Open FE-System for transient simulations (thermal+structural) 3

Every time step of a transient solution is just like a new solution of your model: so you should simply discard the transient functionalities of your code for both model setup and analysis of results and treat each step as a new calculation where the initial conditions come from the preceding step.
You should be able to do this with any FE code, and indeed ANSYS would allow to write general routines to automate the process, though this would be quite complex to do for a general case.
Of course you'll have to resolve many issues: how to account for initial conditions of new and dead boundary conditions and/or elements, print at every step all the results you need, as they won't be available any more, etc. prex
motori@xcalcsREMOVE.com
Online tools for structural design

Toothroot,

Prex is right.... sounds like your trying to do an analysis of a welding process, or something similar, with metal added to the weld pool as the heat source moves along. Most codes should be able to accomadate this - I've personally done somethign similar with ABAQUS, using the methodology described by Prex...... Its not pretty to setup, but then end results can be very good.

GJS

Thank you very much for your replies, Prex and GJS. Actually, I don't want to simulate a welding process but a material removal by a cutting process. Therefore I need to erase certain elements after each time step. This has to be done automatically since I can't set-up a new model after every time step (I expect to simulate at least 10 or 20 steps).
It seems to me that most of the "big players" of FE programmes can accomodate such an analysis. From what Prex wrote, ANSYS should be alright. But I guess that I can do the same with ABAQUS or NASTRAN, when I programme a routine that stops the calculation after every time step and changes the mesh via the input deck file. That promises to become a very nasty sort of simulation (lot of things can go wrong), but it should be possible to be implemented.

GJS: You wrote that you have done something similar for a welding simulation. Do you have any publications or material I can access via the net? This would be very helpful for me, thanks in advance.

Any further tips for this topic are still highly welcome!

Thanks again,
Daniel

Toothroot,

Think I've post this site on another thread, but..


etc is worth a look as it provides sample ABAQUS decks of the code used in this chaps PhD. In ABAQUS the methodology for adding/removing elements is to define all the element you will ever need at the start, then use the *MODEL CHANGE keyword to add and remove elements in each step. This is fine if you know which/how many elements will be added (or in your case removed) in each step, which I'm guessing you'll know if your cutting operation is proceeding at something approaching a constant speed.

Hope this info helps... and good luck!!!

GJS

p.s. I take it you actually want stress/deformation data, hence the need for FEA. If you just want to visualise a cut path from the known movement of your cutter, most CAD packages could be an easier way to go. I've done this in SolidWorks, with very nifty looking results!!

toothroot,
Your problem can be completed two ways :
1. Using parametric options in ANSYS, of course also in PATRAN (but this rather complex), i.e. you model the changing portion of your structure parametrically. So you just need to change this parameter in every step. We have done similar job, i.e. adding and removing stringer from a plate structure in every iteration (step).
2. Using paramtrized CAD tools, such Pro/E, to generate the geometry, export it in to a Pre/Processor and finally mesh it. We have done also such a job. The disadvantage is of course, you need more sotwares to accomplish the job ;-)

cheers

toothroot,
the birth and death feature of ANSYS in each of the different load steps can help to get you a solution.
the birth and death feature in Ansys works in the same manner as what GJS has mentioned

great nicolas, i have over seen this ANSYS capability. Btw, it works only if you also know which elements should be died, so you need parameters too, isn't it?

cheers

There is at least one code that was designed to do this sort of analysis, look at DEFORM uses damage techniques to decide when an element needs turning off - e.g. if the strain in an element reaches a certain value it is assumed to have failed. You may be able to use similar techniques with other codes. Certainly in ABAQUS/Explicit the '*Shear Failure' and/or '*Tensile Failure' can be used. If this is a fast cutting process it may be worth considering explicit codes because of the ease that they deal with complex contact and other non-linearities.
TERRY