Groovy BC - time dependend Inlet
 

hi all,

i am trying to make my first own BC with groovy. I made my own scalarIcoFoam where i implemented just one scalar-field to simulate color in water or sth. like that (without diffusion).

So i wanna build a pulsating inlet for the new scalar field.

The value should switch every 0.5 seconds from value 0 to 1 and after 0.5 from 1 to 0. I think its a very simple implementation with groovy but i need some help.


Thx in advance
Tobi

Further question:
is it possible to create a bc for the inlet that only a few faces use that inlet condition (compare the picture | red line).
I wanna set just a few fields with value 1 to the inlet that i get a little fiber, but i dont know how.

Conditional BCs can be specified using the ?:-notation (see a C/C++/Java-book for the meaning of that). For instance "pos().y<0 ? 1 : 0" would give you 1 in the lower half of the patch. If with "only a few faces use that condition" you mean "use a Dirichlet-condition the other a Neumann-Condition" then you'll have to modify the fractionExpression too

Hey Gschaider,
thx for your replay. I am programming with c++ but never used that kind of programming :) but now (after searching for that notation) i know what you mean.

so i can use sth. like that:


So i defined the value of variableValue between 0.2 to 0.8 to 1 and the other one to zero.
Is that correct?

And i use my own variable to set the valueExpressions:

Thx for your help.
tobi

I think you can do it simpler with

(I think the && makes it easier to read than the nested ?: )

Oh yes, this seems better. THX!

Time dependent inlet pressure
 

Hi Foamers,

I am trying to specify runTime dependent pressure inlet boundary conditions using a GroovyBC.

The expression for this inlet pressure is:
P_inlet = 2^(-runTime+5)+10;

I tried it as follows:

inlet
{
type groovyBC;
valueExpression "2^(-runTime()+5)+10";
value 1.0e6
}

and I get ant fatal error:

"field runTime not existing or of wrong type"

Is there a way to use the run time in the boundary condition without getting this error?

Can someone help me with this.


thank you in advance,
SBU

Two problems:
- time() gives you the current physical time
- ^ is the out product of vectors/tensors in OpenFOAM/swak4Foam. What you probably want is the function pow(a,b) (which gives a^b). The only problem is that the current *released* version only works with constant b. This has been fixed in the current development-version of swak4Foam (the one in the Mercurial-archive). If you don't want to install that the usual log/exp-trick will help you: "exp(log(2)*(-time()+5))+10"

Bernhard,


I have used "pow(x,y)" instead of "x^y" :

inlet
{
type groovyBC;
variables "p0=10.0e5;";
valueExpression "pow(2,-time()+5) + p0";
value uniform 40.0e5;
}

and get this error:

--> FOAM FATAL ERROR:
Parser Error at "1.8-11" :"syntax error, unexpected TOKEN_time, expecting value"
"pow(2,-time()+5) + p0"
" ^^^^ "

From function parsingValue
in file PatchValueExpressionDriver.C at line 192.

FOAM exiting

please help.

thanx,
SBU

That is EXACTLY what I said: "pow currently only works with constant b"

thanks Bernhard will try it and keep you updated.
:)

Hi there,
I am doing a thesis involving flow over a bump. I am finding information on groovyBC difficult to come by. Additionally, the information I do find is somewhat complicated. I am an engineer after all not a programmer haha. If somebody could explain to me how the following code works and what each individual symbol means that would be greatly appreciated. The following is a velocity profile of a wind tunnel inlet patch.

boundaryField
{
inlet
{
type groovyBC;
variables "Umax=1.0;d=0.01;turb_profile=Umax*pow(pos().y,0.1 428571429)*pow((1/d),0.1428571429);";
valueExpression "(pos().y < d) ? vector (turb_profile, 0, 0) : vector (1, 0, 0)";
value uniform (1 0 0 );
}

Hi Peter,

you do not Need programmers knowledge to use the groovy BC. Just read it like a equation ;)


In the following lines you can see the definitions of variables
There you set the following varialbes in math-format:





pos().y = Position of y (so it should be the length)


The Profil used in the BC is:
There you can see that there is an if - else condition:

if pos().y < d then use the vector: (turb_profile 0 0) else use the vector (1 0 0)


So you have a dependend vector in x-direction !

from y=0 till y = d the x-component is calculated with pos().y and the function defined above and after that you have the vector U=(1 0 0)

Hope it s clear enough!

Tobi

thanks heaps tobi that is very helpful indeed

Hey Guys,

I am looking and changing the groovyBC values and expressions for so long now, but don't get an inch further.

I got a closed System (outside wall) with an "inlet" it is also a wall, where i want to put pressure on. In the real world it is a cylinder gliding in the system and due to that pressure occures (liquid filled system).

I am so far

inlet
{
type groovyBC;
variables "pressure=22e05; T1=1e-04;Athmos=1e05:";
valueExpression "(time() < T1)? pressure : Athmos";
}

.. when i execute this there comes an error message that the Athmos couldn't be read and that the pressure was put to 500...

I want that when the time is lower than T1 the pressure occures to the system (inlet face) and after that -> goes back to normal Pressure ( 1 Bar (1e05 Pa)).


Do I have to use the fractionExpression due to my simulation? I read that it toggles the BC from Neumann to Dierlich(wrong spelling?).

Thanks for your Support!

It's always better to copy/paste the exact error message than retelling it.
The way you tell it you switch from one fixed value to another. Then your formulation should be find. Although I'd expect a "kick" to the system with the sudden jump you give

Thanks for you support gschaider!,
I worked it out and want to post my Example here.

inlet
{
type groovyBC;
variables "Druckstoss=22e05;Athmos=1e05;T1=5e-4;";
valueExpression "(time()< T1)? Druckstoss :Athmos ";
value uniform 1e05;
}

You only have to put a default value for the face. E.g. here 1e05 Pa (equal 1 Bar).
It works fine and triggers the boundary from 1 bar to 22 bar and back to 1 bar :)

Hi there,


I am trying to tweak this sine wave inlet BC into generating square wave but I don't seem to figure outhow to generate square wave. The BC below gives me continuous flow. But what I want is inlet that opens say every 0.5s and last for 0.1s.



Would really apperaeciate your feedback !


dropInlet
{
type groovyBC;
variables "xp=pts().x;minX=min(xp);maxX=max(xp);unif=-0.2*normal();";
valueExpression "10*(1+0.5*sin(500*time()))*unif";
value uniform (0.0 0.0 0.0);
}

A quick way to generate a square wave with "frequency" and "height" 1 would be something like

for discussions on the (a bit different) implementation of the modulo operator % in swak4foam see https://www.cfd-online.com/Forums/op...-groovybc.html and https://openfoamwiki.net/index.php/C...e_implemented:

Thank you gschaider,


It does exactly what I wanted to do. I set it at the inlet BC with alpha.water and I get continuous water flow into domain for 0.5 s, then it stops for the next 0.5 s and repeats. But I don't really know how does it work and would really appreciate your feedback. It looks like "%" here is a different than a modulo operator in OF then how does the use of % repeat the cycle every 0.5 s?


I have a new BC created in OF where I am trying to mimic exacty the same thing. I have a working BC code for continuous flow but when I tried to get it in cycle similar to groovy BC then it complains to compile: invalid operands of types double’ and ‘Int’ to binary ‘operator%’. I accessed time and used % operator inside the code as shown below. It doesn't look like % operator works the same way for groovy and OF.


scalar t_ = this->db().time().value();

t_ % 1 > 0






Many thanks!