[cheredha]

Hello;
please , I need help about dynamic mesh.
I have a piston that moves using UDF (I use smoothing & remeshing ) .
the problem is that all cells remeshing , except that sits between the wall and the piston. !!!!!

[vasava]

Can you post inputs of the dynamic mesh settings?

[ciftci.ibrahim]

Well. Have you ever thought to use layering?

[cheredha]

yes ciftci.ibrahim
, it does not work

[D.M]

Hi,
1. first of all i should say that layering definitely works for these kind of problems , so if you don't get any result by layering it is because that you are doing something wrong in your setup for layering method , (after using layering method, u should define the piston as a dynamic mesh zone & as a rigid body motion and in the meshing option you MUST give the cell height an appropriate number based on your mesh and the adjacent zone should be fluid)

2. the second thing is that if you are using local cell remeshing method, in your case i think you should use local face remeshing too (i have not used local face remeshing till now for these kind of problems cause it is mostly used when you got deforming boundary but try to on local face remeshing in remeshing menu maybe it can help u!(i'm not sure))

you know your problem is caused because the local cell remeshing method can't increase the number of nodes on the boundaries (faces), i mean if u got 4 point on your boundary this method cant generate 5 nodes on your boundary during remeshing. look at the picture below...
and please let me know if you find solution for your problem , tnx.
problem.jpg

[cheredha]

Originally Posted by D.M

Hi,
1. first of all i should say that layering definitely works for these kind of problems , so if you don't get any result by layering it is because that you are doing something wrong in your setup for layering method , (after using layering method, u should define the piston as a dynamic mesh zone & as a rigid body motion and in the meshing option you MUST give the cell height an appropriate number based on your mesh and the adjacent zone should be fluid)

2. the second thing is that if you are using local cell remeshing method, in your case i think you should use local face remeshing too (i have not used local face remeshing till now for these kind of problems cause it is mostly used when you got deforming boundary but try to on local face remeshing in remeshing menu maybe it can help u!(i'm not sure))

you know your problem is caused because the local cell remeshing method can't increase the number of nodes on the boundaries (faces), i mean if u got 4 point on your boundary this method cant generate 5 nodes on your boundary during remeshing. look at the picture below...
and please let me know if you find solution for your problem , tnx.
Attachment 49800

I explained all in this video . thank you for all

https://www.youtube.com/watch?v=ezPi...ature=youtu.be

[cheredha]

Originally Posted by ciftci.ibrahim

Well. Have you ever thought to use layering?

https://www.youtube.com/watch?v=ezPi...ature=youtu.be

[cheredha]

Originally Posted by vasava

Can you post inputs of the dynamic mesh settings?

https://www.youtube.com/watch?v=ezPi...ature=youtu.be

[D.M]

Hello again , i saw your video ,

try to use layering method as i say:

1.your mesh should be quad, layering method can't be done with tri.(pic 1)
remember the first cell height of your mesh.(i mean the height of first cell row adjacent to piston)(look at the origin of cartesian coordinates in my mesh, try to place your coordinates exactly in the middle of your piston so there will be no need for additional setup in dynamic mesh menu)

2.in the dynamic mesh methods just click on layering.(pic 2)

3.compile your CG_MOTION udf.(pic 3)

4.set your piston as a rigid body motion, do not forget to set the cell height in the meshing option!!.(pic 4) (the magnitude of cell height should be the height of first cell row adjacent to piston)

5.try to use coupled method for better convergance, it won't take too much time for your problem.(pic 5)

6.for turbulence model use k_e RNG scalable wall function, i think it will be good for your problem but feel free to try something else.

1mesh.jpg

2just layering.jpg

3udf.jpg

4layering setup.jpg

5solution methods.jpg

[cheredha]

Originally Posted by D.M

Hello again , i saw your video ,

try to use layering method as i say:

1.your mesh should be quad, layering method can't be done with tri.(pic 1)
remember the first cell height of your mesh.(i mean the height of first cell row adjacent to piston)(look at the origin of cartesian coordinates in my mesh, try to place your coordinates exactly in the middle of your piston so there will be no need for additional setup in dynamic mesh menu)

2.in the dynamic mesh methods just click on layering.(pic 2)

3.compile your CG_MOTION udf.(pic 3)

4.set your piston as a rigid body motion, do not forget to set the cell height in the meshing option!!.(pic 4) (the magnitude of cell height should be the height of first cell row adjacent to piston)

5.try to use coupled method for better convergance, it won't take too much time for your problem.(pic 5)

6.for turbulence model use k_e RNG scalable wall function, i think it will be good for your problem but feel free to try something else.

Attachment 49807

Attachment 49808

Attachment 49809

Attachment 49810

Attachment 49811

finely. it is work.
thank you very very very much,
you are a good person, i'm really glad to know you.
thanks for all you do

[D.M]

I'm so glad that i could help you to solve your problem, glad to know you too , tnx.