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

Isolated fluid region issue

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

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   April 30, 2017, 22:57
Default Isolated fluid region issue
  #1
New Member
 
Dain
Join Date: Apr 2017
Posts: 10
Rep Power: 9
dccfd is on a distinguished road
Hi Everyone,

I am trying to simulate a drone midflight, which can be seen by the attached image and to do this I have used disks to simulate the rotors which I have made as two separate sub domains with an inlet and outlet. When I try and simulate it, I get the below error:

"If the isolated regions do not have the pressure level set either
by the boundary conditions or using a reference pressure equation,
you may encounter severe robustness problems.

This situation may have arisen because a domain interface was not
properly defined during problem setup. Please carefully check
the setup.

The solver will stop now and write a results file. The isolated
regions can be visualised in CFX Post by making plots of the
variable "Isolated Volumes".

If you are sure that the pressure level is set in each isolated
fluid region then you can force the solver to turn off this check
by setting the expert parameter "check isolated regions = f"."

I have been looking on other threads with a similar issue and other people have said that the domains are not connected. Can someone please explain how to resolve this, or should I just force the solver to turn off this check?

Any information you could provide would be greatly appreciated.

Thanks!
Attached Images
File Type: png Overview.PNG (38.6 KB, 25 views)
File Type: png Drone closeup.PNG (7.1 KB, 22 views)
dccfd is offline   Reply With Quote

Old   May 1, 2017, 00:14
Default
  #2
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,767
Rep Power: 143
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
The normal way of modelling something like a rotor blade is using a momentum source term. It is simpler and better models the true flow condition on the rotor.

Why are you modelling this with multiple domains anyway? It looks like it can be done in one domain to me. That would fix the isolated domains error straight away.

But to answer your original question - the error is because you have not put interfaces to join the domains up. You need to put interfaces in to join the domains up. But I would not bother, address the issues I mention in the previous two paragraphs and you will only have 1 domain anyway.
ghorrocks is offline   Reply With Quote

Old   May 1, 2017, 00:52
Default
  #3
New Member
 
Dain
Join Date: Apr 2017
Posts: 10
Rep Power: 9
dccfd is on a distinguished road
Hi Glenn,

Thank you for getting back to me. The reason I did a sub-domain is that I wanted to simulate just air passing through these discs which meant I didn't have to simulate an actual rotating blade which would of had too many variables.

Is it possible to do this with the momentum source term? And if so how would I go about implementing it into CFX?
dccfd is offline   Reply With Quote

Old   May 1, 2017, 02:09
Default
  #4
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,767
Rep Power: 143
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
Quote:
Is it possible to do this with the momentum source term?
Yes. It is also much simpler and more physically correct than the approach you proposed.

For details on how to implement it look in the CFX documentation and search this forum. I do not know of any tutorials which use it unfortunately.
ghorrocks is offline   Reply With Quote

Old   May 1, 2017, 07:21
Default
  #5
New Member
 
Dain
Join Date: Apr 2017
Posts: 10
Rep Power: 9
dccfd is on a distinguished road
Hi Glenn,

Sorry to bother you again but I am quite stuck on these momentum equations. I want to simulate air passing through those discs, going at a velocity of 20m/s, they have a radius of 0.2m, they're 0.01m thick. How would I go about solving the equations for the x-momentum, y-momentum and z-momentum? Or would it be easier to put into cylindrical co-ordinates?

Any advice you could give would be greatly appreciated.
dccfd is offline   Reply With Quote

Old   May 1, 2017, 08:23
Default
  #6
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,767
Rep Power: 143
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
Do you want the rotors to generate a flow of 20m/s? Or do you want to use a fan curve?

You don't solve the equations with momentum source terms, you just add a new factor into the equations which acts as a momentum source (or sink). So continuity and everything else is still conserved, it is just the momentum in the source term region is modified to reproduce the momentum added to the flow by the rotors.
ghorrocks is offline   Reply With Quote

Old   May 1, 2017, 08:45
Default
  #7
New Member
 
Dain
Join Date: Apr 2017
Posts: 10
Rep Power: 9
dccfd is on a distinguished road
I don't have a fan curve for the rotors, so them just producing a flow at 20m/s would be my best bet.

What would be the inputs at this stage?
dccfd is offline   Reply With Quote

Old   May 1, 2017, 19:26
Default
  #8
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,767
Rep Power: 143
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
Make sub-domains of the rotor regions. Use one domain for the entire thing, but the rotors need to be in sub-domains.

Set the momentum source term in the sub domain to:
X: 0
Y: -C*(v-20[m/s])
Z: 0
Source term coefficient: -C

And set C to a large number, say 1e6.
ghorrocks is offline   Reply With Quote

Old   May 4, 2017, 23:28
Default
  #9
New Member
 
Dain
Join Date: Apr 2017
Posts: 10
Rep Power: 9
dccfd is on a distinguished road
Hi Glenn,

Thank you very much for that, everything is running now. Just one more thing, is it possible to input the momentum source as a force rather than a velocity?
dccfd is offline   Reply With Quote

Old   May 5, 2017, 00:19
Default
  #10
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,767
Rep Power: 143
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
Yes, but it is a force per unit volume. You have to be very careful about units with source terms.
ghorrocks is offline   Reply With Quote

Old   May 5, 2017, 00:35
Default
  #11
New Member
 
Dain
Join Date: Apr 2017
Posts: 10
Rep Power: 9
dccfd is on a distinguished road
So I would be able to simulate a thrust in terms of force, as I know the volume of the rotor? What would an example be of the equation for the force?
dccfd is offline   Reply With Quote

Old   May 5, 2017, 00:44
Default
  #12
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,767
Rep Power: 143
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
Well, the total force applied by the source term would be the source term times the volume the source term is applied over.
ghorrocks is offline   Reply With Quote

Old   May 7, 2017, 07:32
Default
  #13
New Member
 
Dain
Join Date: Apr 2017
Posts: 10
Rep Power: 9
dccfd is on a distinguished road
Hi Glenn,

I have be running the simulation with the following values for my source term in the x,y and z:

The X: 0
The Y: -1.992e7 kg m^-2 s^-2
The Z: -1.743e6 kg m^-2 s

With a source coefficient of 1e6, as you recommended.

I used the equations that you said to above, and then broke the 20m/s into its respective component (Y and Z, at 5 degrees).

In my post processing, this is yielding a 600m/s at the rotors which I don't understand why.

Could you please provide some insight as to why this might be happening? And possibly how to correct it?
dccfd is offline   Reply With Quote

Old   May 7, 2017, 18:43
Default
  #14
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,767
Rep Power: 143
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
For those momentum source terms the momentum source term coefficient should be 0.

Read the documentation on setting the momentum source term coefficient - it should be equal to the derivative of the source term function WRT the equation variable.
ghorrocks is offline   Reply With Quote

Reply

Tags
fluid domain, workbench ansys 17

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
How I can introduce my power heat (W) in chtMultiRegionFoam? aminem OpenFOAM Pre-Processing 32 August 29, 2019 02:23
Boundary conditions for two connected fluid region. hut OpenFOAM Running, Solving & CFD 3 June 20, 2019 16:45
[ANSYS Meshing] Fluent Conjugate heat transfer: Temperature at a small fluid region exceed limit RPjack ANSYS Meshing & Geometry 1 June 20, 2019 07:11
[Commercial meshers] Using starToFoam clo OpenFOAM Meshing & Mesh Conversion 33 September 26, 2012 04:04
asking for isolated fluid region flyingd CFX 0 August 1, 2009 10:02


All times are GMT -4. The time now is 18:28.