ALONG WITH EACH AXIS ATTACHED TO EACH HUB.

Q:And the other ones will be rotating. (each around its own cord sistem) with the rotational frequency you will specify.
-> I GOT THIS

Q:Axis will be named diferently i think (x1,y1,z1)-> (1.1,1.2,1.3) and for the other cord sistem these will be (2.1,2.2,2.3)
-> I GOT THIS

Q:Than you should specify 2 seperate (fluid-fluid) interfaces
-> DO YOU MEAN JUST INSERT TWO INTERFACES?


Q:And conect rotating domain to the stationary one.
-> HOW TO CONNECT?

Q:Select the faces that touch (cilinder shaped faces)
-> THIS PART A BIT CONFUSES ME. SHOULD INTERFACES BE CHOSEN AS CLOSED FACES? I MEAN THAT IF I CHOOSE ONE FLUID I SHOULD CHOOSE THE WHOLE SURFACE WITHOUT THE LEFTOVER OF THE SURFACE.

Q: If you are doing transient analisis select (transient rotor stator)->(pitch change-NONE)->(GGI)
-> I GOTTA RUN TRANSIENT ANLAYSIS

I AM LOOKING FORWARD TO YOUR REPLY

[ghorrocks]

-> DO YOU MEAN JUST INSERT TWO INTERFACES?
Yes, one for each rotating domain.

-> HOW TO CONNECT?
With the interfaces mentioned above.

-> THIS PART A BIT CONFUSES ME. SHOULD INTERFACES BE CHOSEN AS CLOSED FACES? I MEAN THAT IF I CHOOSE ONE FLUID I SHOULD CHOOSE THE WHOLE SURFACE WITHOUT THE LEFTOVER OF THE SURFACE.
You select the face the interface acts over. Have a look at the rotating machinery tutorials for how they do it.

-> I GOTTA RUN TRANSIENT ANLAYSIS
Then use the transient rotor stator model.

[urosgrivc]

I think mr. Glenn cleared it up a bit.
thank you

You must know that if you set up the problem incorectly you will definitly get errors. There is only few ways to get it wright and infinite ways to get it wrong.
You should figure it out now as you are quite close.

I dont qiute like the geometry now thow, as you problably have 5 bodies now and you are complicating the setup proces and meshing.
Rotating domains should have a bit smaller radious, as these are making it hard for you.
Enclosure wals are touching the cilinder shaped parts (tangent) and you have problematic geometry there.
You now have 18 wals just to surround the problem..

-Reduce the diameter of rotating domains (remaining the size of outer domain)
-Make named selections for the surfaces (make seperate selections for those cilinder wals where the interface is going on (side1, side2) it will make it easier for you, as you have to call in those surfaces while setting up the interface.

You have probably inported you geometry, as cilinder surface is divided in half as i can see. Design modeler is a wery good program (best) for manipulating parts, try to use it.

If you`ll have problems...-> ask again

[hikinam]

Originally Posted by urosgrivc

I think mr. Glenn cleared it up a bit.
thank you

You must know that if you set up the problem incorectly you will definitly get errors. There is only few ways to get it wright and infinite ways to get it wrong.
You should figure it out now.

I dont qiute like the geometry now thow, as you problably have 5 bodies now and you are complicating the setup proces and meshing.
Rotating domains should have a bit smaller radious, as these are making it hard for you.
Enclosure wals are touching the cilinder shaped parts (tangent) and you have problematic geometry there.

Q:You must know that if you set up the problem incorectly you will definitly get errors. There is only few ways to get it wright and infinite ways to get it wrong.You should figure it out now.
-> I SEE, NOW I'M STRUGGLING WITH THE MODEL

Q:I dont qiute like the geometry now thow, as you problably have 5 bodies now and you are complicating the setup proces and meshing.
-> YES, IT HAS 5 BODIES

Q:Rotating domains should have a bit smaller radious, as these are making it hard for you.
-> MAYBE BECAUSE OF THE SIZE OF ROTATING DOMAIN I HAVE FACED THE ERRORS.

Q:Enclosure wals are touching the cilinder shaped parts (tangent) and you have problematic geometry there
-> OK I'LL SCALE IT DOWN A BIT

[urosgrivc]

Yes it is quite dificult (to dificult; probably 4 interfaces and a lot more complicated) to set it up with the geometry you had.

Change it and i think you should be able to make it work (errors are pointing to that)
As i can see you havent spent time meshing the domains, mesh is something you will have to do at least a bit better but when you will want results than you will have to do it a lot better.

Ouu!
I see now
You must slice the domain where the interfece is going on (name those cilindrical surfaces as you will call for them in interface setup) you now have owerlaping bodies.
When you will slice it you will have 2 surfaces for the interface, and it will be easy from there on.

I would sugest tutorials to you, so you could understand how setup works, and theory behind it is wery usefull asweal.
As this is one of more basic and simplest of problems.

[hikinam]

Originally Posted by urosgrivc

Yes it is quite dificult (to dificult; probably 4 interfaces and a lot more complicated) to set it up with the geometry you had.

Change it and i think you should be able to make it work (errors are pointing to that)
As i can see you havent spent time meshing the domains, mesh is something you will have to do at least a bit better but when you will want results than you will have to do it a lot better.

Ouu!
I see now
You must slice the domain where the interfece is going on (name those cilindrical surfaces as you will call for them in interface setup) you now have owerlaping bodies.
When you will slice it you will have 2 surfaces for the interface, and it will be easy from there on.

I would sugest tutorials to you, so you could understand how setup works, and theory behind it is wery usefull asweal.
As this is one of more basic and simplest of problems.

THE PATHLINE IS QUITE STRANGE. I think I wrongly set up in the predecessor.

I think the problem is from interface.

Give me some advice on this.

cheers

[urosgrivc]

Hi

Ok so you managed to make it work. good job

Do jou have an opening tipe boundary on the walls of your outer domain?
What are your Boundari conditions?
What are you trying to simulate?
what are your goals for the simulation...

If you are simulating a tank than use wall for BC.
As it looks like flow goes threw the wall now.

It looks like you are using wery large timesteps?

Ou and the mesh on the interface is sliding so you must have a finer mesh there and try to keep the element size the same on both sides of the interface.

[hikinam]

Originally Posted by urosgrivc

Hi

Ok so you managed to make it work. good job

Do jou have an opening tipe boundary on the walls of your outer domain?
What are your Boundari conditions?
What are you trying to simulate?
what are your goals for the simulation...

If you are simulating a tank than use wall for BC.
As it looks like flow goes threw the wall now.

It looks like you are using wery large timesteps?

Ou and the mesh on the interface is sliding so you must have a finer mesh there and try to keep the element size the same on both sides of the interface.

Qo jou have an opening tipe boundary on the walls of your outer domain?
-> NO, I DID NOT DO ANYTHING ON THAT

Q:What are your Boundari conditions?
->NO SLIP WALL

Q:What are you trying to simulate?
-> TESTING AGITATORS IN WASTE WATER TREATMENT

Q:what are your goals for the simulation... 1
-> CHECKING THE STREAMLINE WHETHER IT CAN DISPERSE PARTICLES IN THE WASTEWATER

Q:It looks like you are using wery large timesteps?
->5 SEC, TIME STEP IS 0.1

WELL, I COULD RUN THE MODEL DUE TO YOUR HELP.

CAN YOU HELP ME WITH CHANGING PATH-LINES INTO BETTER LOOKING LIKE THE BELOW LINK.

http://youtu.be/iKVE5jl8cPI

MY WORK=
https://drive.google.com/open?id=0B5...ThFanEzcXgxd2M

[urosgrivc]

+ Smaler mesh elements
+ Smaler time steps
->beter animations
->longer computational times and huge files

I dont know what angular velocity you are using, but video in the link from youtube is definetly around 2-5[°/timestep]

if you are spining the propelers at 10rps that is 3600°/s the timestep for a video like that should be 0,0008s just for comparison.

And its beter to initiate this tipe of transient simulation with results from a static one. as it will take a lot of computational time just to start the flow.


Ou and for strimlines you could use a static analisis (without rotors actualy turning). Hope you have a computer that will manage this transient simulation