XANSYS Message: 42307 [Go back to message list]
No rating yet
Rate item:

Subject: Re: contact stiffness, convergence, and solution time.
Author: Bill Bulat
Date: 2002-09-30 13:17:00

Sheldon kindly passed some additional info to me a short while ago:

Hi Bill,

Saw your XANSYS posting. Sparse solver does not create a .tri file, so
that's why you don't see one.

Expansion pass can be done with the sparse solver or with the PCG solver. If
the .LN22 file exists, the sparse solver will be used for back-substitution.
If no .LN22 file exists, the PCG solver will be used by doing a static
re-solve to get the solution.

Laters,

Shelly

Thanks Shelly!

cheers,

Bill Bulat
ANSYS Inc.

----- Original Message -----
To:
Sent: Monday, September 30, 2002 12:56 PM

> Hi Roberto,

> The sparse solver may be used in a generation pass at release 6.1 (it's a
> beta feature).

> I tried it and it seemed to work with a very small test model. I don't see
a
> .tri file in my working directory however. Presently, I'm not certain you
> could do an expansion pass (I believe you need the .tri file for that).
You
> CAN do a use pass, however. If you have 6.1 and don't need to do an
> expansion pass, you might consider substructuring.

> Bill Bulat
> ANSYS Inc

> ----- Original Message -----
> From: "Roberto Porto"
> To:
> Sent: Monday, September 30, 2002 11:28 AM
> Subject: Re: [xansys] RE: contact stiffness, convergence, and solution
time.

> > I tryed to use substructuring tecnique, but I gave up because it is
still
> > using the frontal solver and has a limit on the number of elements used
> > (46000), which made it much slower than solving the full model with
sparse
> > solver.
> > The substructure method doesn't allow you to choose the solver.

> > Regards,

> > Roberto Porto
> > DSC Engenharia

> > ----- Original Message -----
> > From: "Newland, Bill"
> > To:
> > Sent: Monday, September 30, 2002 11:48 AM
> > Subject: RE: [xansys] RE: contact stiffness, convergence, and solution
> time.

> > > It's been a long time since I have done substructuring. Another
> limitation
> > > of the frontal solver which was also the only solver available for the
> USE
> > > pass was a limitation on the master degrees of freedom. I recall
hitting
> > > this limitation quickly with Contact52's in the USE pass interfacing
> solid
> > > model portions defined as superelements.

> > > I was under the impression that Substructuring had become somewhat
> > obsolete
> > > with the advent of Solid92's and new solvers, but now that the Sparse
> > solver
> > > can be utilized for the Substructuring technique - maybe this
technique
> > > should be re-evaluated as a possible method to reduce run time for
solid
> > > model assemblies interfaced with Contact170/174's.

> > > I was wondering if anyone has had any recent Substructuring experience
> in
> > > this regard.

> > > Bill Newland
> > > Bell Helicopter, Textron

> > > -----Original Message-----
> > > From: Metrisin Joe [mailto:jmetrisin@f...]
> > > Sent: Friday, September 27, 2002 7:06 AM
> > > To: 'xansys@yahoogroups.com'
> > > Subject: [xansys] RE: contact stiffness, convergence, and solution
time.

> > > Several years ago, I wrote a macro that would automatically
substructure
> a
> > > contact problem so that once the superelements were generated, you
only
> > had
> > > to iterate on the contact elements. It wasn't very efficient because
> you
> > > had to use the frontal solver for the generation pass, which was about
> 20x
> > > slower than solving the entire model once with the PCG solver.

> > > The latest version of ANSYS now lets you do superelement generation
with
> > the
> > > sparse solver, so it might be worth trying this technique again.

> > > Joe Metrisin
> > > Florida Turbine Technologies, Inc.

> > > Date: Thu, 26 Sep 2002 13:20:17 -0500
> > > From: "Newland, Bill"
> > > Subject: contact stiffness, convergence, and solution time.

> > > My compliments to Don Shaffer on expounding the need of faster
solution
> > > time for detailed models with contact elements!

> > > Thanks to CAD transfers, automatic tetrahedron element meshing, and
> > contact
> > > elements - we are finally able to model interconnecting machine
> components
> > > as they really are. Now, if we could just do it without tying up our
> > > computers for days.

> > > One model I solved recently has about 800,000 dof's , 41 Contact
170/174
> > > interface sets, and about 20,000 Contact 170/174 elements. I did get
> good
> > > results - but it took 6 cpu DAYS on an SGI Octane. Substantial
modeling
> > work

> > > was expended to get the model size down without deleting important
> detail.
> > > While it is amazing that ANSYS can solve a problem like this at all, a
> > much
> > > faster turn around time is required in order to be practical.

> > > Bill Newland
> > > Bell Helicopter, Textron
Posts possibly associated with message #42307AuthorDateScore
42208contact stiffness, convergence, and solution time.Bill Newland2002/09/26 
42209Re: contact stiffness, convergence, and solution time.Dan Bohlen2002/09/26 
42210Re: contact stiffness, convergence, and solution time.Bill Kelly2002/09/26 
42228Re: contact stiffness, convergence, and solution time.Joe Metrisin2002/09/27 
42241Re: contact stiffness, convergence, and solution time.Bill Kelly bill.kelly@2002/09/27 
42303Re: contact stiffness, convergence, and solution time.Roberto Porto2002/09/30 
42306Re: contact stiffness, convergence, and solution time.Bill Bulat2002/09/30 
42307Re: contact stiffness, convergence, and solution time.Bill Bulat2002/09/30 
42315Re: contact stiffness, convergence, and solution time.Roberto Porto2002/09/30