An engineer's pipe flow
From Gerris
Revision as of 22:54, 4 February 2008 Traumflug (Talk  contribs) (Changed mind about grid refinement strategy.) ← Previous diff 
Revision as of 23:07, 4 February 2008 Traumflug (Talk  contribs) (typo) Next diff → 

Line 83:  Line 83:  
* The fluid domain is set to have an inflow boundary condition with fluid velocitiy = 1 to the left and an outflow boundary condition to the right. These two are the cube sides where our modeled pipe starts and ends.  * The fluid domain is set to have an inflow boundary condition with fluid velocitiy = 1 to the left and an outflow boundary condition to the right. These two are the cube sides where our modeled pipe starts and ends.  
* The other four sides of the cube need no boundary conditions as they are fully covered by our solid.  * The other four sides of the cube need no boundary conditions as they are fully covered by our solid.  
  * The initial grid is with a <code>GfsRefine 4</code> rarther coarse (remember how tiny our pipe is). To adapt solid geometry better, the grid is refined with a [[GfsRefineSolid 7]]. As we expect most of the vortices to be near the solod walls, this is fine.  +  * The initial grid is with a <code>GfsRefine 4</code> rarther coarse (remember how tiny our pipe is). To adapt solid geometry better, the grid is refined with a <code>[[GfsRefineSolid]] 7</code>. As we expect most of the vortices to be near the solod walls, this is fine. 
* There is no <code>[[GfsAdaptVorticity]]</code>, as this is easily a source of trouble, at least for beginners.  * There is no <code>[[GfsAdaptVorticity]]</code>, as this is easily a source of trouble, at least for beginners.  
* With <code>[[SourceDiffusion]]</code> the viscosity of the fluid is set to something. I'll be back on this when discussing physical properties.  * With <code>[[SourceDiffusion]]</code> the viscosity of the fluid is set to something. I'll be back on this when discussing physical properties. 
Revision as of 23:07, 4 February 2008
All these oceans with their tides and ships cuising in it are impressive, aren't they? Did you notice how stiff and probably refreshing the breeze around MS Tangaroa is?
Well, as an ordinary mechanical engineer I often have much less impressive things to work out. Like water taps, curved pipes or some sort of flow meter. These smallsized internal flows are, what this tutorial is about. I'll take an example on a simple pipe with two bows in it.
In this tutorial I'll explain how to get more or less arbitrary geometry of internal flows into the Gerris flow solver and how to compute the fluid's behavior there. I'll discuss on what's all this fuss with the Reynolds Number is and how it translates to simple engineering tasks. Finally, I'll do some basic measures in the results and will compare against what a textbook on hydraulics considers as the correct solution.
Computer Aided Design
Undoubtly, different engineers have different tastes about what a good software package for doing CAD is. So, I'll keep this part short and will explain how the result should look, only.
The few steps mentioned here sound simple, but can be a lot of work, of course:
 Create a model of where in your design the fluid flows.
 Create a cube of arbitrary size to cover this fluid model.
 Substract the modeled fluid flow from this cube.
 Make sure the inlet and outlet of this flow reaches the cube's sides.
The result might look like this:
Additional requirements for your CAD work:
 All of the cube's edges should be of equal size (or it wouldn't be a cube).
 It's only one inlet or outlet per cube side allowed.
 Avoid trapped volumes as it's a waste of computing time.
If you have this, save the geometry in STL format. For the sample scripts in this tutorial I'll use doppelbogen.stl
as the file name.
From CAD geometry to Gerris geometry
This step is pretty straightforward as it's mostly a single step to resize the geometry to fit Gerris' fluid domain and to convert from STL to GTS format. Gerris comes along with all the tools needed.
The only caveat is, you have to make the cube slightly larger than the fluid domain as many CAD applications write triangualted data pretty exact, but not exact enough to be unambiguous. Small errors at the 15th digit behind the decimal point are common.
The transform
tool has a handy normalize
option which does resizing and relocating in one step. All put together, a single shell line to do the conversion and transformation looks like this:
tr d '\r' < doppelbogen.stl  \ stl2gts  transform revert normalize  \ transform scale 1.0001 > doppelbogen.gts
The commands in detail:

tr d '\r'
is put in to convert DOS line endings to Unix line endings, e.g. if your CAD runs on Windows. It doesn't hurt if the STL already has Unix line endings. If you ever happen to use a traditional Macintosh text editor, use atr '\r' '\n'
instead. 
stl2gts
does, as the name already hints, the conversion from STL format to GTS format. 
transform revert normalize
handily makes the geometry fit into the minimal Gerris fluid domain, a single GfsBox. For therevert
see next paragraph. 
transform scale 1.0001
oversizes the cube slightly (see above).
Depending on your CAD, the revert
option in one of the transform
commands might be needed to switch the triangles "inside out". The fastest way to find out wether this option is needed or not is to just proceed with it and to redo this step in case you run into calculation errors later. I'll refer to this when explaining how to calculate the flow.
As all commands read from standard input and write to standard output, there's no need for intermediate files.
The result of this step is a file with the name doppelbogen.gts
.
A simple calculation script
There are plenty of examples and descriptions on how to put a Gerris calculation script together, so I'll discuss only few topics here. First, have a look at what I usually use to get started:
1 0 GfsSimulation GfsBox GfsGEdge {} { GfsTime { end = 1 } GfsRefine 4 GfsRefineSolid 7 GfsSolid doppelbogen.gts # The Reynolds number is Re = L * U / Nu. SourceDiffusion {} U 1e3 SourceDiffusion {} V 1e3 GfsOutputTime { istep = 1 } stdout GfsOutputScalarStats { step = 0.1 } stdout { v = Vorticity } GfsOutputScalarStats { step = 0.1 } stdout { v = Velocity } GfsOutputScalarStats { step = 0.1 } stdout { v = P } GfsOutputTiming { start = end } stdout GfsOutputSimulation { step = 0.1 } result%2.1f.gfs } GfsBox { left = GfsBoundaryInflowConstant 1 right = GfsBoundaryOutflow }
Besides a bunch of GfsOutput... stuff, the experienced Gerris user will notice the following:
 The simulation domain is set to a single cube. As you've seen in the chapter before, there's a quick way to make a cube designed in CAD to fit into this single GfsBox. The only drawback is, Gerris insists (for good reason) on calculating a single GfsBox on a single processor. The advantage is, the other processor of your dual core chip will still be available for your entertainmant.
 The fluid domain is set to have an inflow boundary condition with fluid velocitiy = 1 to the left and an outflow boundary condition to the right. These two are the cube sides where our modeled pipe starts and ends.
 The other four sides of the cube need no boundary conditions as they are fully covered by our solid.
 The initial grid is with a
GfsRefine 4
rarther coarse (remember how tiny our pipe is). To adapt solid geometry better, the grid is refined with aGfsRefineSolid 7
. As we expect most of the vortices to be near the solod walls, this is fine.  There is no
GfsAdaptVorticity
, as this is easily a source of trouble, at least for beginners.  With
SourceDiffusion
the viscosity of the fluid is set to something. I'll be back on this when discussing physical properties.
So, fire up your favourite text editor and copy the script above into a file with the name calculation.gfs
. Save the file in the same directory as the doppelbogen.gts
file.
The result of this step is a file with the name calculation.gfs
.
Calculating and viewing results
Ready to enter the number crunching performance test? If so, fire up a Terminal, go to the directory containing the calculation.gfs
and doppelbogen.gts
file and enter:
gerris3D calculation.gfs
That's all!
As of this writing, the calculation for the fluid's time from t = 0 to t = 1 takes almost 4 hours of wall clock time on my fastest CPU. Luckily, we've set the calculation script to write out result files a few times in between, so you can launch GfsView3D
and look what Gerris is doing (and wether it is doing what you intend it to do) a lot earlier.
As Gerris continues to calculate the flow, play around with GfsView, click the buttons available in the toolbar, look which mouse button does what in the main view. The timestep viewed is set by which of the results file you open, all other variants shown (pressure, velocity, turbulence, ...) can be changed by doubleclicking on one of the items in the panel to the left.
One error commonly hits beginners: Gerris computes the "wrong side" of the solid. You easily spot it in GfsView: the pipe where in the fluid should flow is black and everywhere a concretelike solid should be shown colorful fluids appear: Gerris is actually computing something like a thick wire in the wind.
Another possible result of this mismatch is Gerris refusing to start doing fluid calculations at all:
GfsERROR **: root cell is entirely outside of the fluid domain the solid surface orientation may be incorrect aborting...
The reason for this is, different STL modeling software has different conventions about where the "inside" of a triangle representing a solid surface fraction is. The simple solution is, go back to the step converting geometry from STL to GTS and remove the revert
option. Insert it if you didn't use it.
Once you found out wether your CAD package needs the option or not you can stick with your choice with all other STL geometry exported from there.
Is it water or is it air: physical properties
So, now you can almost feel how the fluid flows through your pipe. If you followed the Tips and Tricks section, you've perhaps already some movie showing the development of the flow over time.
But wait! What is this fluid? Is it air? Is it water? Is it pasty like honey? Sure, you know the size of your geometry in CAD, but didn't we scale all this by some magnitudes?
To get some light in this confusion, some very knowledgeable people invented a characteristic number to compare flows against each other: the Reynolds Number. The simple rule is:
 same Reynolds number = same fluid behaviour
So, all we have to do is to calculate the Reynolds Number for our real geometry and to make sure our model features the same number. The number, as given in literature, is:
 Reynolds number = fluid velocity * characteristic length / kinematic fluid viscosity
 Fluid velocity is a number you should already have for your real flow. In our example calculation, the fluid velocity is set to 1.
 Characteristic length is some length of the geometry. For pipes, typically the pipe's diameter is used. Other dimensions work just as fine. For the real flow, you can easily measure a characteristic length. For the modeled flow, it's the same length, multiplied with the scaling factor used when converting CAD geometry to Gerris geometry.
 Kinematic fluid viscosity should be known for the real flow. In the Gerris model, we use it to adjust the Reynolds number to match the real flow.
All this put together, we have to calculate the model's fluid viscosity by the following formula:
 model viscosity = model velocity * real viscosity / real velocity * model length / real length
 = model velocity * real viscosity / real velocity * scaling factor
The same with numbers for our example geometry, water as a fluid and an real fluid velocity of 0.5 m/s:
 model viscosity = 1 m/s * 1.006*10^{6}m^{2}/s / 0.5 m/s * 1 m / 0.050 m
 = 4.024 * 10^{5}m^{2}/s
 Nota Bene: In literature you'll often see the term "dynamic viscosity", expressed in N*s/m^{2} or Pa*s. This is not to be confused with the kinematic viscosity we need here. However, both are related by density:
 kinematic viscosity = dynamic viscosity / density
Fine. Let's insert this number into our calculation script:
[...] SourceDiffusion {} U 4.024e5 SourceDiffusion {} V 4.024e5 [...]
Rename the former results file for later access, then run the calculation again.
Unfortunately, the timestep dt Gerris uses goes down slowly but steadily. After some 1100 steps, it's somewhere at time = 0.171 and td = 1e8 at 4 seconds/step. A rough estimation for the finish at time = 1.0 with the pocket caclulator resulted in something like 10 years. I hit ControlC.
Obviously the solver gets stuck in some detail, so I changed resolution to adapt the solid better:
GfsAdaptVorticity { istep = 1 } { maxlevel = 8 }
This time the adventure lastet two hours only and finished it's self:
... step: 113 t: 0.06447135 dt: 1.000000e09 cpu: 7074.68000000 step: 114 t: 0.06447135 dt: 1.000000e09 cpu: 7097.22000000 GfsERROR **: file timestep.c: line 564 (gfs_diffusion): assertion failed: (par>residual.infty <= par>tolerance) aborting...
Fine. I'll continue the search to find a setting which has an calculation ending.