XANSYS Message: 93034 [Go back to message list]
[bookmark on del.icio.us]
No rating yet
Subject: Re: Ansys FSI nightmare
Author: Peter Joseph Attar
Date: 2008-04-26 01:22:43You should reply to the list directly so that other people may benefit from
the discussion. With regards to the automatic timestepping, I would guess
that it
would start cutting the substep size when the elment gets distorted, however I
am not sure. Really the automatic timestepping is based upon how well the
Newton-Raphson convergence history is going. If a previous substep takes a
lot of Newton-Raphson steps, then the next step will have a
smaller "timestep" However in the case of buckling the change might be so
dramatic that this won't work. If I were you at this point I would try to use
small substeps from the start and not rely on the automatic substepping to
get you through the problem area.
Peter
On Friday 25 April 2008 20:14, Y Y Tan wrote:
> Hi Peter,
>
> Thanks for spending so much time to write to me.
>
> Yea I get it now. Element formulation is either pure displacement of mixed
> u-p whereas element technology is full/reduced integration. Anyway since
> you mention that my problem doesn't concern any of this I would probably
> not dwell further into this.
>
> I would probably try to make a refinement to my elements where the collapse
> happens. Anyway as for the time-stepping, I'm using the auto-timestepping
> feature and I've set the maximum substep to a very high value and from how
> I understand, if the solution does not converge the auto time step would
> make the time steps smaller until I reach my maximum limit, however in my
> solution, the maximum has not even been reached and the mesh has turned
> inside out. Does this mean that this has nothing to do with my timestep
> size or could it be that mesh distortion isin't counted as a diverge
> solution and hence the auto-timestepping feature does not kick in?
>
> I hardly want to see myself in this postion rite now. There are a few
> people who have actually done this before on other programs like ls-dyna
> and adina but I've not come across any published literiture where one has
> used Ansys to model my problem. So do I conclude that it is very difficult
> to get Ansys to perform such a highly non-linear coupled problem?
>
> I am actually someone who enjoys the feeling of achievement. Its just that
> at this very point in my life, things are not going too well and after
> putting in so much effort, there have been no results for me. Its very very
> discouraging. Anyway thanks for the advice, hopefully i'll be more capable
> in handling things in the near future.
>
> Regards,
> Tan Yi Yong
>
> Quoting Peter Joseph Attar :
> > Hmm..I thought you were doing a transient simulation..sorry my fault.
> > Doing a time accurate solution might actually alleviate some of your
> > issues ..
> > but I digress.
> >
> > Anyway, elements turning inside out has nothing to do with hourglassing.
> > Basically what is happening is that your element is getting so distorted
> > that
> >
> > your element Jacobian becomes negative.
> >
> > With regards to the element formulation, full and reduced integration are
> > completely separate ideas from displacement and mixed formulations.
> > With a mixed formulation you not only have displacement as element dof
> > but you
> > also have pressure. It is called mixed for this reason. The variational
> > statement includes both displacement and pressure as dependent variables
> > unlike the principle of virtual work which just has displacements as the
> > variables being varied. This is one way of getting around the volumetric
> > locking that might occur for materials which are incompressible (or
> > nearly incompressible). The other way, less elegant and perhaps less
> > accurate is to
> >
> > use reduced integration. This is all explained in the manual, or at least
> > I think it is.
> >
> > However your problem is more than likely not with any sort of locking
> > behavior, but with the fact that within a timestep your elements areAlso
> > with regards to my previous suggestion, if the buckled shape would not
> > allow
> >
> > flow you could get the buckled shape and perhaps perturb it a bit to get
> > a geometry which would allow flow through. The whole point is to get
> > around the
> >
> > point where you go from unbuckled to buckled. If you are only interested
> > in the final steady solution (if there is even such a thing for this
> > problem), then
> > deforming too much causing them to "turn inside out". The simplest way
> > to get
> > around this would be to 1) put many more elements in the region of
> > interest and 2) increase the number of substeps/loadsteps. Also as I
> > stated, shell181s might be better here since they might handle the
> > extreme deformations a bit better.
> >
> > At this point, as you probably have figured out already, all of the
> > advice given on how to actually model the thing is not going to help you
> > in a week.
> >
> > As Martin stated, the best thing for you to do now would be to clearly
> > explain what you have tried up to this point, the problems you have run
> > into,
> >
> > and some ideas for future work. This would be of great benefit to
> > whomever takes over this project after you and would be worthy
> > contribution for an undergraduate project.
> >
> > Finally, and probably most importantly, I stand by my statement about the
> > problem being a fun one. I don't know if you plan on continuing your
> > career in research or engineering for that matter. However if you do, you
> > had better
> >
> > learn to live with running into things which don't work out correctly at
> > first. Nobody said independent research is going to be easy. The fun part
> > about research is running into obstacles, and then realizing that you are
> > smart and clever enough to think your way through the obstacles and
> > finally getting it to work. Once this happens to you once, you'll see
> > what I mean. Unfortunately, this is your first time delving into this and
> > you have yet to
> >
> > experience the feeling I am referring to. One of the main jobs of your
> > advisor should have been to continually reinforce this idea with you. It
> > looks like he or she failed in this regard.
> >
> > Anyway good luck.It looks like you have learned some things which is the
> > main
> >
> > idea, especially for an undergraduate research topic.
> >
> > Peter
> >
> > On Friday 25 April 2008 19:03, you wrote:
> > > Hi again,
> > >
> > > For the past couple of hours, i've ran another 5 simulations. One thing
> > > I realize is that lowering the under-relaxation factor for the
> > > displacement from Ansys cures the negative volume better than lowering
> > > the pseudo timestep or incresing the mesh stiffness and increasing the
> > > mesh quality. However the bad news is i'm still stuck. :(
> > >
> > > Peter, the thing i want to validate the capability of Ansys in
> > > simulating the FSI of a collapsible tube flow. I'm using the exact
> > > boundary
> >
> > conditions
> >
> > > from another paper to do this in Ansys and i'm only interested in the
> >
> > final
> >
> > > result since this is a steady solution anyway. I've tried solving the
> > > structural part first but the thing is if I solve the structural part
> > > first, the external pressure would cause the pipe to buckle so much
> > > that
> >
> > it
> >
> > > will prevent any fluid from flowing through and the analysis would just
> > > crash.
> > >
> > > I really think that the problem now is with my Solsh190, I've been
> > > reading alot about hourglassing and volumetric locking. I'm very
> > > confused about this. In Ansys, I could only set the keyopt to change
> > > between using a pure displacement formulation or a mixed u-p
> > > formulation. However as i'm
> >
> > working
> >
> > > on Workbench, the only option I can change is the brick integration
> >
> > scheme
> >
> > > which is either full or reduced. Does full means mixed u-p and reduced
> > > means pure displacement? or its a completely different thing. So please
> >
> > can
> >
> > > someone tell me when error message is element turning inside out, does
> > > it mean its hourglassing or there's volumetric locking because I don't
> > > know how to explain the shape of the element. Anyway how do I specify a
> > > mixed u-p formulation for solsh190 in workbench?
> > >
> > > Anyway does anyone know how to use shell 181 in workbench? I could only
> >
> > get
> >
> > > the mesher to mesh shell 181 when I import a surface body and when I do
> > > that, there seems to be only 1 face and I cant specify if my loadings
> > > are on which side of the face.
> > >
> > > Peter, its not a fun problem. :( ... I have not been able to sleep
> >
> > properly
> >
> > > for the past few months.
> > >
> > > Fern, I really wish my supervisor understands what i'm facing but the
> >
> > thing
> >
> > > is, people would only think of this problem as a fluid flowing through
> > > an elastic pipe..how difficult can this be compared to people who are
> > > modelling flow past an airplane or stuff like that. I have tried to
> > > talk
> >
> > to
> >
> > > my supervisor before but she can't help me and she wouldn't allow me to
> > > change the way I approach my project. Everytime I tell her that my
> > > project is difficult, she'll just think that i'm lazy and i'm not
> > > trying hard enough. Anyway what u suggested cant be done as I've
> > > already mention it earlier but thank you so so much.
> > >
> > > Regards,
> > > Tan Yi Yong
> > > The University of Sheffield
> > >
> > >
> > > ^--------------------------------------------------------
> > >
> > > | XANSYS - www.xansys.org |
> > > | The Discussion List for users of ANSYS, Inc. Software |
> > > | Hosted by PADT - www.padtinc.com |
> > >
> > > ^--------------------------------------------------------
> >
> > --
> > Peter Attar
> > Assistant Professor
> > The University of Oklahoma
> > Dept. of Aerospace and Mechanical Engineering
> > 865 Asp Avenue, Felgar Hall Room 212
> > Norman,OK 73019-1052
> > phone: 405-325-1749
> > fax: 405-325-1088
--
Peter Attar
Assistant Professor
The University of Oklahoma
Dept. of Aerospace and Mechanical Engineering
865 Asp Avenue, Felgar Hall Room 212
Norman,OK 73019-1052
phone: 405-325-1749
fax: 405-325-1088
^--------------------------------------------------------
| XANSYS - www.xansys.org |
| The Discussion List for users of ANSYS, Inc. Software |
| Hosted by PADT - www.padtinc.com |
^--------------------------------------------------------