CFD Online Discussion Forums

CFD Online Discussion Forums (
-   ANSYS (
-   -   Solid Fluid interactions with non newtonian fluid (

daniebae October 21, 2010 14:34

Solid Fluid interactions with non newtonian fluid
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#.

- 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 ?

michael_owen October 21, 2010 16:00

What material are you using for the solid parts in ANSYS Mechanical?

daniebae October 22, 2010 10:17


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

michael_owen October 22, 2010 10:22

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.

daniebae October 22, 2010 10:48

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).


*** 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 ?

michael_owen October 22, 2010 11:12

How are you constraining the structural model?

daniebae October 22, 2010 11:18

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.

michael_owen October 22, 2010 11:22

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.

daniebae October 27, 2010 09:15

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 ;)

michael_owen October 27, 2010 11:30

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. ;)

daniebae October 28, 2010 12:34

where is that post about negative elements?

haha, yes i need to learn more of this mesh application !:D

adeban November 2, 2010 08:25

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

karupps8 May 27, 2013 03:57

FSI Error pls Solve Urgent:
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

All times are GMT -4. The time now is 10:59.