CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > ANSYS

Solid Fluid interactions with non newtonian fluid

Register Blogs Members List Search Today's Posts Mark Forums Read

Reply
 
LinkBack Thread Tools Display Modes
Old   October 21, 2010, 14:34
Unhappy Solid Fluid interactions with non newtonian fluid
  #1
New Member
 
Daniel Baeriswyl
Join Date: Oct 2009
Posts: 9
Rep Power: 7
daniebae is on a distinguished road
Dear all,

I try to set up an Imprint Simulation. Means, a Pattern adept a Pressure on the top and will be pressed into a liquid polymer, which is placed on a plate.

I tried to set this all up with Workbench. I followed the Tutorial #Oscillating Plate with Two-Way Fluid-Structure Interaction#.

In ANSYS MECHANICAL
- A simple Hex mesh for the pattern and the plate
- a load applied on the top of the pattern
- solid fluid interaction between pattern and liquid polymer
- solid fluid interaction between liquid polymer and plate

in CFX:
- Material with Non-Newtonian model Carreau Yasuda = Liquid Polystyrene
- Symmetry Boundary conditions at each open wall
- Boundaries for MultiField Interactions on the top and bottom of the polymer ( as in the tutorial)

All properties set as the tutorial, so the ANSYS SOLVER gives out the ERROR:

-----------------------
*** WARNING *** CP = 51.406 TIME= 14:11:25
Material number 4 (used by element 34186 ) should normally have at
least one MP or one TB type command associated with it. Output of
energy by material may not be available.



*** WARNING *** CP = 2839.312 TIME= 14:35:18
The unconverged solution (identified as time 0.1 substep 999999) is
output for analysis debug purposes. Results should not be used for
any other purpose.



*** ERROR *** CP = 2839.281 TIME= 14:35:18
One or more elements have become highly distorted. Excessive
distortion of elements is usually a symptom indicating the need for
corrective action elsewhere. Try ramping the load up instead of step
applying the load (KBC,1). You may need to improve your mesh to
obtain elements with better aspect ratios. Also consider the behavior
of materials, contact pairs, and/or constraint equations. If this
message appears in the first iteration of first substep, be sure to
run shape checking of elements.



And the CFX SOLVER givs out:
| ERROR #001100279 has occurred in subroutine ErrAction. |
| Message: |
| CFX encountered the error: Read. Fatal error occurred when reque- |
| sting Total Mesh Displacement for bottom.


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


-- I tried to improve the mesh, I tested with other materials Newtonian fluids. I donít know if there are any other constrains needed.

The surprising thing is, that when I add a Displacement instead of a Pressure to the Pattern, the simulation runs! As I want to do a pressure study, this do not help me that much.


Does someone have a tipp or an idea what i could do ?
daniebae is offline   Reply With Quote

Old   October 21, 2010, 16:00
Default
  #2
Senior Member
 
Michael P. Owen
Join Date: Mar 2009
Posts: 195
Rep Power: 8
michael_owen is on a distinguished road
What material are you using for the solid parts in ANSYS Mechanical?
michael_owen is offline   Reply With Quote

Old   October 22, 2010, 10:17
Default
  #3
New Member
 
Daniel Baeriswyl
Join Date: Oct 2009
Posts: 9
Rep Power: 7
daniebae is on a distinguished road
hey,

i use for the pattern Si (Sillicum, Density 2329 kg m^-3, Youngs Modulus 1.85e11, Poisson Ratio 0.28)
for the Plate PET(density 1400 kg m^-3, Youngsmodulus 2.95e9, Poissons Ratio)


Does it require more properties ?

thank you
daniebae is offline   Reply With Quote

Old   October 22, 2010, 10:22
Default
  #4
Senior Member
 
Michael P. Owen
Join Date: Mar 2009
Posts: 195
Rep Power: 8
michael_owen is on a distinguished road
What pressure are you applying? Are you ramping it in or stepping it? What time stepping are you using on the structural side?

The structural solver is crashing because one or more elements are becoming highly distorted. This is happening in your PET material, which is soft.
michael_owen is offline   Reply With Quote

Old   October 22, 2010, 10:48
Default
  #5
New Member
 
Daniel Baeriswyl
Join Date: Oct 2009
Posts: 9
Rep Power: 7
daniebae is on a distinguished road
i applied a ramped pressure of 1e6 Pa. Starting from 0 s to 5 s, with time step of 0.1 sec. The time steps are equal in ansys and CFX.

I used once the Stainless Steel as Material for the Pattern and the Plate in ANSYS and i gave me an other error:




*** ERROR *** CP = 100.594 TIME= 11:38:21
Preconditioned conjugate gradient solver error level 1. Possibly, the
model is unconstrained or additional iterations may be needed. Try
running setting the multiplier MULT on the EQSLV command to greater
than 1.0 (but less than 3.0).

PRECONDITIONED SOLVER CP TIME = 21.875
PRECONDITIONED SOLVER ELAPSED TIME = 14.674

*** NOTE *** CP = 100.703 TIME= 11:38:21
During this loadstep the PCG iterative solver took more than 1000
iterations to solve the system of equations. In the future it may be
more efficient to choose a direct solver, such as the SPARSE solver,
for this analysis.

what you think ?
daniebae is offline   Reply With Quote

Old   October 22, 2010, 11:12
Default
  #6
Senior Member
 
Michael P. Owen
Join Date: Mar 2009
Posts: 195
Rep Power: 8
michael_owen is on a distinguished road
How are you constraining the structural model?
michael_owen is offline   Reply With Quote

Old   October 22, 2010, 11:18
Default
  #7
New Member
 
Daniel Baeriswyl
Join Date: Oct 2009
Posts: 9
Rep Power: 7
daniebae is on a distinguished road
Pressure appllied on the top of the pattern

Solid Fluid interaction between the polymer and the Plate

Fixed Support of the bottom of the PET.

[IMG]file:///C:/Documents%20and%20Settings/dbaerisw/Desktop/nanoimprint%20sym/geometry.JPG[/IMG]means the polymer is in a sandwich.
There are empty spaces, which are the cavities to be filled. Can i do this, instead of puting there a mesh with properties of Air.
daniebae is offline   Reply With Quote

Old   October 22, 2010, 11:22
Default
  #8
Senior Member
 
Michael P. Owen
Join Date: Mar 2009
Posts: 195
Rep Power: 8
michael_owen is on a distinguished road
I can't look at an image on your hard drive.

Are there any structural constraints on the plate, other than the pressure load? The pressure load is always normal to the surface; it does not constrain the model against tangential motions in any way. It sounds like your plate is sliding to the side in an unconstrained way. You need to put something like frictionless supports on the sides of the plate to keep it from sliding.
michael_owen is offline   Reply With Quote

Old   October 27, 2010, 09:15
Default
  #9
New Member
 
Daniel Baeriswyl
Join Date: Oct 2009
Posts: 9
Rep Power: 7
daniebae is on a distinguished road
Thank you i could fix that problem, but have a new one


So i put on the walls which are not into the moving direciton a frictionless support.

But now, it says that after a certain time step a "negative" element is created.

ERROR #002100012 has occurred in subroutine cVolSec. |
| Message: |
| A negative ELEMENT volume has been detected. This is a fatal |
| error and execution will be terminated. The location of the first |
| negative volume is reported below. |
| Volume : -0.1273E-11 |
| Location : ( -0.14598E-04, 0.78216E-07, -0.33727E+03)


I think that i have to downsize my mesh. But it is already thin enought to run my computer out of memory.

How can i import an ICEM MESH to Workbench. Cause meshing is much more easier in ICEM.

Again what do you think ?
thank you
daniebae is offline   Reply With Quote

Old   October 27, 2010, 11:30
Default
  #10
Senior Member
 
Michael P. Owen
Join Date: Mar 2009
Posts: 195
Rep Power: 8
michael_owen is on a distinguished road
As always, pictures would help.

What has happened is that you folded the fluid mesh. I made a post recently explaining what this means, why it can happen, and some things to do about it.

Try setting up a run that will stop just before the error, then post process the results and look at some cut planes with mesh lines turned on, and try to find where the mesh is folding and why. Then fix it.

If you think meshing in ICEM is easier then the meshing application, then you don't know how to use the meshing application.
michael_owen is offline   Reply With Quote

Old   October 28, 2010, 12:34
Default
  #11
New Member
 
Daniel Baeriswyl
Join Date: Oct 2009
Posts: 9
Rep Power: 7
daniebae is on a distinguished road
where is that post about negative elements?

haha, yes i need to learn more of this mesh application !
daniebae is offline   Reply With Quote

Old   November 2, 2010, 08:25
Default
  #12
New Member
 
Klas Johansson
Join Date: Mar 2009
Posts: 16
Rep Power: 8
adeban is on a distinguished road
How do you ramp up the load in ANSYS? Are you using a loadvariation table in workbench or is it rampend using KBC,1? The latter doesnt work in an MFX environment as each time step is a load step. With KBC,1 it will then apply the entire load directly.



Klas Johansson, Ph.D.
Technical Consultant at EDR
mailto:klas.johansson@edr.se

adeban is offline   Reply With Quote

Old   May 27, 2013, 03:57
Question FSI Error pls Solve Urgent:
  #13
New Member
 
karuppasamy
Join Date: Apr 2013
Posts: 2
Rep Power: 0
karupps8 is on a distinguished road
Dear Michael P. Owen,

I've got the following error at starting of the FSI run. Ansys 14.0-system coupling.

Preconditioned conjugate gradient solver error level 1. Possibly, the
model is unconstrained or additional iterations may be needed. Try
running setting the multiplier MULT on the EQSLV command to greater
than 1.0 (but less than 3.0).

My problem was fluid flow inside the cylindrical tube have a thickness of 30 cm and Inner dia =20 cm length=600cm.

outer wall was fixed .....fluid pressure was applied inside wall of cylinder.

Material is viscoelastic: density=1680 kg/m^-3, E=0.55MPa, Prony series model


Karuppasamy Pandian M
student
karupps8@gamail.com
karupps8 is offline   Reply With Quote

Reply

Tags
solid fluid interaction

Thread Tools
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
fluid or solid ??? Krish FLUENT 1 June 24, 2009 04:38
why is solid temperature same as fluid temperature on flow simulation ? qihongming FloEFD, FloWorks & FloTHERM 0 May 26, 2009 08:57
Defining Solid Zones Not working elmcmaster FLUENT 3 May 22, 2009 07:14
Conjugate Heat Transfer between fluid and solid Li Yang Main CFD Forum 8 March 27, 2004 12:05
Terrible Mistake In Fluid Dynamics History Abhi Main CFD Forum 12 July 8, 2002 09:11


All times are GMT -4. The time now is 03:14.