[vinerm]

This is because you might have created separate parts. All that's needed are separate bodies but these bodies should belong to same part. Then, you won't have any mesh interface.

[RJE]

that's true but i have all really seperate bodies only but i come out with the same problem in meshing

[vinerm]

In Ansys Meshing Tree, check if it shows single part or multiple parts. If it shows single part and you still get mesh interfaces in Fluent, then you have to check which boundaries are listed under mesh interfaces in Fluent.

[RJE]

1-i said the problem when i set it as bodies of the same part in on meshing and not in interfaces.
2- when plotting velocity or or displacement vs time in a specific surface eg : the piston , do u know how?

[vinerm]

Image makes the reason for interface clear. You need to keep both bodies, small duct and upper portion of the cylinder shown in the image, as separate bodies but in a single part, the way you have it right now. But you need to have a third body, which is lower portion of the cylinder, the one that will deform. Only that portion should have sweep mesh. The bodies shown in the image can have any type of mesh.

The reason for the interface is the existence of connections. For CFD, you should ensure that there are no Connections or Contacts at Meshing stage. Delete all the contacts under Connections and remesh. Do include the third body.

[RJE]

the third body should exist in the same part ?

[vinerm]

You have should only one part but either two or three bodies. The lower cylinder portion that will go under deformation should always be a separate body. The upper portion of the cylinder that has small duct attached could be either separate from the small duct or could be combined with the small duct. Part should always be one.

[RJE]

Yes i get that.
However while running the simulation , i get out the plot of velocity and displacement vs time of the piston (moving), but i'm not sure about the result i get , because while entering the fuid with a pressure which increase little by little with time (pressure photo) , i was looking for a result like that this last photo and i don't really find an explanation for the sinusoide part in the beginning of the plot of velocity

[vinerm]

The oscillations could be physical or numerical. Try animating the piston with every time-step and observe it the piston really goes in the manner depicted by graph.

[RJE]

ok i'll try that.
i have few other questions :
1-sometimes while running the simulation i get this warning "floating point exception", although my time step is very small e-3 or e-4 , i think the some is diverging ?
2-i want to have video of velocity for eg , what should i do to get this video and not just an animation solution

[srsel6]

RJE,

Are you still having the "negative cell volume" problem?

We are doing something similar and I've managed to solve the problem

For the piston chamber, use the sweep method when meshing. Then in Fluent, select Layering and smoothing. Set spring constant factor to 0.3 and convergence tolerance to 0.001. These settings seem to work for me.

[RJE]

yes sometimes i get negatives cell zones and sometimes i get this warning "floating point exception",
ok i 'll try that but i try sweeping last time in the piston zone, although that , they put some triangles although i oblige meshing to be all quad

[srsel6]

I forgot to add, since the sweep method gives you a layered mesh, I set my timestep in such a way that the piston only moves a maximum of 20% of the cell height (at the highest velocity)

[RJE]

how can i do that ?

[srsel6]

Originally Posted by vinerm

Though dynamic mesh does not care about it but the zone should be fluid and not solid because the zone represents the gas region. As far as piston is concerned, only its crown is important. Rest of the walls represent side wall of cylinder and cylinder head. Gravity is not essential. If the height of one layer of mesh is close to 0.002 m, then your setup is correct. However, your time-step could be too high. You should test your case with 1e-3 or 1e-4 s. The other option is to calculate the velocity manually and then determine what you should use. This can be done by integrating Newton's equation for motion with mass of piston as mass and the force of preloaded spring as force. But 1e-3 or 1e-4 should work.

vinerm has explained it here already.

time step (t) = 0.2*cell height (d) / max velocity (v)

[RJE]

i tried already this way but i get the same pb

[srsel6]

Originally Posted by RJE

i tried already this way but i get the same pb

Have you made sure the upper section and the lower section are separate bodies? Meaning you should have 2 bodies. 1 body where it is completely static and the other where a dynamic mesh is applied. An interface will then be necessary to connect the two together without facing negative cell volume issues.

In my case, that is what I did. In Solidworks I made them all separate bodies (4 bodies). I loaded them into design modeller and combined necessary parts using the "form new part" function. However I made sure to keep the dynamic mesh zone as its own single body so I can apply a swept mesh and use the layering technique.

[RJE]

yes i have made 2 bodies in the same part
i mesh the body close to the piston with mutizone option (quad) and the rest with tetra, but for the connexion? there is nothing

[srsel6]

Originally Posted by RJE

1-i said the problem when i set it as bodies of the same part in on meshing and not in interfaces.
2- when plotting velocity or or displacement vs time in a specific surface eg : the piston , do u know how?

The connections can be seen by clicking on the "plus" sign. Can you post a picture of your mesh?

[RJE]

yes, i sign up for connexions and there's nothing inside.
here's the picture of the mesh