[cfd seeker]

Hi everyone,

I have to do the dynamic mesh analysis of a hydraulic actuator. The attached figure shows the 2D model in which Inlet and moving walls are labeled. Wall labeled as "Moving Wall" moves vertically upwards some 20 units and increases the volume. Also the whole of inlet moves upwards by the same distance.

My question is: if the distance between "Wall 1" and "Wall 3" is to remain same then both of these walls should be defined as moving walls? And "Wall 2" will be defined as stationary or what? BTW whole of "Wall 4" is stationary.

Its a bit confusing but I think my explanation is clear.

Regards

[Lance]

Originally Posted by cfd seeker

Its a bit confusing[...]

There is no wall 4 in your figure. If walls 1-3 are not moving they should be stationary. Then the distance between 1 and 3 will be fixed. If only the "moving wall" part is moving, then prescribe the motion on that wall, and set unspecified on the two vertical walls next to it.

Or is wall 1-3 translating up and down as well? then prescribe that motion on those walls and set unspecified on the right vertical wall.

[cfd seeker]

Originally Posted by Lance

There is no wall 4 in your figure. If walls 1-3 are not moving they should be stationary. Then the distance between 1 and 3 will be fixed. If only the "moving wall" part is moving, then prescribe the motion on that wall, and set unspecified on the two vertical walls next to it.

Or is wall 1-3 translating up and down as well? then prescribe that motion on those walls and set unspecified on the right vertical wall.

Hi Lance,

thanks for the reply. Sorry I forgot to label in figure that whole of the right wall (two verticals and one horizontal ) is Wall 4. Yes actually Wall 1-3 are also translating up such that the distance between 1 and 3 remain the same. So in this case Wall 2 will be defined as Moving Wall or Unspecified? Do remember the vertical wall (part of Wall 4) is stationary.

[cfd seeker]

In the attached figure you can see the actual scenario that how the Walls 1,2 and 3 are moving along the vertical wall so that the distance between Walls 1 and 3 remain the same. Domain is actually extending upwards but since in the flow model I can't take the empty upper part along which other walls are sliding. So I am bit confused which walls will get which condition?

I hope I explained it well.

[Lance]

Specify vertical motion on walls 1-3 and vertical wall between moving wall and wall 1.

Upper vertical wall 4 should be unspecified, horizontal wall 4 stationary, lower vertical wall 4 stationary.


Depending on how far the walls are moving you might get issues with mesh folding, but that is another issue. Hex mesh is probably preferable.

[cfd seeker]

Originally Posted by Lance

Specify vertical motion on walls 1-3 and vertical wall between moving wall and wall 1.

Upper vertical wall 4 should be unspecified, horizontal wall 4 stationary, lower vertical wall 4 stationary.


Depending on how far the walls are moving you might get issues with mesh folding, but that is another issue. Hex mesh is probably preferable.

thanks for your help I think lower vertical part will also be specified as Unspecified because the walls opposite to it including Inlet also sliding vertically upwards. So it will´be specified as Unspecified. Right?

By mesh folding you mean mesh deformation?

[Lance]

Originally Posted by cfd seeker

I think lower vertical part will also be specified as Unspecified because the walls opposite to it including Inlet also sliding vertically upwards. So it will´be specified as Unspecified.

sounds reasonable.

Originally Posted by cfd seeker

By mesh folding you mean mesh deformation?

No. Mesh folding may occur with excessive mesh deformation, i.e. mesh cell quality will become poor (high skewness or cells will turn inside out)

[cfd seeker]

Originally Posted by Lance

No. Mesh folding may occur with excessive mesh deformation, i.e. mesh cell quality will become poor (high skewness or cells will turn inside out)

Yes in that case I have to use dynamic remeshing but first I will try to run the model with only small vertical displacement and once I have the working model I will specify full vertical displacement.

If I use hexa mesh then with vertical motion upwards cells will be streched too much like if the isplacement is 20-30 units. So in this case (streched hexa cells) dynamic remeshing will be needed or CFX can handle such cells?

Another question regarding motion specification. Actually Inlet is also moving upwards but at inlet i can't specify any motion as it's not a wall. Motion can only be specified to walls. What should I do for inlet face so that it also moves upwards with vertical walls?

[Lance]

Originally Posted by cfd seeker

Yes in that case I have to use dynamic remeshing but first I will try to run the model with only small vertical displacement and once I have the working model I will specify full vertical displacement.

When debugging specified mesh motion models turn off the other equations (flow, heat, etc) with expert parameters. Solving only mesh motion is much faster.

solve fluids = f

Originally Posted by cfd seeker

If I use hexa mesh then with vertical motion upwards cells will be streched too much like if the isplacement is 20-30 units. So in this case (streched hexa cells) dynamic remeshing will be needed or CFX can handle such cells?

Remeshing in CFX is not straightforward, but it can be done. But since your geometry is simple you should not have too much trouble with folded cells. Good quality mesh is key.

Originally Posted by cfd seeker

Inlet is also moving upwards but at inlet i can't specify any motion as it's not a wall. Motion can only be specified to walls. What should I do for inlet face so that it also moves upwards with vertical walls?

Not true. You can specify motion on inlets. You will get a warning:
"Mesh motion is specified on the boundary 'inlet'. This is valid for motion that is tangential to the boundary but solution errors will occur if motion is normal to the boundary."

[cfd seeker]

When debugging specified mesh motion models turn off the other equations (flow, heat, etc) with expert parameters. Solving only mesh motion is much faster.

solve fluids = f

Thanks for this wonderful advice!! Bravo But can you please tell me how and where I can specify this code to turn off flow equations?

Not true. You can specify motion on inlets. You will get a warning:
"Mesh motion is specified on the boundary 'inlet'. This is valid for motion that is tangential to the boundary but solution errors will occur if motion is normal to the boundary

Yes my bad. I checked it afterwards.

[Lance]

Originally Posted by cfd seeker

Thanks for this wonderful advice!! Bravo But can you please tell me how and where I can specify this code to turn off flow equations?

Right click solver, insert, expert parameters. Look under the 'Model overrides' tab.

[cfd seeker]

Thanks Lance.

I tried to run the simulation by turning off the flow equations.

For the displacement of mesh in y-direction I used the following two expressions separately in two different simulations

 
 
0.01[m/s]*atstep[s]

0.01[m/s]*t

But i think the mesh is not being displaced as the residuals for Mesh displacement remained at zero as can be seen in the attached figure. Also the mesh quality statistics remained the same as in the original mesh. What could be the reason for that? Is the expression for mesh displacement correct? What else can be the reason for this?

[Lance]

The expressions should work. Must be something wrong with your setup. Did you check the displacement in post? After 2500 iterations your first expression should have displaced the wall 25 [m].