Rotating Region and mesh

[Anonymous]

Hello Everyone,

I'm Quentin Mercier, a french student in mechanical engeneering. Today I come to you cause I have a problem with rotationnal region in CDF simulation.

My purpose is to study a Savonius type wind turbine in dynamics, the huge problem I have is that I can't trust my results, because my mesh totaly influenced my results.

Here is a picture of my work:

                          yellow circle=rotating region

I can give you my boundaries:-pressure imposed at the the outlet

                                                -wind celerity at the inlet (5000mm/s)

                                                -normal celerity = 0 on the other sides of the air volume

I have tried many many many meshes for this problem and here are my results post treated (only rotationnal speed here in RPM during time)

maille=1.00 is my reference mesh (automaticly calculated, approximatively 13,000 elements and maille=0.10 370,000). The 7 first plot has no rotationnal region included and the two last have.

Look at my results ... none of those can be trusted. Maybe you can help me about rotationnal region and with the mesh?

An other question I would ask you is about the inertia you should put in the rotationnal region.

Is this the inertia of the air volume contained in the region?

Or the inertia of my solid?

PS: my rotationnal region have a uniform mesh and I spread it to the entire volume (you can see it 1st picture)

Quentin

[Jon.Wilde]

Hi Quentin.

What you are probably seeing is a model that is not yet mesh independent.

Could you detail your setup? What Boundary Conditions are you using and what size is the wind tunnel?

You only really need a good mesh on the blades and a uniform mesh on the outer surface of the Rotating Region (RR). The RR volume mesh does not have to be uniform.

As you add more mesh, the results should tend towards a solution and gradually become independent of the mesh.

Do you have a plot with the expected result included also?

The inertia should be that of the solid part.

Hopefully some of that helps you progress.

Jon

[apolo_vanderberg]

Quentin,

 One aspect here that can be part of the issue is when you have a notably tighter mesh inside the rotating region versus outside the region we will need to drop our timestep size.

To maintain a proper balance and continuity of the flow field with these models we would want the rotation of the region to be roughly 3-4elements or less.

So in a model such as this where you may have notably refined the mesh on the rotating region, rather than using a more typical 6ºtimestep size, we will need to drop it down further so that the rotation is only a couple of elements each time. This will allow for better continuity and have less impact on the results.

With the image, you may be able to do a lot of the testing on this with a 2D model which would run faster and then allow you to take those lessons learned to the 3D model

[Anonymous]

Hi,

First of all, I'd like to thank you two for you anwsers.

First i'll try to anwser your questions, you asked me to precise my boundaries and my setup.

So my work is to optimize a savonius type wind turbine and for now i'm on the modelisation, I try to simulate the turbine submit to a 5000mm/s wind in the nature ( so no wind tunnel size officialy, I just create a air volume which is 20 times bigger than my turbine dimeter in each direction of space)

Here are my only boundaries conditions:-pressure imposed at the the "outlet" (back of the picture)

                                                -wind celerity at the "inlet" (5000mm/s) (front of the picture)

                                                -normal celerity = 0 on the other sides of the air volume

                                                -Angular movement which depend on the flow (so i do not have the exact angular speed of my turbine...it normaly goes from 0 to 800 RPM!!)

and that's all.

A picture helping you to understand the boundaries

I do not have the realistic solution and response of the turbine through time... but my solutions must converge towards one solution with different meshes, I just need to know the error range.

About my resolution:

->time step used: 0.004s...do I have to decrease this value?!

Ok thank's about the inertia information!

Ok so if I try to recap:

-> No need to put a uniform mesh inside the RR

->Increase the spread of the mesh to get a better continuity

->put the solid inertia on the RR

I thank you a lot, I'll try this tomorrow and give you information in the day!

Quentin

[apolo_vanderberg]

Quentin -

Let me touch on a couple items:

Boundary Conditions -

   I see you have velocity Normal set on 5 of the 6 surfaces - are all of these the same 5m/s magnitude?

Typically we would only assign the inlet (upstream) the Velocity normal as flow will come in normal to this face. We do not need to assign a Velocity = zero to the other faces, this is assumed automatically.

To represent that the air domain is not a wind tunnel, you can assign a component velocity (Vx, Vy or Vz) to the inlet as well as the lateral faces. This might be more appropriate as you would be forcing all 5 faces to have the same vector (for example Vy -5m/s  would be 5m/s in the Neg Y direction)

As far as the Mesh:

We do need a tight mesh in and around the baldes to capture the detail of the flow solution. Whether that is done by assigning a uniform mesh or by refining the distribution, either is acceptable as long as the mesh size will capture the physics.

Timestep size:

  Our typical recommendation is to do 1 blade passage (when there are >3 blades )

  Many times you can run 3-6º per timestep as a starting point.

What i was referring to about adjusting the timestep is taht is that even with 3º timestep there are times where this is not small enough to maintain flow continuity across the linking of the rotating region.

If you put a Plane through the Rotating regino and surrounding air, you can show mesh on that plane and get an idea as to the mesh quality.

A more conservative timestep (and in some cases required) is to have a value small enough such that the rotation of the region is not more than 3 elements of the static fluid around it. To put this in a more mathematical form, if we had 360 nodes around the circumference of the region we would have a node at every 1º and thus the 3º recommendation would be fine. However if our mesh was such that we had ~800 nodes around the circumference we would have a Node every ~0.5º At this point if we had a 3º timestep we would rotate ~6 elements, so to help maintain continuity we would need to drop the timestep size down to ~1º/timestep

Again, considering how you are starting out, you could take a 2D slice through the model and run that to work out the meshing requirements as well as the timestep size and then move to 3D.

[Anonymous]

Hello Apolo,

About my boundaries, I didn't know that speed=0 was a default parameter so i put velocity=0mm/s all around on the right left top and bottom side of the air volume (refer to my last picture). It's pretty hard for my to take a mesh that respect the 3° per time step because my turbine goes from 0RPM to 800RPM...

About the 2D, I wish to get a 2D model but I only have Autodesk Inventor as a CAD program... so no 2D... I may take a freeware which can make 2D model...?

I just arrived to my work, I'll give you info about my testes, I'll make a post in the day!!

[Jon.Wilde]

Morning Quentin,

I thought I would add here. You can model 2D in Inventor. Just use patches to convert a sketch to a surface.

Be sure to have your model on the x-y plane when you read it into CFD. Hopefully this helps you out, certainly if you can run this in 2D it will save huge amounts of time.

[apolo_vanderberg]

As Jon mentioned, Inventor can do 2D.

Make closed sketches and then Insert a Patch (Boundary Patch) to build a planar surface.

This all has to be done on the XY plane for CFD.

As far as the timestep, I'm not following your concern.

If the wind turbine can move upwards of 800RPM, then based on the mesh size we would not want a timestep size that moves more than a handful of elements for rotation (this could be equivalent to 1º/timestep depending on how large/small the mesh is at the interface between the rotating region and the surrounding air).

Granted as we set the timestep size based on the potential for 800RPM, if we are operating at 400RPM the timestep will be more than small enough to maintain continuity.

[Anonymous]

Hello again,

I did some simulations with your advises and that's look better for sure but my solid does not follow the rotating mesh! Just one or two things i have to ask.

->What dimension must my rotating region have to be optimized (compared with my turbine size)?

->should I add an angular movement which depends on the flow to my solid too?

->Is there any solution to get a variable time steps during time or which depend on rotational speed?

->Should I put some intern iteration for each time step?

And my last question is for Apolo and is not a real question, but you answered me on my post about the resistive torque  as a fonction of rotational speed... but i did not understand anything, could you please reexplain to me. That would be nice.^^

I show you some results fast, I'm waiting for a simulation.

[apolo_vanderberg]

Quentin,

1) there isnt a specific "optimal" size of the rotating region. We typically will make is a cylinder that is perhaps 15% larger than the diamter of the blades

2) if using a rotating region you should not be using /assigning Angular motion in the Motion task dialog. For your model it would be either a Rotating Region or Motion, not both.

3) Not specifically, we do not have a method of prescribing a timestep as a function of time or rotational speed. If you'd like you can log that on the IdeaStation as an enhancement request

4) We typically do not need inner iterations for rotating region analyses as long as you have a sufficiently small enough timestep.

I'm not sure what you mean by your solid does not folow the rotating mesh. Unless you mixed motion + rotating region the solid should stay within the region and the region should spin.

For a rotating region you can assign a driving torque to drive the rotation of the turbine. This is typical of when someone knows the motors torque details and wants to see the RPM based on the torque and the wind speed.

What I was suggeting (I have not tried specifically) but trying to use the driving torque in revers, such that you specify a negative torque vs RPM  so that as the RPM increases a larger torque is assigned trying to restrict the rotation.

This again is where 2D would come in hand as you could more easily test this out to see if it provides useful results.

Apolo

[Anonymous]

Ok I will go for a time step that make 1° per step at 800RPM ... but that will be so slow at the begining.

I think, I'll just cut my [0,800] into several parts to get a more efficient simulation.

I'll try the 2D with Inventor in a few, I just wait my computer (sooo slow)^^

Does anyone have an idea to put forward the turbulences which are produced (any option more than activate the turbulence resolution option)? Cause that will help me for my future resolutions.

[apolo_vanderberg]

Yes, while the timestep will be on the smaller side for the initial part of the simulation it will help maintain stability as the RPM grows.

I would start with the default turbulence settings. No specific need to change these.

[Anonymous]

Hello Everyone,

Here are some news from my first problem. It began to work well with the rotating region, but I have some questions left.

My recent purpose was to test on the savonius and with the rotating region different meshes and time step to have an idea of what parameter i should take for my final simulation.

So here are some results rotating celerity:

with a realy weird 7e-4s time step.... turbine do not start up. 

Mesh variation.

I think something is like weird with time step! My physic is not pretty concern by mesh size. But time does play a real important role!! Any idea? (about the 7e-4s timestep....too)

[apolo_vanderberg]

Please attach your support sharefile (*_Support.cfz) so taht I can see your setup

[Anonymous]

Do I have to link my CAO too?

[apolo_vanderberg]

At first glance --

This model still has all the zero velocity conditions, we should remove these

You also have both Motion and a Rotating Region. As I mentioned (and in our help) you would use one OR the other, not both.

The mesh on this model is notably too coarse (especially the mesh on the blades themselves).

I would consider refining the mesh and then re-assessing the details that you have posted.

With small timesteps it can take time to evolve the flow solution and the RPM. I see that you have 150 as the total timestep, we will need quite a bit more than that to evolve this. We also do not need 3 inner iterations , the default 1 for rotating regions would be sufficient.