[tsram90]

I am Trying to stimulate a IC engine combustion using fluent.

I am getting the following error during previewing mesh motion.

Mesh Statistics:
Min Volume =4.95612e-008
Max Volume =1.00199e-006 Done.
Updating mesh to time 1.04167e-03 (step = 00025) (crank-angle = 192.50)

WARNING: non-positive volumes exist.

Mesh Statistics:
Min Volume =-3.13968e-008
Max Volume =1.00199e-006
Warning: negative cell volume detected!
Error: Update dynamic mesh failed!
Error Object: ()

If I start from BDC I get error at 192deg, If I start from TDC I get error at 333deg.

I first tried using a piston with a hemisphere in center, Also tried a square clearance volume. Cannot get the results in any case.

Is there something I missed?
My procedure was:
Read
Models->unsteady
Energy Eqn
K epsilon (2 eqn)
Dynamic-> parameters
Smoothing and remeshing
Set min and max values in remeshing from the info panel
In Cylinder- Set incylinder values
Dynamic-> zones
Set piston as rigid body, Side walls as Deforming(Cylinder)

Type the following:(No idea why:). Found in some forum this is needed, First tried without this also)

> define/models/dynamic-mesh-controls
/define/models/dynamic-mesh-controls> icp
/define/models/dynamic-mesh-controls/in-cylinder-parameter> ppl
#f
Lift Profile:(1) [()] **piston-full**
Lift Profile:(2) [()] <Enter>
Start: [180] 0
End: [720] <Enter>
Increment: [10] 5
Plot lift? [yes] <Enter>
/define/models/dynamic-mesh-controls/in-cylinder-parameter>


Is there something I missed? I am getting this error in all the things I done. But a friend did one in his PC And I checked it in mine it worked.

[emreg]

hi,

i hav faced same problem last days.
i found that this is a mesh problem not an fluent settings error.

Follow this, if you will be succeed, inform me plz:

- Keep in mind that this error occurs usually while subtracting volumes.
Do u have some substracted volumes whic u performed in gambit?
Be careful while subtracting them especially for the volumes which they hav interfaces. (do u hav any interface BCs? )

- Check ur mesh and observe if there exists an error about Contact points.. exist?

inform me ...
regards,
emre gungor

[tsram90]

First of all. I don't have any subtracted volumes. ( I don't have volumes. Its 2D) Still I haven't done any face subtractions.

I don't have any interface BC either. Just 2 Vel in, 1 Pre out and rest are walls.

My geometry is quite simple. Just a square(defined using lines) with 3 valves in top.(also just lines)

I havn't got any error so far on contact points. I am not sure what they are and where to look for them. My grid-> check didn't give any errors

[raj.cfd]

Hi,

Negative volumes appear, if the centroid of a cell ( 2D or 3D ) is beyond the geometrical boundaries. Try getting a good mesh before proceeding further..

[tsram90]

Originally Posted by raj.cfd

Hi,

Negative volumes appear, if the centroid of a cell ( 2D or 3D ) is beyond the geometrical boundaries. Try getting a good mesh before proceeding further..

Centroid of the 'cell is beyond cell boundary right. Not the total centroid?


How to get a good mesh? I am doing 2D so I tried meshs with equal interval size on all edges and both tri and quad meshs. The geometry is simple.Its a square.

[raj.cfd]

Hi,

From your original post, I can make out you are simulating a 2D IC engine - using dynamic mesh, right...??? . I have already worked on dynamic mesh for a IC-Cylinder. Here in your case , I suppose the negative volumes appear when the mesh is deforming/layer compression, ie when the piston moves from BDC to TDC. In order to solve this say for example, you have a piston, cylinder, bowl region, ports . you can create a pure quad mesh from the piston until the construction plane/reference plane and then upwards you can mesh it with tria. The construction plane is something like a reference plane until where the reciprocating motion of the piston takes place using dynamic mesh in FLUENT. You can either use smoothing, layering and/or remeshing option .You can probably look into IC engine simulation tutorial provided by Ansys Fluent. This should solve your problem.

[tsram90]

Originally Posted by raj.cfd

Hi,

I suppose the negative volumes appear when the mesh is deforming/layer compression, ie when the piston moves from BDC to TDC. In order to solve this say for example, you have a piston, cylinder, bowl region, ports . you can create a pure quad mesh from the piston until the construction plane/reference plane and then upwards you can mesh it with tria. The construction plane is something like a reference plane until where the reciprocating motion of the piston takes place using dynamic mesh in FLUENT. You can either use smoothing, layering and/or remeshing option .

I tried starting from BDC and from TDC. I am getting negetive volume either way.( if from TDC then during down stroke.). I also tried reducing teh problem. Removed all vcalves, ports etc. Just a square. Still I am getting it.

I tried with Tri mesh only and quad mesh only. Getting error. I want to try using both of them mixed as said above. But I can't get any tuts on how to do it. Plz explain or give a link.

TQ..

[karthickeyan]

hi friend
after seeing your post i found that you are using IN-cylinder motion. in that you are using remeshing ?because it only cause negative volume in dynamic mesh. you should give minimum cell size and maximum cell size value in remeshing option . it should be (0.4 *average cell size)and (1.2*average cell size)for maximum cell size. sorry for the delay in replying.

[tsram90]

Originally Posted by karthickeyan

hi friend
after seeing your post i found that you are using IN-cylinder motion. in that you are using remeshing ?because it only cause negative volume in dynamic mesh. you should give minimum cell size and maximum cell size value in remeshing option . it should be (0.4 *average cell size)and (1.2*average cell size)for maximum cell size. sorry for the delay in replying.

TQ for the reply. I was seriously held back in with my project progress by this problem.

I am not using layering. using both Smoothing and remeshing.
I gave the values from the 'mesh scale info' just under where we give these value.

By ur method, how do we get the average cell size?

[tsram90]

Got It.

Adjusted the remeshing cell size in the Zone defining section with .4 and 1.4 of the avg cell length. (got length as min+max /2)


Now someone tell me what this is

> define/models/dynamic-mesh-controls
/define/models/dynamic-mesh-controls> icp
/define/models/dynamic-mesh-controls/in-cylinder-parameter> ppl
#f
Lift Profile:(1) [()] **piston-full**
Lift Profile:(2) [()] <Enter>
Start: [180] 0
End: [720] <Enter>
Increment: [10] 5
Plot lift? [yes] <Enter>
/define/models/dynamic-mesh-controls/in-cylinder-parameter>

[karthickeyan]

]


while specifying side wall as deforming there is an option 'mesh scale info' from that there is minimum cell size and maximum cell size from this take an average value and multiply with .4 for minimum cell size and specify for remeshing similarly 1.2 * avg cell value for maxicell value