[bertozzi_marco]

hallo Everybody

here you can find a simple simulation of stirlig alpha engine.
With the same condition I've made a theorical calculation and I expect
to gain positive work.
With CFX simulation there isn't any positive work

Any advice ?

[ghorrocks]

Please post an image of what you are simulating.

Why do you have gravity enabled? What does it do?

This sounds like an FAQ: http://www.cfd-online.com/Wiki/Ansys..._inaccurate.3F

[bertozzi_marco]

Gravity does nothing, it's only for work buoyant model.

in this tread you see the model I l'like to simulate
http://www.cfd-online.com/Forums/flo...ng-engine.html

I don't think to find something useful in FAQ, the model give resultrs
very different from theoric calculation, I expect a power of 1.5 / 2 Kw
and the model give -0.2 Kw negative work

If you review results you see the fluid doesn't gain enough heat from bonduary,
and pressure doesn't increase during expansion.

Is known this type of engine work for sure with condition you see in the model

[ghorrocks]

What do you mean by "work buoyant model"?

Can you post an image of your geometry, your mesh and the flows you are getting (particularly if you think some part of the flow looks wrong).

[bertozzi_marco]

Pressure: http://youtu.be/l-2CPJg-llU

Temperature: http://youtu.be/edIgvUl11rc

and images of geometry and mesh

[ghorrocks]

Your mesh is too coarse. Your heat transfer will be miles off with a mesh that coarse - which is exactly what you have found. If you had gone through the points described in the FAQ you would have worked that out for yourself.

[bertozzi_marco]

I will do a simple model to understand only the influence of the coarse mesh
and I will post the results......
thanks for the moment....

[bertozzi_marco]

here you find simulation with poor mesh: http://youtu.be/ln_CnugS1mI

and with fine mesh: http://youtu.be/xtPTV8xm6Fc

there are some difference of about 100 k at the end of simulation, but the question now is how fine should be mesh?
very fine mesh need a lot of CPU time, poor mesh need less CPU time
but is inacurate, so there are some guidelines to deside appropriate mesh
refinemet ?

[ghorrocks]

This is all discussed in the FAQ I posted right at the start

In short: You need to perform a sensitivity analysis on mesh size. Choose a parameter of importance to you (maybe the work generated) and generate a series of meshes, each with different mesh size. And don't make it different by 10%, the difference needs to be large, like halving the edge length. Do simulations of all these meshes and plot your parameter versus mesh size. Hopefully it will start converging on a value as the mesh is refined. Then you choose an accuracy you are happy to live with and read off the mesh size required to give it.

There are more sophisticated methods of doing this (grid refinement index etc) which are highly recommended and mean you can do this quicker with less simulations - but the concept is the same.

And yes, this will inevitably lead to big simulations, and probably lead to simulations too big to run on a desktop PC. That is why people make supercomputers to run CFD simulations. It is because they have to use a computer that big to run it.

[bertozzi_marco]

I understand,
About the model I'd like to explore, I think the heat transfer be the core
parameter for the simulation. Because the simulation of the engine will
take in account a lot of variables, I can use a simple model like you have
seen in the videos before, to explore only the heat transfer phenomena.
Once found the appropriate mesh size I can transfer it to the engine model
and obtain a valid solution with one run. What is your opinion about ?

[ghorrocks]

Yes, that is a good plan - Providing the heat transfer is the key parameter in the simulation. Even if that is not the case it is a good start.

Don't forget fluid flow along the pipe and in the entry/exit will also contribute.

[bertozzi_marco]

Hallo
here you can find results of simple analisys of a can heated for 3 seconds.
here you can find the immages of the most fine and coarse mesh of
the sensitive analisys, also the table of the sensitive analisys with
the target parameter, the target parameter is the temperature at center
of the can

The strange thing is that the temperature doesn't vary a lot varying the
quality of the mesh, why ?

[ghorrocks]

This is showing that for the case you have modelled you are reasonably accurate. But this case has no flow so the only thing causing heat transfer is conduction - and conduction does not include the tricky non-linear terms which are difficult to get mehs convergence for. This is why you have easily got mesh convergence in this case.

But I think you will find your actual engine case has the majority of the heat transfer from convection effects, and that will be much more sensitive to mesh density. So it is a matter of finding a simple analogy which contains all the important physics but is not too complex to model properly.

I would add an inlet and exhaust port with constant flow to your cylinder. Make the flow rate of the same magnitude as the flows you expect in the engine. Then repeat the mesh sensitivity study on this case and I suspect you will find you will require a considerably finer mesh.

[bertozzi_marco]

Here the simulation according your advices,
There is a notable difference of the temperature contour.
But at the outlet the mean temperature isn't so different.

I'd expect a big variation of temperature in the outlet tube,
I don't know if this will vary a lot the work of the engine, is clear the
distribution of temperature is better.

I attach also ccl for your kind check

[ghorrocks]

The temperature change is limited to just the boundary layer in the cylinder, so not much has happened yet. You need to run this for more time so the temperature effects convects into the main flow. Better still, run it as a steady state simulation and get the steady state result.

[bertozzi_marco]

I have a question about buoyant model, this model
Enable different density of fluid to float over when it is The case,
But if I have fluid speed enough to make the different density negligible
In front of the turbolence due to the speed, should I Enable buoyancy?

[ghorrocks]

The question to ask is actually - given the flow velocities in my model, will buoyancy make a significant difference? If the answer is no (which your last post seems to imply) then you can turn buoyancy off.

[bertozzi_marco]

yes it is, but I'd like to understand the concept in general,
I'd think the buoyant model will be usefull when the speed of
fluid is very low or comparable with the buoyant turbolence.
So I think that where is fluid driven from high speed volume variation
(like piston engine) the buoyant model could be disabled.

[ghorrocks]

If you are in doubt then activate buoyancy. In forced convection flows it does not add much (if anything) to simulation time. It only adds to simulation time in low speed simulations - but that is because it is doing what it is meant to be doing and generating flows.

[mcout]

https://www.youtube.com/watch?v=edIg...ature=youtu.be

I need to make a simulation like this. Its so important for me please help me for this. Can I take Ansys Workbench file for this? Please