[abminternet]

ok I must be missing something, I keep getting the same error, do I need the dynamicFvMeshDict? it seems like perhaps I need to remove '# include "dynamicFvMesh.H" ' from my solver, but then that brings other errors, like, createDynamicFvMesh.H does not work any more :S

[abminternet]

wait, I modified the solver, I think I answered my own question

[abminternet]

hey Peter, so I modified the solver to be able to use engineTopoChangerMesh, and seems to compile alright, do you maybe have a test case I could run? there are many keywords I need to add and I'm not familiar with :S Would appreciate it

[Peter_600]

Try to replace # include "createDynamicFvMesh.H" with
# include "createEngineDynamicMesh.H"
in the sonicTurbDyMEngineFoam. C file and recompile.

[Peter_600]

I don t have a test case. But feel free to post any question you have. We may debug it together here.

[abminternet]

great I have one well I am testing verticalValves now but perhaps you know, it asks for valveHeadPatch, but also for poppetPatch, I thought they were the same, so I know what is the poppetPatch from my simpleEngine test case, but do u know what is the valveHeadPatch?

[Peter_600]

http://powerlab.fsb.hr/ped/kturbo/Op...Zagreb2007.pdf
Maybe this can be useful for you.

[Peter_600]

Try for valveHeadPatch -> none;

[abminternet]

thx for the tutorial so one quick question, what is the difference between valveTopTol and deformationLift? they are from the class verticalValves and engineVerticalValves respectively, but from the definition, it looks like they both do the same thing, disable top layering for the valves when lift < valveTopTol (or deformationLift).

[jajcevic]

Hi guys,
I have started the tutorial "simpleEngineStem" posted by abm, but after only several time steps following error occurs:

"Floating point exception"

I am using 1.6-ext and "sonicTurbDyMEngineFoam".


Do you have any idea why I can not successfully run this tutorial?

[abminternet]

hi Peter,

could you send me the engineGeometry file you used for your accordionEngineMesh class and for the verticalValves too? I would really appreciate it

[Peter_600]

Hi,

no problem. Here is my engineGeometry file for the accordionEngineMesh class. U will find a lot of things which are not used by the class, but the class requires an entry for it in the script. I didn t check which entry is really needed, thus I used it always like that. I will highlight the parts which are important for you.

I don t have a file for the verticalValves class.

Peter

conRodLength conRodLength [0 1 0 0 0 0 0] 0.161;

bore bore [0 1 0 0 0 0 0] 0.084;

stroke stroke [0 1 0 0 0 0 0] 0.09;

clearance clearance [0 1 0 0 0 0 0] 0.0014;

rpm rpm [0 0 -1 0 0 0 0] 2000;


cylinderHeadName cylinderHead;
linerName liner;
pistonAuxPoints pistonPoints;

moveDetach on;
correctPointsMotion yes;
delta 0.0001;
offSet 0.0005;

valveTopTol 1e-3;
bottomValveTol 5e-3;
poppetValveTol 5e-3;
checkMesh on;
cylinderSetName cylinder;


engineTopoChangerMesh accordionEngineMesh;

deformAngle 34;

piston
{
patch piston;
// patch none;

coordinateSystem
{
type cartesian;
origin (0 0 0);
axis (0 0 1);
direction (0 1 0);
}

minLayer 0.0005;
maxLayer 0.0015;
pistonCellSetName emptyfaces;
pistonFaceSetName emptyfaces;
pistonPointSetName emptyPoints;
bowlInPistonPatchName off;
bowlInCylinderPatchName off;

}

accordionEngineMesh
(
valve1
{
coordinateSystem
{
type cylindrical;
origin (-0.0203 -0.015518978 0.097944030);
axis (0 -0.258819 0.965926);
direction (1 0 0);
}
bottomPatch valve1_intake_bottom;
poppetPatch valve1_intake_top;
stemPatch valve1_intake_stem;
sidePatch off;
minLift 0.00025;
curtainInPortPatch off;
curtainInCylinderPatch off;
detachInCylinderPatch valveDetachInCyl1;
detachInPortPatch valveDetachInPort1;
valveHeadPatch off;
detachFaces detach1;
detachDistance 0.95e-8;
detachTol 0.005e-8;
stemEdge (0 0 0);
diameter -10;
deformationLift 0.005;
liftProfileFile valve1.lift;
staticPoints valve_fixed_points_1;
movingPoints valve_moving_points_1;
movingInternalPoints valve_moving_inernal_points_1;
staticCells valve_fixed_cells_1;
movingCells valve_moving_cells_1;
}

valve2......
.......
);

[abminternet]

Hi Peter, thanks a lot!! it is very helpful. I've got a couple of questions though:

When you set a variable to off, does that actually turn it off in the motion solver, so that it won't use it?
Also, what is the difference between the movingPoints and movingInternalPoints for the valve?

and the pistonCellset, pointSet and faceSet, what should they contain? the cells in the piston bowl but not the cylinder maybe?

thanks a lot for your help

[Peter_600]

Hi
First of all, do you have a mesh which has a similar designed like this?

http://www.engines.polimi.it/images/...eMotionGDI.gif

Which tools did you use to create the mesh? It is crucial to have a folder (named sets) in the polyMesh folder which conists all the different regions. For instance, I create the meshes in Gambit and name the boundaries directly there. Than I use

FluentMeshToFoam -writeSets

and the sets folder is automatically created with the required files. Do you follow a similiar approach?

Peter

[abminternet]

Hi Peter,

I am following a similar approach, but I am using Ansa for meshing. The thing is, I haven't really done it before and am not sure if I can write out the sets from ansa. So the moving points would be the points moving together with the valve, and the movingInternal points would be the ones were layering is being done on the picture? Is there some kind of documentation on this?

[vangelis]

Hi there,

I would like to help on the ANSA part of the issue.
I assume you are using ANSA v13.1.3
and that you are starting in CFD mode.
If you want to create SETs of nodes or elements
in ANSA for OpenFOAM you should do the following.

Activate the SET button at the top main toolbar
Press NEW
The selection mode window opens
you can mark if you want to select Nodes or Elements
or Properties
Select from the screen the entities you want to load
in the SET and confirm with middle mouse button.
The SETs card opens
Type in the name of the SET and press OK
The SET is created and displayed in the list

Now you can output in OpenFOAM format
In the output options window
activate the Output Sets flag.

ANSA will create the sets folder inside polymesh
as needed

Hope this helps

Vangelis

[abminternet]

wow great tipp, thanks a lot

[vangelis]

Let me know if you need anything about ANSA

[abminternet]

Thanks Vangelis, I do have a question, how do I create facesets in ansa? I need a set of internal faces, and I tried with the volToshell function to transform them to a shell and then selecting them in the sets option, but when I tried to write the mesh out, I didnt see the "write sets" option, and indeed the set was not written any ideas? Would appreciate it

[abminternet]

Hi Peter, I've also got a question for you, hope I'm not causing too much problem. Which faces would you set as the attach/detach faces? I mean, in the test case I did, the faces were at the very entrance of the port, but this faces were not moving. So, is it possible to select faces which are in the valve curtain for example? or faces in the layering zone, etc? Say in the picture you posted, which ones would be the attach/detach faces?