Anyone interested in starting
 

Anyone interested in starting a project to develop a Foam application to simulate the injection molding process (polymers) with the following capability:

- Two-phase flow (based on interFoam)
- Non-isothermal
- Compressible (?)
- Viscoelastic flow


Post here.

Hi, Billy, I am interested.
 

Hi, Billy,

I am interested. What do you have in mind?

Pei

thanks billy for opening this
 

thanks billy for opening this topic.
just yesterday i expressed my interest in related topics and its good to see we have some interest in this.
in addition to the list of capabilities, i'd like to add the use of a 3D model.
hele-shaw approximation for 2.5d is reaching its limitation as part these days are bulkier.
if anyone is interested in taking this up, i have a paper that walks through implementing 3d flow simulation process.

Hi, Sathya, Could you pleas
 

Hi, Sathya,

Could you please email me the paper?

pei

Which paper is that?
 

Which paper is that?

Sathya, I'd be interested in s
 

Sathya, I'd be interested in seeing that paper. I have some experience in this issue as I used to develop commercial code in this arena.

here is the reference: "three-
 

here is the reference: "three-dimensional finite element method for the filling simulation of injection molding"
Geng Tie, Li Dequn, Zhou Huamin.
Engineering with computers (2006) 21: 289-295

In my opinion, this reference
 

In my opinion, this reference is closer to what we want since OpenFOAM uses the finite volume method.

"Numerical simulation of mold filling in injection molding using a three-dimensional finite volume approach"
CHANG Rong-Yeu & YANG Wen-Hsien
International journal for numerical methods in fluids
2001, vol. 37, no2, pp. 125-148

Once upon a time I used to hav
 

Once upon a time I used to have access to the original papers, but now I'd have to pay for these citations. Here's a couple of *free* papers from guys at Moldex3d who've referenced Chang and Yang
http://w3.moldex3d.com/en/services/techpapers/0401.pdf
http://w3.moldex3d.com/en/services/techpapers/0402.pdf
(The second paper looks more useful)
Its time to consider what you want the system to deliver i.e. is it an academic research analysis tool or a practical molding tool. I know even now that there are a large number of small molders for whom the cost of Moldflow type system is too great. However when you start reaching into the realms of visoelasticity and compressibility (and temperature and pressure specific heats and so on..) you will find that you'll spend most of your time in materials characterisation and modelling and not in doing the fun stuff. But from my experiences in Hele-Shaw (2.5D) I'd suggest the following development strategy.

1. Steady-state isothermal, newtonian flow solution. I'm not an expert in OpenFOAM but this looks like an out of the box solution.

Now there's two options
2a. Isothermal, newtonian transient flow with flow front advancement. Most systems use FVM with a fractional volume of fill model modelling the frontal location - some are using ficticious liquids to model air evacuation. This is unlikely to model "jetting" - is this a requirement?
2b. Develop non-newtonian model for viscosity - keep it isothermal as the temperature terms can be loosley coupled later. Do you need viscoelasticity or just 3d viscous terms? In a practical sense viscoelastics terms may be locally significant near "gates" and other sharp discontinuities but in a "real" large component are they needed? From my past, the most significant impact of viscoelasticity is in calculating the free surface die swell in extrusion. Transport models that incorporate "wall slip" aka "plug flow" are notoriuosly difficult to handle.

3. Add the temperature terms to develop a non-isothermal flow. Again if you use compressibility and other temp,pressure dependent properties these will complicate the solution. Then consider temperature evolution and local velocities at the flow front - "fountain flow effect" - also used in fibre orientaton models. Then there is the issue of cooling and the buildup of frozen layers - I used to handle this with a generic no-flow temperature and a psuedo high newtonian viscosity but there are probably more recent ways of modelling this effect. Freezing has the effect of reducing the flow channel resulting in increased pressure drop.

4. Look a the effect of mold wall temperatures, cooling channels etc (I never quite got this far <grin>). We did enable the mold temps to be profiled over different areas, but just used a high heat transfer cooefficient to model the mold wall boundary condition.

Enjoy

I added a new solver based on
 

I added a new solver based on interFoam for non-isothermal flow. So it has a temperature transport equation and CrossWLF viscosity model.

http://www.cfd-online.com/OpenFOAM_D...your_image.gif

I still don't know how to implement a boundary condition which acts as a wall for the polymer and acts as an outlet for air. Maybe there is a better approach to solve this. Maybe I can split the mesh and consider the interface an outlet. Any ideas?

hi Billy, i am interested ne
 

hi Billy,
i am interested nearly in the same problem than you: simulating the RTM process the thermomechanical problem.
i began since only 2 months, i need some bibliographical refrences that help me to understand problems involved and different models devoloped to solve that problem

Is there any updated informati
 

Is there any updated information on this proposed project? Has anyone implemented it? If not, I'm interested in being part of this. Please let me know. Any information is appreciated!

Hello, we are going to mode
 

Hello,

we are going to model hot melt extrusion of a polymer with OpenFOAM. However, I've not started yet but we definitely will start within this month. The flow will be non-isothermal with a high influence of dissipation on temperature and hence viscosity. So if anybody can give me a hint where to start in OF (Billy?) or want to help in the programming work is welcome.

Cheers
Stefan

Hi, Anyupdates on this proj
 

Hi,

Anyupdates on this project, I'm interseted in being a part of this effort.

Any Information will be appreciated.

Regards
Vaidya

Hi All, I'm trying to simu
 

Hi All,

I'm trying to simulate molding injection in OpenFOAM, I've started playing with interFoam, then I've implemented the BC which Billy suggested and now I'm testing it. Next step is using Billy's moldFoam solver to include temperature.

If someone is interested or would like to give me any advice or suggestion about it will be a pleasure for me.

Thanks in advance

Francesco

Hi, I have tried the mold
 

Hi,

I have tried the molding injection application that added CorssWLF and temperature T.But it did not work correctly. I find the problem is the staintRate()(fvc::mag(grad(U_))).
Then I modified the nonNewtonianFoam (singlephase)and used CrossWLF to calculate a case . Surprisingly it worked well! That is to say the problem is in twophaseMixture.
Now I do not know where the problem is .
I will make it sure !

Does others have problems in CrossWLF ?

Dear zhiwei liu,
I have the same problem with you.
In order to simulate the filling process of injection molding,I added CrossWLF viscosity model and temperature equation to the interFoam solver.But during calculating,the courant number increased enormously after a few steps.Then the calculation stopped.

I have also tried to use the WLF model:
nu=nu0*exp(-C1*(T-Tr)/(C2+T-Tr))
It worked well in polymer filling simulation.

So,I think the problem is the staintRate(),just as you have mentioned above.
Have you solved this problem? Please give me some suggestions.:)

Thanks in advance.

Jitao Liu

Hello Foamers

i am trying to develop a solver for injection molding using interFoam considering two Newtonian fluids (polymer / air). The flow inside the cavity is assumed to be incompressible, unsteady and isothermal.

The difficult part for me is that i don't know how to specify the boundary conditions at the outlet. I want only air to leave the cavity. is that correct if i drill a hole(s) (at the opposite side of the polymer inlet) for air outlet?

Can anyone help me to solve this problem?

Thanks in advance.
Nurye

Solver Development
 

Hi
Is there any updated information on this proposed project?
Has anyone implemented it?
I'm interested in being a part of this effort.I have done some works on viscoelastic fluids in OpenFOAM.
Please let me know. Any Information will be appreciated.
Best Regards

Interest in moldFoam
 

Hello all,
I am very interested in the discussion about a moldFoam group.I would like to know if there has been any new development in this area and also would like to offer any assistance that I can as far as testing of proposed moldFOAM solver.

I have been in the Injection molding industry for 12 years now and would relish the idea of producing or helping advance the OpenFOAM project. The only solution I know of at this point is MOLDFLOW by autodesk or MOLD-3D by Moldex, both of which are very expensive and out of the financial reach of most small companies.

Thanks for your time in advance,
Kyle L

Hi KyleL
As I said I am interested in. I had some literature review. Did you have too?
What is your plan?

Ata,
I guess my plan is to first find out what if any development has been done? Then I would like to review any information available, and maybe find a programmer that would be willing to help develop the needed moldFOAM solver.
I would very much like to see any information you have available.
Thanks,
KyleL

Any updates?
 

Are there any updates about this matter? I'm really interested in any applications wich involve the use of the OpenFOAM frame in simulating the injection molding process for polymers.

Thank you in advance

Polymer processing injection molding application
 

Hi
I have written a two phase code for polymer processing but now I am PhD student and I can not release it until the end of my PhD but if you want may be I could help you in code preparation or you can wait until the end of my PhD.
Best regards
Good luck

Hint: write a paper on it, with the details of the implementation, the numerical treatment and all the bits. It's a very good way to protect the authorship of your work.

Good luck!

Polymer processing injection molding application
 

Hi Alberto Passalacqua
I am doing that and after publishing my work, I'll release my code.
Best regards

Thank you for the reply
 

First of all thanks for the reply. Secondly, of course I do not ask for your source code if it hasn't been released yet (I'm a PhD student too, soo I can easily understand the importance of protect the autorship of your work). Actually at this stage I only want to understand if such a complex flow has already been approached inside the OpenFOAM frame and how, in general terms, it can be implemented. So, generally speaking, can you tell me how did you approach the problem (I mean: are the two phases isothermal or not? Did you start with modifying some pre-existing multiphase solver, such as the interFoam one? Is the polymer fluid treated as a non-newtonian one?)? Thank you and good luck for your PhD!

Hi
My code is isothermal solver for two phase flow. Two phases can be viscoelastic-viscoelastc fluids or viscoelastic-Newtonian fluids. There is about 15 constitutive models available for viscoelastic fluids in my code and geometry is general in it. I used from interFoam and viscoelasticFluidFoam solvers and combined them.
I think it is not very hard to add energy equation to may code.
Thank you very much for your understanding me and my restrictions
Good luck with your PhD too

That's great! I suggested that because a lot of work is going on with OpenFOAM, at least judging from this forum, but not as many papers are around ;-)

P.S. Didn't mean to put pressure :-)

Non-Isothermal solver
 

Hi
I have some students working on developing a code for simulation of injection moulding. They used interFoam and added an energy equation to the solver, part of the problem is discussed in following thread:

http://www.cfd-online.com/Forums/ope...sitymodel.html

The non-isothermal behavoiur is based on the paper:

"A novel design for hot-melt extrusion pelletizers"
Stefan Radel et. al.
Chmical Engineering Science 65 (2010) page 1976-1988

If the company involved in the project accepts, I will ask them to disclose the code and test case. However, there is still an issue about the frozen layer.

Hi Ata,

Is the melt compressible in your code? Do you take melt solidification into account in your solver? I am interested in injection molding simulation, too. Hope that we can hellp each other.

Best regards

Polymer processing injection molding application
 

Hi Jitao Liu
As now code is incompressible with no melt solidification. I would be very glad if I can help you and have cooperation with you.
Best regards

Ata

Hi, Ata
I want to combine the interFoam and viscoelasticFoam to simulate the polymer injection, just like i said in the other post. But in the interFoam solver, there is a "transportmodle" file in it ..., I have no idea to put the viscoelastic informations in it. How can I do? can you give me some advises on that?
If it is convenient, you are appreciated to e-mail me: skykzhang@hotmail.com:o

Hi
I ignored the transportmodle. Write one similar to it for your self.

ata, did you get your PhD already? you are appreciated for realseing the solver.

Hi all, i'm very interested in this project. There is still someone working on it?

up?

it is possible to access to all the work you did guys?

Hi guys,
any updates on the solvers? Would be interested to contribute, maybe adding a scalartransport equation to introduce temperature in the flow.
Let me know,
Christian

Injection molding in OpenFOAM? Euh....
 

Hi guys,

throughout this OpenFOAM forum, I see that many people are interested on the topic of "injection molding" with OpenFOAM.

It seems that some people have build a solver for this topic. Something based on interFoam for interface tracking, adding heat transfer, rheology and so on. Nevertheless, I'm not aware of anybody who has released such a solver;)

Well, I work on this topic for a long time and, from my point of view, it is a quite complex story to build such a tool. You could find some hints below.


Overview of the problem:

the cornerstone of the problem is not the heat transfer or rheology behavior (not an easy task nevertheless...) but the tracking of the interface by itself. Indeed, the main difficulty (for OpenFOAM) is that we need to deal with a highly viscous phase (the polymer) with something like air (not viscous at all). Mmm, it seems abstract at this point of the story:( We have something like interFoam no? Where is the problem?


Common simplifications:

in a first step, you can drop all transient and convective terms in the base Navier-Stokes solver --> you are dealing with pure Stokes problem now (it is what all standard softwares like Moldflow do by default). It should be easy now? --> not at all in fact :D You are just at the cornerstone of the problem: you need to deal with a Stokes system with a highly viscous term and a quasi inviscid one. Ok, another common simplification is to consider that air has a viscosity something like viscosity(polymer)/1000. For example, if your polymer has mu = 1000 Pa.s, then take mu(air) = 1Pa.s. It doesn't change significantly the flow front evolution and it reduces the stifness of the problem.


Still a nightmare:

Previous simplifications are good but far from being enough:mad:
The Stokes problem we need to deal with is still too stiff... for OpenFOAM.
The problem is heavily linked with the numerical kernel of OF: cell-centered FV with segregated approach for U/p. Not good at all for Stokes operator with strong jump on viscosity and high viscosity. The underlying reasons are not so clear from strict analytic point of view (search this topic on google scholar / you won't find many things). Ok, two things: 1- first recall at least that it is a quite well-known fact that cell-centered FV are bad for diffusion operators on irregular meshes --> there is "reminescence" of this behavior on eulerian tracking schemes (on perfectly regular meshes!), 2- secondly, try to use the interFoam to simulate the falling (by gravity) of a highly viscous drop (say a drop of radius 1mm with density 1000 and viscosity 1000Pa.s) in ambiant air and see the result. You should understand quickly what happens.


What you could do:

1- Work with a finite element solver for U/p :p (you can track alpha with FV if you -- still -- like them!).

2- Ok, i'm a bad guy. It could have some solutions also for finite volume framework but it is not "proven" and they are difficult to implement in OpenFOAM:

a- modern finite volume methods like DDFV. Search a paper of Jerome Droniou, "Finite volume schemes for diffusion equations. Introduction to and review of modern methods" --> just an introduction, not focused at all in diphasic Stokes problem / rather some approachs (DDFV but some others) for working with quite irregular meshes / some peoples have succesfully applied them for biphasic Stokes flows with good results. Highly interesting / quite valuable for amening OpenFOAM to a high level of numeric technology / but quite complex to implement properly and quickly. Obviously, if you are able to do such a thing by yourself, you would be a god if you release freely such an extension to the OpenFOAM community! Seriously, it is a quite complex topic and "a job by itself". You need to be a researcher on this topic to achieve it.

b- things should be quite better if you work with the coupled U/p solver of the extend version --> I haven't do it. If you do it, please give me a feedback... and I will give you the implementation the 3rd solution;)

c- keep the segregated approach, strenghen the viscosity flux (like for classical diffusion), clean up gradient pressure reconstruction used in OF, use a ghost fluid type method with a levelSet, and do a lot (:() of pimple iteration to enforce U/p coupling. It is the easiest approach. It is "not so long" to implement / it "works"... but not the result (accuracy versus CPU time) is not as good as a standard software based on Finite Element.

Nightmare is not finish... It begins!

If you start some works on this topic, you will quickly face the problem of the wall boundary condition treatment:D A physical fact: at the melt front position, the polymer "partially slip" along the wall... It is a big / interesting / and complex story to deal accurately and efficiently with this (now you should guess that it is not sufficient to use something like the "partialSlip" BC of OF).
Maybe more on this topic later:p


.................................................. ...........................

Well, is it yet an easy task to do injection molding with OpenFOAM??? Mmm, maybe it is for this reason that nobody has released a real solver for it... :)