[tsram90]

I am doing a analysis of a An IC engine with Hydrogen and diesel pilot injection.
When I try to do the mesh motion in fluent I am getting negative volume error. I am getting results when using a normal flat piston but my work is of a piston with a hemisphere in center.
Can someone do a mesh file and gambit file for me? (2D). I think the error is due to problems in meshing and I tried various types of meshing but its not working out.

I am using Gambit 2.2.30, Fluent 6.2.16

Engine Specs:
Stroke 110 mm
Bore 80 mm
Clearance volume: 2mm gap and a semi circle with 25 mm radius in center

Origin (0,0) At top of cylinder in center, No need of valves, need a diesel injector at center.

Thank you.

[-mAx-]

You are talking about moving stuff, so I suppose you are working with moving Mesh.
Can you post a sketch to see how you set up your geometry/mesh for moving mesh and what kind of moving option you are working with (remeshing-smoothing or layering).

[tsram90]

Originally Posted by -mAx-

You are talking about moving stuff, so I suppose you are working with moving Mesh.
Can you post a sketch to see how you set up your geometry/mesh for moving mesh and what kind of moving option you are working with (remeshing-smoothing or layering).

I did dynamic mesh in fluent with Remeshing and smooting. I didn't do layering because some tutorials told its best not to use layering in IC engine analysis.

I tried many options in meshing, I had tried different meshes(tri, quad) with varying interval sizes. I also tried splitting the volumes (stroke volume and clearance volume) as 2 and making the wall between them as 'interface.'

Still getting negative volume error at some point. It worked well with a normal flat piston. I am getting trouble when having the hemispherical piston.
I have attached the geometry as a .jpeg file in the first post.

[-mAx-]

Check if your mesh at t=0s (no motion), has negative volume.

[tsram90]

Originally Posted by -mAx-

Check if your mesh at t=0s (no motion), has negative volume.

How do I do that? I have done Grid-> Check and It returns no error

[-mAx-]

then you mesh is ok.
Problem should be on your moving mesh control parameters.
Try to display your mesh when error occures, to see where are negative cells

[tsram90]

Originally Posted by -mAx-

then you mesh is ok.
Problem should be on your moving mesh control parameters.
Try to display your mesh when error occures, to see where are negative cells

The negative cells are occurring at the lower most part during compression.( I think) . That is the part that is having a high density of cell. I have tried a normal piston( flat) and It worked well. But When i do this piston with same steps I am getting error. that's why I thought its the problem of meshing.

How can I separate the 2 parts into 2 meshes and then have a deforming mesh to the stroke volume.

What changes should i make from a normal procedure?

[-mAx-]

you can use split tool for separating your domain.
But I don't understand why layering is not recommended.
I think, that layering is more easy to use in IC (my opinion)

[tsram90]

Originally Posted by -mAx-

you can use split tool for separating your domain.
But I don't understand why layering is not recommended.
I think, that layering is more easy to use in IC (my opinion)

How do i put the options for layering?(Should I use laying and remeshing?)

Constant Height or Const ratio?
Split Factor and Collapse Factor.??
We Copy it frm Mesh info iin remeshing rite?? Anything similar for Layering?


Any files on how to use the split tool? Do i need an edge between the 2 meshes? (one mesh is deforming another one is just moving.

[-mAx-]

for layering you need quad mesh
http://my.fit.edu/itresources/manual...tg/node207.htm
http://my.fit.edu/itresources/manual.../th/node40.htm
http://my.fit.edu/itresources/manual...eom_face_split

[tsram90]

Originally Posted by -mAx-

for layering you need quad mesh
http://my.fit.edu/itresources/manual...tg/node207.htm
http://my.fit.edu/itresources/manual.../th/node40.htm
http://my.fit.edu/itresources/manual...eom_face_split

Thank You.. I will try some and get back soon..

[tsram90]

I tried some and is not getting results :-)

I couldn't mesh the geometry with quads... So I had to use Tri mesh..

3 Files are attached.. original mesh, Mesh when i got error by using layering, Mesh when using layering and remeshing.

When using both remeshing and layering, I got the negetive volume at a later stage. (about 1/2 of the compression cycle).

[ghost82]

Why can't you use quad mesh?
You can split the geometry into 2 faces, a rectangle and a semicircle, mesh the rectangle with quad map and the circle with quad pave for example, or you can split your geometri into 5 faces, and mesh all with quad map, as in the picture.
But I don't know which is better for layering and remeshing since I've never use it..

Daniele

[ghost82]

I attach also a couple of qualitative pictures taken from gambit: you can see also a boundary layer.

Daniele

[tsram90]

Originally Posted by ghost82

Why can't you use quad mesh?
You can split the geometry into 2 faces, a rectangle and a semicircle, mesh the rectangle with quad map and the circle with quad pave for example, or you can split your geometri into 5 faces, and mesh all with quad map, as in the picture.
But I don't know which is better for layering and remeshing since I've never use it..

Daniele

Thank you for that help.. I will try it.. But I need some more info on that.. How do we define the boundaries between each mesh? Do we put it as interface boundary condition?
Should we define 2 points with same (x,Y) and make 2 edges? So that we can have a edge interface in fluent.

[ghost82]

Originally Posted by tsram90

Thank you for that help.. I will try it.. But I need some more info on that.. How do we define the boundaries between each mesh? Do we put it as interface boundary condition?
Should we define 2 points with same (x,Y) and make 2 edges? So that we can have a edge interface in fluent.

Hi, please tell me more about your problem: since I didn't understand well and since I've never used dynamic mesh I need more info.
In dynamic mesh I think you have a mesh which is moving, so I think you have to define 2 zones in gambit: one for the moving mesh and one for the static one (if you have a static zone), so you will set in fluent parameters for the moving mesh zone.
Do you want to move mesh at the bottom of the rectangle (the 2 mm gap) and in the semicircle?
If so, all you have to do is to create an horizontal line at the bottom of your rectangle and define two zones in gambit (one which includes the faces of the semicircle and the face of the smaller rectangle at the bottom of the big ractangle and one for the big rectangle less the smaller one).
No need to create interfaces (I think..)..Fluent will treat internal edges as continuum.
If you wand you can upload somewere your dbs file with tri mesh and I will transform that "working" mesh in quad mesh ("working" means that that mesh has defined boudaries and zones).

However you should wait for max reply, he is absolutely more expert than me..
OT: Thank you max for your posts I learnt a lot from you.

Daniele

[tsram90]

My problem is simple. I have a Diesel IC engine. I want to study the combustion in it.
The geometry is as given above.
Engine Specs:
Stroke 110 mm
Bore 80 mm
Clearance volume: 2mm gap and a semi circle with 25 mm radius in center

Origin (0,0) At top of cylinder in center, No need of valves, need a diesel injector at center.

Problem is I cannot complete the mesh motion( I am getting negative volume after some time steps). Its due to the geometry, because I got it working in a normal flat piston. How should I change the meshing so as to get it working. I am getting the negative volumes inside that semi circle part, or at its edges.

[tsram90]

I got it working at last. I meshed it with tri mesh, as a single face, put the maximum skewness as 1. That got it running.
Max,Ghost Thank you very much.

Plz tell me what's the difference between layering and remeshing? I read the articles max posted but they say when a given condition is violated, a cell is added or subtracted. So what's the difference?

[-mAx-]

Remeshing means you have a mesh, and the solver will remesh your moving domain.
Layering means you will add (or suppress) cell layers in your moving domain >> on the the BC where you decided to add/suppress cells, first cell layer will be stretched (or compressed) untill a criterion will be satisfied. Then the solver will split (or collapse) the cell layer.

Remeshing is only available for tri (2d) or tetrad(3d)
Layering is only available for quad (2d) or hexa/wedge (3d)

[tsram90]

Originally Posted by ghost82

Why can't you use quad mesh?
You can split the geometry into 2 faces, a rectangle and a semicircle, mesh the rectangle with quad map and the circle with quad pave for example, or you can split your geometri into 5 faces, and mesh all with quad map, as in the picture.
But I don't know which is better for layering and remeshing since I've never use it..

Daniele

@ghost and max

If I convert the face into 2 faces or 5 faces as you told, how do I do the dynamic meshing part in fluent?
In a single face case, I put the top end stationary, Sides as deforming and bottom part(piston head) as rigid body.
Here should I define all the face boundaries as rigid bodies?
What type of boundary should be those? interface?