2D engine simulation
2 Attachment(s)
Hi foamers ,
I am simulating a 2D engine with sonicTurbDyMEngineFoam and simpleEngineTopoFVmesh library... my simulation is according to the 2D Tutorial case that attached by Prof.Jasak http://www.cfd-online.com/Forums/openfoam/83177-engine-simulation-mesh-motion-topological-changes-4.html Actually my result is not good.I attached the case and a picture of it at CAD=110. My problem is that velocity on the slave patch and master patch is zero(in paraview).(two boundaries that created for sliding interface.) these boundaries are valveCurtainCyl and valveCurtainPort. Boundary condition in my case for velocity on these boundaries is uniform (0 0 0) (similar to the 2D Tutorial ) But in the result of the tutorial case velocity on these boundaries is not zero(in paraview). How can I overcome this problem? Thanks and best regards, Sasan. |
Hi,
I had a similar problem with sliding interfaces (AMI). In my case, it was a rendering artifact due to paraview. When loading internalMesh alone and choosing "cell data" instead of "point data" the solution looks good. Best regards. |
1 Attachment(s)
Hi Laurent,
I did it . But I haven't got good result... I think my boundary condition have a problem... I appreciate any help... Thanks, Sasan. |
Hey Sasan,
I'd have to look a little deeper at the simpleEngineTopoFvMesh mesh class, but it seems like the sliding patches are set to be walls, when they should be just general patches. Try that and see if it helps, as right now it seems like each port is separated from the rest of the cylinder. |
Hey Dear Marco,
Thank you very much . I appreciate your help. yes,It seems sliding patches have seperated the cylinder to five regions...I don't know where is the problem.... Thanks, Sasan. |
Hi Sasan.
Could you post the whole case somewhere here? It will be helpful. The correct setup of the case is in the ICE sim. really difficult and without the case I am not able to tell you what is wrong. However, I think that your problem is hidden in the settings of motionU boundary conditions. For the the outer sliding interface you have to have the commponentMixed bc and for the inner it has to be zeroGradient. You should probably look at the Jasak's case. ¨ I will expect something like Quote:
|
1 Attachment(s)
Hi Martin ,
Thanks for your reply. I attached the case in the first post of this thread. I attached the case again here . Actually the motionU file of my case is similar to the jasak's case but my geometry is in the X-Y plane and jasak's case is in the X-Z plane , So I changed some things in my case. The motionU file for my case: Code:
/*--------------------------------*- C++ -*----------------------------------*\ Thanks and best regards, Sasan. |
Quote:
motionU seems fine, but you have made mistake in the naming of the sliding interafaces. valveCurtainCyl is outer (without "hole") and valveCurtainPort is inner (with "hole"). If you take a look in meshModifiers, you will see that just 5 of them have been created insteed of 9. So change the naming and the case should be fine. |
2 Attachment(s)
Hi Martin ,
Thank you very much.. I corrected the name of valveCurtainCyl and valveCurtainPort and I created all mesh modifier : Code:
/*--------------------------------*- C++ -*----------------------------------*\ Code:
--> FOAM FATAL ERROR: I attached a picture from grid around the intake valve at this time.The picture shows that the grid is degenerating ..... Also I attached the case.. Can you help me for overcoming this error? Do you know what is the origin of this error? I appreciate your help. Thanks and best regards, Sasan. |
Quote:
I am on vacation, so I can not test it by myself. Do you keep me informed about your progress? Martin |
Dear Martin ,
Thank you very much.. I appreciate your help.. I am very glad that you help me. I will try to do it and I will report my result and progressing to you. Thanks and best regards, Sasan. |
Hi Martin ,
I hope you have a happy vacation. I played with min layer thickness for the valves (several times) and I changed the deform angle to 0.. I corrected the clearance (=0.01) and the bore(=0.1) and I checked the valve diameters (they were correct). unfortunately I couldn't overcome the error... I found a thread [ http://www.cfd-online.com/Forums/ope...t-working.html ] that they have discussed about this error for engine simulation they have said this error occurs when all points on the sliding interface are not on the same radius and they attached a utility that can repair this problem. I compiled the utility but I don't know that how can I use this utility to solve my problem.. I appreciate any help from you. Thanks and best regards, Sasan. |
I created a small change in geometry and I increased the gap between valve and valve seat and I refined the mesh at this gap and I could run the case... ;)
Thanks, Sasan. |
Hi guys,
Sorry for hacking into this threads. However, when I tried to run the case shared in the very beginning, some error showed up: Unknown solver type laplaceFaceDecomposition Code:
Valid solver types are: |
All times are GMT -4. The time now is 19:11. |