# solidification viscosity governed through an additional variable

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

 September 13, 2012, 04:02 solidification viscosity governed through an additional variable #1 New Member   Join Date: Sep 2012 Location: Europe Posts: 25 Rep Power: 7 Hi dears, I have a problem: I want simulate a resin material that enters in a cylindrical die, solidifies and exit from the other side of the die. Solidification is governed by the resin viscosity, that increases with an additional variable, alfa, modeled as a volumetric transport equation (without diffusion) through the resin domain, with a additional variable source therm activated by the temperature of the die. The problem is that the resin thermal equation and the transport equation related to the additional variable, don't meet the convergence: their residuals are stable about 10^-1 also for many and many iterations (4000). It seems that as the viscosity increases from the initial values (1.5 Pa*s), the system is less able to rase the residual as the resin viscosity grows. If I set a costant viscosity of 1,5 Pa*s the simulation works and the residuals are raised below 10^-4. If I set a costant high viscosity the simulation don'works because the residuals are stable about 10^0- 10^-1. It is a problem that come when the viscosity becomes high. How I can do to run the viscosity governed solidification process of this resin? Can you help me?

 September 13, 2012, 07:03 #2 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 14,335 Rep Power: 110 What Re number does this run at when the resin is at maximum viscosity? CFX (and indeed all Navier-Stokes solvers I am aware of) do not run well at very low Re number (Re<0.01 or so) and will have troubles converging. This sort of simulation is best done on a stokes flow solver.

September 13, 2012, 07:13
#3
New Member

Join Date: Sep 2012
Location: Europe
Posts: 25
Rep Power: 7
Quote:
 Originally Posted by ghorrocks What Re number does this run at when the resin is at maximum viscosity? CFX (and indeed all Navier-Stokes solvers I am aware of) do not run well at very low Re number (Re<0.01 or so) and will have troubles converging. This sort of simulation is best done on a stokes flow solver.
Reynolds in this simulation is effectively very low: infact the velocity of the resin in the die is very low (0.002 m/s), the radius of the cylindircal part is 0.0025 m and the viscosity accordingly with the law of variation that I have, sould increase from 1.5 Pa*s to also 10^7 Pa*s (practically a solid). So Reynolds finally is about zero. What I can do in CFX, is there an option to switch to Stokes flow solver?

 September 13, 2012, 07:23 #4 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 14,335 Rep Power: 110 So your Re=1e-9, I think that qualifies as low Re... CFX cannot handle flows as slow as this. It does not have a stokes flow solver, you need to switch to one which does - or write your own, with no inertial terms Stokes flow solvers are a bit simpler than NS solvers.

 September 13, 2012, 08:19 #5 New Member   Talita Possamai Join Date: Sep 2012 Posts: 23 Rep Power: 7 Hello l.te, I agree with ghorrocks, you won't be able to solve that fluid flow with CFX as it is. CFX has it's limitations, and that's why people has to develop codes to solve some complex problems. But, if I may, I have a suggestion for you: Simplify your problem. Think on the aim of your work. Do you really need to have the fluid flow, or are you more interested in the solidification process as the resin pass through the die? If so, then treat the resin as a solid. Adapt the solid material to behave like you need (play with material properties). If your die format is simple you can prescribe a estimated solid velocity profile. Keep in mind that this is a suggestion to estimate your results with the CFX. But if you really need to solve the fluid flow field, then you should follow ghorrocks suggestion. Regards, Possa.

 September 13, 2012, 09:01 #6 New Member   Join Date: Sep 2012 Location: Europe Posts: 25 Rep Power: 7 Hello dears, thanks for our suggestions! In my work the resin (together with unidirectional glass fibers) is part of a cylindrical composite material that, passing with a continous low velocity through the heated die, solidifies and is pulled downstream from the die by means of a puller (this process is called pultrusion). The aim of my work is exactly study the viscous forces between the die and the resin , (and them increase as the viscosity increase!), until a point (inside the die) at which the part detaches from the die. Pratically I want know what is the force to be provided at a puller to pull the composite out from the die, and to calculate it, I think that is fondamental to have a model with an initial resin defined as fluid, with its viscosity that grow with during the heating process in the die... How I can do? I have learned CFX exactly to do this study..

 September 13, 2012, 09:11 #7 New Member   Talita Possamai Join Date: Sep 2012 Posts: 23 Rep Power: 7 Hello l.te, Unfortunately, I believe you won't be able to solve it like you want in CFX. As I see it you have two options: 1 - learn another software, as suggested by ghorrocks, or develop a code of your own that is able to solve that; 2 - Think of a way to simplify your problem and model what you need in another way (remembering that the problem is the low Re number). I suggest you talk with someone with experience in low Re number CFD. It also helps to do a bibliografic revision on articles and works in that area. Regards, Possa.

 September 13, 2012, 09:29 #8 New Member   Join Date: Sep 2012 Location: Europe Posts: 25 Rep Power: 7 Ok, many many thanks for the aid at all of you!

 September 13, 2012, 19:19 #9 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 14,335 Rep Power: 110 I am no expert in this area but I do not think that an increasing Newtonian viscosity is a good model for the polymerisation process going on in resin cure. Do you have any evidense to show it is a good model? I would do a literature study, as recommended by Talita, and work out what is an appropriate model for this process. You may well be better off with an lagrangian FEA approach, such as ABAQUS, ANSYS Mechanical; with non-linear material properties.

 Thread Tools Display Modes Linear Mode

 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 OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post TDK FLUENT 11 July 31, 2016 06:03 Clark Griswold CFX 2 April 21, 2012 07:20 charlotte CFX 4 March 22, 2011 10:14 lego CFX 3 November 5, 2002 21:09 George Bergantz Main CFD Forum 15 September 19, 2000 14:28

All times are GMT -4. The time now is 03:21.