[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

[famon]

Originally Posted by 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 Profile1) [()] **piston-full**
Lift Profile2) [()] <Enter>
Start: [180] 0
End: [720] <Enter>
Increment: [10] 5
Plot lift? [yes] <Enter>
/define/models/dynamic-mesh-controls/in-cylinder-parameter>

hi
when I enter following command (define/models/dynamic-mesh-controls)
after pressing enter it says :
invalid command [define]
could you please guide?

[tsram90]

Originally Posted by famon

hi
when I enter following command (define/models/dynamic-mesh-controls)
after pressing enter it says :
invalid command [define]
could you please guide?

You have to enter it one by one..
define
models
...
...

[famon]

Thanks for your quick reply, worked ;-)

[sanjeetlimbu]

I am trying to simulate the compression stroke using 2D planner, mesh . I have to use axisymmetric option for my consider the real cylinder volume.
I made UDF and profile both case for the velocity of the piston. The inside will be gas mixture that I will load in chemkin import
I am unable to use the preview motion in both cases. I saw the piston with the profile - motion is as per the need, it move same distance I need. But it seems that the dynamic mesh is not good and causes the error

I am getting "Negative cell volume detected- dynamic mesh failed"
Pl share your feedback on how to solve the dynamic mesh motion

I am using Quad currently. Can u suggest the type of element to use for mesh and how to improve skewness /Orthogonal quality for the mesh to be used for the 2D axisymmetric case to represent the Cylinder

[tsram90]

Share your UDF and engine dimensions. Most probably the pistion is not returning, or you haven't given clearance volume.

Originally Posted by sanjeetlimbu

I am trying to simulate the compression stroke using 2D planner, mesh . I have to use axisymmetric option for my consider the real cylinder volume.
I made UDF and profile both case for the velocity of the piston. The inside will be gas mixture that I will load in chemkin import
I am unable to use the preview motion in both cases. I saw the piston with the profile - motion is as per the need, it move same distance I need. But it seems that the dynamic mesh is not good and causes the error

I am getting "Negative cell volume detected- dynamic mesh failed"
Pl share your feedback on how to solve the dynamic mesh motion

I am using Quad currently. Can u suggest the type of element to use for mesh and how to improve skewness /Orthogonal quality for the mesh to be used for the 2D axisymmetric case to represent the Cylinder

[sanjeetlimbu]

My dimension for the cylinder is :
Stroke length – 254mm (travel by piston edge), bore – 25.4mm (breath of mesh rectangle)
In cylinder motion: time step 0.000041s (default).
Compression stroke time = 30 ms , + 30ms to see combustion event
Veloity profile= start from zero to peak 14 m/s and abrupt deceleration to zero at 254 stroke travel

I have to use this for 2D axisymetric mode.
I ran for few time it run for 2D case, but show negative volume for axisymetric.

[tsram90]

Originally Posted by sanjeetlimbu

My dimension for the cylinder is :
Stroke length – 254mm (travel by piston edge), bore – 25.4mm (breath of mesh rectangle)
In cylinder motion: time step 0.000041s (default).
Compression stroke time = 30 ms , + 30ms to see combustion event
Veloity profile= start from zero to peak 14 m/s and abrupt deceleration to zero at 254 stroke travel

I have to use this for 2D axisymetric mode.
I ran for few time it run for 2D case, but show negative volume for axisymetric.

You have set clearance volume there? ie. after the cylinder has reached the TDC, there should be a small portion left.

And why is your total volume going to .007 from .013 in zero seconds?

[sanjeetlimbu]

Yes there will be clearance total length 254+14 mm

I am trying to make the piston side mesh in 2D there is crevice- step which is having some shape kink- small conduit area.

I am trying to simulate the piston stroke by - CFD modeling of two-stage ignition in a rapid compression machine:Assessment of zero-dimensional approach-Gaurav Mittal a,*, Mandhapati

at https://www.infona.pl/resource/bwmet...8-f989c9508de1

Answer: The volume is selected as moniter s , since it is compression stroke so reduction from 0.13 to 0.07, it may not be zero seconds

[sanjeetlimbu]

I tried using the edge sizing option
but still getting the negative volume error. even as the orthogonal is good 0.634 and the skewness there is one point element at 0.70