CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > FloEFD, FloWorks & FloTHERM

Error unsolved: "Unable to solve the local rotating region"

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

Reply
 
LinkBack Thread Tools Display Modes
Old   September 18, 2012, 19:29
Default Error unsolved: "Unable to solve the local rotating region"
  #1
New Member
 
Rian Lauwrens
Join Date: Sep 2012
Posts: 11
Rep Power: 4
Rian is on a distinguished road
Hi there. I am really new to CFD and have only had introductory training in FloEFD. I don't know if FloEFD is suitable for my application but I'd prefer to use it if possible since my time is quite limited.

The aim of my project is to test two different configurations in a CVT (Continuous Variable Transmission) cover to find out if an inlet improves the cooling of the belt significantly. Here is a few pictures, just for clarification:

(https://www.dropbox.com/s/3t2hs7fzri...Cover_Sim1.JPG)

(https://www.dropbox.com/s/q0mvafah4f...Cover_Sim2.jpg)

The inlet will in the first configuration be closed and in the second one open to see the difference (hopefully it is large). The reason for the odd shape of the inlet is due to space limitations.

After doing a few tutorials and checking the capabilities of FloEFD, this is how I defined my system: (please comment if something is wrong)
Analysis type: External, exclude cavities without flow conditions
Physical features: Heat conduction in solids, Rotation (Local regions)
Fluid: Air and Solid: Aluminum
The rest are all default.

I created a rotating region that fully encloses the driving CVT, the CVT cover was inserted as an insulator. The boundary conditions are "Real Wall" at the CVT cover walls and "Environment Pressure" at the outlet. The inner and outer sheaves of the driving CVT were defined as volume sources with a constant temperature. This will be modified later. The only goal that was defined for now is the mass flow rate at the outlet.

After running the simulation, the error "Unable to solve the local rotating region" still appears. The rotating region has been disabled in the component control.

What may I be doing wrong/can do better? Any comments/suggestions will be really appreciated!! Even if I defined the system incorrectly.

Last edited by Rian; September 19, 2012 at 02:21. Reason: Images didn't post
Rian is offline   Reply With Quote

Old   September 19, 2012, 05:33
Default
  #2
Senior Member
 
Boris Marovic
Join Date: Jul 2009
Posts: 382
Rep Power: 12
Boris_M is on a distinguished road
Hi Rian,

two things I noticed, you are using external analysis yet you close the lids. Is there a different coolant inside the CVT that has no connection to the exterior?
If this is just airflow going in from the outside and is driven by the radial fan of the CVT then you don't need any lids except maybe for the outlet if there is a pipe or so instead leading directly into the environment.
Second, what type of real wall are you using? Do you mean stator wall? There are different settings you can apply for a wall such as roughness or temperature etc.

Also it looks like your rotating region is cutting into the housing at the inlets. You will need a distance to the wall of the planar side of the housing as there are holes in the wall. Also I cannot quite see the shape of your rotating region and the rotating component in it. I think the rotating region might be defined in a bad way. If you could post some images from just the purple component with the rotating region around which is highlighted, this would help to understand how it looks like relative to the rotor.

Also, did you use gravitation and if yes in which direction relative to the axis of rotation is the vector?

Boris
Boris_M is offline   Reply With Quote

Old   September 19, 2012, 10:40
Default
  #3
New Member
 
Rian Lauwrens
Join Date: Sep 2012
Posts: 11
Rep Power: 4
Rian is on a distinguished road
Hi Boris

I understand what you mean with the closing of the lids. I initially wanted to do an internal analysis but changed to external, that's the reason for the lids. I also don't want the air to exit at the inlet, so hopefully I'll get that results. There is no different coolant, so I'll remove the lids.
- Would you recommend an internal or external analysis for this setup?

The type of real wall I am using is stator. The thing is, I want the cover to keep the air inside and I am assuming it as an insulator at room temperature, that is the reason for the "Solid Material", the "CVT_Cover_Insulator".
- Do I need to define the wall differently for what I require?

So do you mean that I need to define the rotating region so that it is far enough (about 5mm) away from the backplate? Because at the moment, it is flat with the plane of the backplate. Below is the image that you requested. At the left is the Rotating region model. I defined it as being 2mm from the rotor (driving CVT), assuming that is where the boundary effects of the rotor will be when rotating. I also mated the rotating region with the rotor with a concentric constraint and coincident constraint at the shaft face.
https://www.dropbox.com/s/pntijzc5s7...Cover_Sim3.JPG
- What did I do wrong in the rotating region? I'm suspecting that I constrained it incorrectly.

I didn't use gravitation, but if it was present it would have been in the x-direction, looking at this sketch:
https://www.dropbox.com/s/3t2hs7fzri...Cover_Sim1.JPG

Thanks for your reply, I appreciate the input so far.

EDIT: I removed the lids and made the rotating region smaller so that there is a space between it and the backplate. Since the system is not enclosed anymore, it gives the following error: "There is no fluid volume in the project. Please check geometry or boundary conditions." Oh and I don't really know what boundary conditions to define since there is no outlet lid to define a mass flow on and since there is "no fluid volume", I can not define stator walls (error: "Face... is not laying on the boundary between solid and fluid region."). I'm kind of stuck right now... I'll try some different approaches in the mean time.

Rian

Last edited by Rian; September 19, 2012 at 12:05. Reason: Unsuccessful attempt with new definitions
Rian is offline   Reply With Quote

Old   September 21, 2012, 12:18
Default
  #4
Senior Member
 
Boris Marovic
Join Date: Jul 2009
Posts: 382
Rep Power: 12
Boris_M is on a distinguished road
Well for external you don't force any specific boundary condition (BC) on an opening that is not present or unknown at such a lid. If there is a pipe attached to the outlet then you can do it but if not it is better to see how the flow really develops and not accidently forcing it to some direction.

No, I just wasn't sure what the real wall BC was used for. You should as you probably know define all walls as stator that are stationary but inside the rotating region.
Also I would suggest you reduce the rotating region by half the distance between your cover and the fan to have a gap between it and the cover. For good results you should use minimum 3 cells between the rotating regions and the top side of the fan blades and also from rotating region to the cover. this is neccessary as there is a software internal BC between outer area and internal rotating region area and you would want to have a small distance and some cells to resolve the flow that comes out of this BC. This is also the reason for the next suggestion...
try to model the rotating region inside the solid where there is no extrusion of some kind that really causes a flow resistance during the rotation such as a fan blade or these bolts I can see as you will have to model the 3 cell rule again. Meaning for the two conical surfaces on the other side of the fan blade area where probably the belt lies, you also have to have 3 cells between the rotor and the rotating region which causes a lot of cells in a 360° model etc. You can avoid this completely on such surfaces by entering the rotating region sketch into the solid where the base of the fan blades is and inside the solid (where you don't need any 3 cells for the BC as there is solid) and come out of the solid again after the second conical face and include the whole bolts up to the end of the model in the rotating region and also go inside the housing of the other end and model it inside the housing back to the center line of the axis of rotation. Now apply all walls that are stator with stator walls and all the rotational walls such as the conicals that would rotate with a real wall that specifies a rotatinal velocity just like the rotating region instead of stator. With that you can save a lot of cells and would cause a moving boundary layer due to the friction on the wall just like in reality.

Try this and it should give you better results, also now the error message should not appear any more if the model is designed as I intended to describe (its hard to do by words).

If you still face the issue of exiting flow at the inlet then it might actually be the case as the fan blades do not have a destinctive flow driving curved form.
Considering your rotational direction, if you would curve the blades against the rotational direction, it would not be nutral to any direction and would also not "shovel" the air towards the center of the rotating shaft and therefore not towards the lids but away from them causing a suction at the lids. They don't have to be complex 3D bent etc. just a little bend against the rotating direction, still simply extruded in y-direction.

Let me know if this worked.

Boris

Edit:
Ups, wasn't finished with your question :-)
Don't use gravity, it wouldn't work here. currently rotating axis and gravity has to be alligned.
Try to use "check geometry" You might have an invalid contact but it would be weird since it worked before. Make sure you use external then if it cannot find the fluid volume it has to be an invalid contact. basically a tangantial contact of some sort, like a cylinder on a flat plate.
Of an external analysis you don't need a boundary condition on any lid. Since it is like in reality sitting in an air volume, the rotation will drive the flow and determine the volume flow. If you want to know the amount of air entering through each lid opeing simply deactivate them in the component control and apply a surface goal to them with volume or mass flow rate or what else you are interested in, maybe fluid temperature between inlet and outlet etc.
Make sure the external space is not too big and adjust it to an area slightly bigger than the model. Mostly a little bigger where there is stron flow going in or out to model the reality better. For example the inlet will suck from the surrounding the air and with that around the corner of the cover into the opening and if there is not a little more space it can give wrong pressure loss cause by this bending around the corner into the opening and that would influence the volume flow etc. The ourlet should be good regarind the distance from the yx-plane of the computational domain.
Boris_M is offline   Reply With Quote

Old   October 10, 2012, 11:33
Default
  #5
New Member
 
Rian Lauwrens
Join Date: Sep 2012
Posts: 11
Rep Power: 4
Rian is on a distinguished road
Hi Boris

Thanks a lot for your detailed reply. I had tests and other projects to finish for the past few weeks, so I'm only getting back to this now.

I understand most of the comments, just not the suggestion on how to model it like you described. I have an idea of what you're saying, so I'll finish it and post an image so you can check if you like.

I'll let you know if it works.

Rian
Rian is offline   Reply With Quote

Old   October 10, 2012, 11:37
Default
  #6
Senior Member
 
Boris Marovic
Join Date: Jul 2009
Posts: 382
Rep Power: 12
Boris_M is on a distinguished road
Ok, just post it here, then I'll have a look.

Boris
Boris_M is offline   Reply With Quote

Old   October 10, 2012, 13:16
Default
  #7
New Member
 
Rian Lauwrens
Join Date: Sep 2012
Posts: 11
Rep Power: 4
Rian is on a distinguished road
Quote:
Originally Posted by Boris_M View Post
No, I just wasn't sure what the real wall BC was used for. You should as you probably know define all walls as stator that are stationary but inside the rotating region.
Quote:
Originally Posted by Boris_M View Post

…Now apply all walls that are stator with stator walls and all the rotational walls such as the conicals that would rotate with a real wall that specifies a rotatinal velocity just like the rotating region instead of stator. With that you can save a lot of cells and would cause a moving boundary layer due to the friction on the wall just like in reality.


The whole purple component (rotor) rotates so should I define all of the surfaces on it as rotating walls? And walls that are not part of the rotating region (i.e. the cover and backplate), should they also be defined as stator walls or not?
As soon as I get an analysis running, I need to define a rotating region around the light blue component as well, which is called the secondary/driven rotor. I hope it doesn’t produce too much problems. It also affects the flow due to rotation, although it doesn’t drive the flow. So I still need to consider that as well.

Quote:
Originally Posted by Boris_M View Post
If you still face the issue of exiting flow at the inlet then it might actually be the case as the fan blades do not have a destinctive flow driving curved form.
Quote:
Originally Posted by Boris_M View Post
Considering your rotational direction, if you would curve the blades against the rotational direction, it would not be nutral to any direction and would also not "shovel" the air towards the center of the rotating shaft and therefore not towards the lids but away from them causing a suction at the lids. They don't have to be complex 3D bent etc. just a little bend against the rotating direction, still simply extruded in y-direction.


I have finished my experimental tests and there was a very definite suction at the inlet and outflow of air at the outlet. It also showed a strong temperature increase as soon as the inlet was closed. Curving the blades might be part of one of my final recommendations for my thesis and it may be a good idea to simulate it and show the difference it makes using CFD.

Quote:
Originally Posted by Boris_M View Post
Try to use "check geometry" You might have an invalid contact but it would be weird since it worked before. Make sure you use external then if it cannot find the fluid volume it has to be an invalid contact. basically a tangantial contact of some sort, like a cylinder on a flat plate.


I have interferences where the backplate and the cover mate. I believe this won't be a problem with the analysis as there will be no fluid flow in those regions. I had to create the interferences to seal the cover tightly since there is some geometry issues and the surfaces not being perfectly flat. I also found invalid contacts due to this same geometry issues. It's solved now and no invalid contacts are present.

I just posted this for now to indicate my progress, I’ll post again as soon as I finish the modelling as you described previously.
Rian is offline   Reply With Quote

Old   October 11, 2012, 17:20
Default
  #8
New Member
 
Rian Lauwrens
Join Date: Sep 2012
Posts: 11
Rep Power: 4
Rian is on a distinguished road
Hi Boris

Please see the attached images below:

https://dl.dropbox.com/u/103182017/C...g%20region.jpg

The model is as I understood your description. I also added a few notes:
A-E - To help with the description of certain regions
Real Wall BC's - Please let me know if the way it is defined in the sketch is how you tried to explain it?

Is the model fine? I'll be able to run a simulation later this week again. Thanks for your help!
Rian is offline   Reply With Quote

Old   October 15, 2012, 10:34
Default
  #9
New Member
 
Rian Lauwrens
Join Date: Sep 2012
Posts: 11
Rep Power: 4
Rian is on a distinguished road
I started with simulation again. This was after I changed the model and defined the 4 reall wall BCs as in the previous message. There is also one temperature heat source.

I first generated the mesh to see how it looks before I try to solve for it. I left the initial mesh settings at default at a result resolution level of 3 and FloEFD crashed, giving me the error:
"Not enough memory to continue the calculation. Failed to allocate requested continuous memory block of 18.515 MB."

The system I am running on has a Quad core CPU at 2.7 GHz and RAM of 3.25 Gb. I am running from a flash disk and not the C-drive which may produce problems.

As a second approach I lowered the result resolution level to 1, just to see if it can mesh. After 40 minutes, it finished and according to me the mesh was quite well defined since it was small at the areas of high detail. I then tried to solve it, after which I got the error (after about another 30 minutes) of:
"SOLVER ABNORMALLY TERMINATED".
Just for extra info:
Fluid cells: 69531
Solid cells: 35307
Partial cells: 107191
Iterations: 0
No Warning messages

Does this mean I have to start to consider using control planes? I guess the system is too roughly defined for it to solve.

As a third approach, I also suppressed the 4 BCs to see what happens and I got the "memory problem" again.

Does anyone recommend that I use control planes for the mesh or will that only increase the required memory? Any comments or suggestions will be appreciated!
Rian is offline   Reply With Quote

Old   October 16, 2012, 07:58
Default
  #10
New Member
 
Rian Lauwrens
Join Date: Sep 2012
Posts: 11
Rep Power: 4
Rian is on a distinguished road
Quote:
Originally Posted by Rian View Post
Does this mean I have to start to consider using control planes? I guess the system is too roughly defined for it to solve.

As a third approach, I also suppressed the 4 BCs to see what happens and I got the "memory problem" again.

Does anyone recommend that I use control planes for the mesh or will that only increase the required memory? Any comments or suggestions will be appreciated!
Just to give feedback. Defining control planes has quite a signicant effect. I defined them in the positions where I thought it would be best and the meshing was perfect in the areas of interest, with 3-4 cells between the rotating region and solid areas.

Suppressing all the parameters, including BCs, enables it to solve without crashing again. It was good to see that it can solve! As soon as I enable only one of the BCs, it crashes again.

I assume this problem is either out of the reach of FloEFD or you need some sort of super-computer to run it. Don't really know what else to do now. If anyone has some comments that may help, please post them!

Thanks.
Rian is offline   Reply With Quote

Old   October 22, 2012, 09:21
Default
  #11
Senior Member
 
Boris Marovic
Join Date: Jul 2009
Posts: 382
Rep Power: 12
Boris_M is on a distinguished road
Hi Rian,

sorry I was away a few days and haven't had the chance to help you.
So lets start with your second comment from the 10th Oct.


No, rotating walls are only applied if it is a rotational symetric wall that is rotating and not inside or partially cutting (but completely rotating) a rotating region. For example the rotating walls of the V shaped sheave if they were not inside the rotating region.
Also stator walls should only be defined if they are inside or cutting a rotating region but are part of a stator. Also here they should only enter the rotating region if they are rotational symmetric without any extrusions.


No, you don't need a super computer to run it. The model might be at the limit of your computer depending if you use a 32 or 64 bit system. the automatic settings are often hard to control for the cells that you generate. Often it gets you a perfect mesh but if dimensions are too big and you have some small features you can have a too coarse mesh. Also you can have very fine cells along edges causing more cells than you would need and therefor too high computational time for the solver compared to an optimized mesh.

I cannot really tell about the mesh you created without an image of it. The numbers are not too high for a 32 bit problem but that was for a very low mesh level for some qualitative results and the solver can have some reasons to crash. I cannot really tell without the model, seeing all the BCs and checking the mesh settings. Can you provide me with the model? You can send me a PM with a download link so I can have a look if that is ok with you.


Boris
Boris_M is offline   Reply With Quote

Old   October 22, 2012, 13:21
Default
  #12
New Member
 
Rian Lauwrens
Join Date: Sep 2012
Posts: 11
Rep Power: 4
Rian is on a distinguished road
Thanks for your response Boris.

I managed to solve the problem by first simplifying the geometry and then reading up about meshing, etc. I also changed the rotating region and rotating walls to more or less how you specified it. It shows very good results and compares quite good to my experimental results. I handed the project in today and it was part of my final year thesis. So I am finished for now.

If you (or anyone else) would like to see how I solved the problem, I would be happy to post my procedures and some images of the meshing as well as the results. Just let me know!

Rian
Rian is offline   Reply With Quote

Old   October 23, 2012, 03:23
Default
  #13
Senior Member
 
Boris Marovic
Join Date: Jul 2009
Posts: 382
Rep Power: 12
Boris_M is on a distinguished road
Hi Rian,
it would be great if you could share some information. I think some people here might like to hear more about it. Thank you.

Boris
Boris_M is offline   Reply With Quote

Reply

Thread Tools
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 On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
How to write k and epsilon before the abnormal end xiuying OpenFOAM Running, Solving & CFD 8 August 27, 2013 15:33
"Unable to solve the local rotating region" Walle FloEFD, FloWorks & FloTHERM 3 September 19, 2012 05:28
question about governing equation in CFX using rotating/non rotating reference frame rystokes CFX 0 January 12, 2010 07:14
BlockMeshmergePatchPairs hjasak OpenFOAM Native Meshers: blockMesh 11 August 15, 2008 07:36
Modeling in micron scale using icoFoam m9819348 OpenFOAM Running, Solving & CFD 7 October 27, 2007 00:36


All times are GMT -4. The time now is 19:11.