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

Rian · September 18, 2012, 19:29

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.

Boris_M · September 19, 2012, 05:33

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

Rian · September 19, 2012, 10:40

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

Boris_M · September 21, 2012, 12:18

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.

Rian · October 10, 2012, 11:33

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

Boris_M · October 10, 2012, 11:37

Ok, just post it here, then I'll have a look.

Boris

Rian · October 10, 2012, 13:16

Quote: