[srsel6]

Hi everyone,

I'm trying to setup a dynamic mesh for a sinusoidally displaced piston. Seen in the attached pictures is my geometry. In Picture1.jpg and 2:

Green -- Defined piston face
1 -- "Reservoir" of fluid
2 -- Bridge connecting Reservoir and working chamber
3 -- working chamber
X -- point at which upon the piston reaches, Fluent crashes
4 -- Ignore this, just a bad mesh element I can't seem to get rid of.
Red arrows -- Fluid flow direction

I obtained picture 2 by drawing and meshing it directly, just to help illustrate my problem.


What I'm trying to do is to move the piston to the position as seen in Picture2.jpg where the fluid flow from the bridge to the working chamber is getting more and more cut off as the piston moves downward. However, when the piston reaches the "X" spot, Fluent gives this error and crashes:


Error at Node 0: coalesce_rib_faces: can't interpolate data, zones of different type detected.


I've tried looking around but no luck in finding the solution so far. I understand that making a complete cut off like that results in mesh topological change but I'm not sure how to configure it. Does anyone have any clue on how to solve this problem?


I've found this video on Youtube, which shows that it should be possible to have some sort of periodic mesh interface

https://www.youtube.com/watch?v=8cBA1fWP0QQ

[vinerm]

In the video as well as in your case, dynamic mesh is not required. All you need is a moving mesh. However, an extra element is required to do what is being done in the video. You have to setup Dynamic events to convert interfaces into walls and back into interfaces whenever required.

[srsel6]

In the video as well as in your case, dynamic mesh is not required. All you need is a moving mesh.

I'm using the layering method to simulate my piston moving up and down. I searched online and in Fluent but couldn't find any other "moving mesh" method except for setting the piston surface boundary condition to "moving wall", where I was able to set an expression for the velocity of the piston face. But when I performed a transient simulation, it didn't actually move the boundary ( which I expected ) because there was no "movement" applied. In short, I'm not exactly sure what you mean by moving mesh?

However, an extra element is required to do what is being done in the video. You have to setup Dynamic events to convert interfaces into walls and back into interfaces whenever required.

I tried your suggestion with two meshes:

1. All hexahedral elements with conformal mesh "interface" between the bridge and working piston chamber. In Design Modeller, the whole geometry is defined as a single solid. There really isn't any interface, it's just a mesh that's perfectly fitted with the geometry (Figure3.jpg)

2. Hexahedral elements for working piston chamber and tet/hex mix for reservoir & bridge with a non-conformal mesh interface between the bridge and working piston chamber. In Design Modeller, the whole geometry is defined as two solids, (i) The reservoir + bridge and (ii) The working piston chamber. (Figure4.jpg)
-----------------------------------------------------------------------------------
For the first mesh, I created a named selection for the "interface" between the piston chamber and bridge. I then set an event:

Event: Convert "interface" to wall

But I only managed to get as far as in picture3.jpg of this reply. Fluent crashed right after.

I've also tried (and a bunch of other options)

Event: Convert "interface" to sliding wall

Fluent immediately crashed the moment it reached the "X" spot in picture1.jpg

------------------------------------------------------------------------------------
When I tried mesh 2, (because you mentioned needing to convert an interface , which only mesh 2 gives)

It managed to work even without using any events. The mesh is shown in picture4.jpg. However, due to the mismatch of the nodes, I am skeptical of the results. The maximum linear velocity of the piston surface should be 0.47 m/s but the velocity contours show the velocity is almost constant everywhere. I'm going to try with a higher RPM to see if it works. But in the mean time, will the mismatch of nodes (even though an interface is already defined) cause bad results?. Do I need to apply a moving boundary condition (derivative of sinusoidal displacement function) on the piston surface as well?

[vinerm]

Within cell zone conditions for each cell, there are two options - Frame Motion and Mesh Motion. Mesh Motion makes the mesh move and is also called as moving mesh. So, in case the central region in domain only moves up and down but does not change its size, i.e., its length, then you can work with moving mesh. If it is like a space of a cylinder in a piston pump or engine, where volume changes during the stroke, then you have to use dynamic mesh and moving mesh cannot be used.

For interfaces, you have to ensure that not just the bodies are different but they also belong to different parts at DM and Meshing stage. The aim is to get non-comformal mesh so that there is no problem during the motion. In that case, only the wall belonging to the cylinder or piston, whatever it is, would need to be deformed. The other wall would not require any deformation.

[srsel6]

Originally Posted by vinerm

For interfaces, you have to ensure that not just the bodies are different but they also belong to different parts at DM and Meshing stage. The aim is to get non-comformal mesh so that there is no problem during the motion. In that case, only the wall belonging to the cylinder or piston, whatever it is, would need to be deformed. The other wall would not require any deformation.

I've just managed today to complete a full cycle at 1800 RPM. I've made some slight adjustments to the geometry. I have also used the patch function (underneath the initialize button) to set the temperature of the volume of the upper piston chamber (coloured red in all the pictures in this and my next reply post). The issue is that as the piston moves down, I'm expecting the temperature in the working chamber to diffuse into the reservoir, however, this does not happen.


----------------------------------------------------------

Seen in figure 5, is my geometry.

Green triangle --> Reservoir
Green diamond --> Piston faces
Green circle --> Reservoir - Working Chamber Contact region

Figures 5 and 6 show the geometry at the initial time step,

Figures 7 and 8 show the geometry and the final time step.

When the piston "opens" the reservoir by allowing the working chamber to come into contact with the reservoir, the higher pressure fluid (I've checked the pressure contours look the same as temperature contours, but are not presented here) from the working cylindrical chamber should force its way into the reservoir. There should not be such a sharp temperature gradient as shown in figures 9 and 10. I've checked the mass flux through the interface and it is a finite value, thus there should be temperature flux as well. I'm not really sure what is wrong, I've been looking around for a solution relating to mass flux but no luck so far.

I've even tried on a test case whereby I have a backward facing step. Whereby I initialized the left body to 1000K and the right body at 300K. However the temperature contour shows no temperature gradients at all, so I'm guessing the issue is with the initialization itself?

[srsel6]

Here are the remaining pictures. Figure 10 shows how I suppose the temperature flux should dissipating into the reservoir.

Figure 11 shows the backward facing step as I described in the previous post.

[vinerm]

What kind of interfaces have you defined? To debug the case, simplify it. Do not use any motion. Just bring the sliding chamber in contact with the rest of the domain and then initialize with high temperature in the sliding chamber. Observe if there is thermal diffusion across or not.

[srsel6]

I have double checked everything based on your recommendations, and I realized that I forgot to specify the interface between the chamber wall and reservoir wall. It is working perfectly now, thanks so much for the help! Took me 4 weeks of debugging to finally get here!

[vinerm]

It's good that it works finally.

[Master312]

Originally Posted by srsel6

I have double checked everything based on your recommendations, and I realized that I forgot to specify the interface between the chamber wall and reservoir wall. It is working perfectly now, thanks so much for the help! Took me 4 weeks of debugging to finally get here!

Hello,
I want to know how u repair the problem, cant interpolate data, zones of different type detected?
you defined the interfaces as deform meshes in "dynamic mesh"?

Thanks.