XANSYS Message: 93158 [Go back to message list] [bookmark on del.icio.us]
No rating yet Subject: Re: [STRUC] Bonded contacts Author: Dimitris Panagiotopoulos Date: 2008-05-05 23:00:58Hello Christiane The bonded contact (full bonded) doesn't permit any sliding or separation once contact is established that is why you don't see any "micromotions". This is not physics. It is a mathematical constraint you put into the model and it has nothing to do with standard (frictional or not) contact. This constraint is clear if you think of the basic equation of contact P=Kn*Un when Un (contact gap size) less or equal to zero and Kn the contact stiffness. When a bonded contact then P=-Kn*Un if Un greater than zero. That is all, the program keeps calculating negative (tensile) contact traction due to adhesion you put. In the standard contact the code puts the P zero value when Un greater than zero. The amplitude of the Kn and P depends only on the deformation of the contact surfaces and are calculated in the same way as in standard contact with negative sign. Please note that in this method you can't model physical behaviour of the "glue" because you order the contact surfaces to stay together and they will. This method is usefull only if you want to study the stress and deformation field of the elastic bodies due to adhesion tensile stresses assuming ideal adhesion. Otherwise you have to model the "glue" between the bodies as a third body and solve for two contact pairs. The Computational Contact Mechanics is a difficult discipline and requires attention. You must always understand the physics of your problem and the scope of your study before you set the model. See P. Wriggers "Computational Contact Mechanics" for more understanding on contacts with FEM.
Best regards
Dimitris Panagiotopoulos HAF Greece
Quoting Christiane Caouette :
> Hello everyone, > > Joseph: Yes, I did read section 14.174. It is very complete in almost > every aspect of contact technology in Ansys (I must add release 11 is > greatly improved compared to 10!). The only missing info in there is > about contact surface behavior (bonded, standard, rough...): they only > say that "contact points are attached" for bonded contact, whatever that > means... > > Martin: You're absolutely right; I did all that testing during my > master's... :-) . To simulate primary stability (the implant's just > been put in, no cellular reaction yet), standard contacts did a fine job > as long as FKN and FKT where properly set. But if I use bonded contacts > (with penalty algorithm and same FKN/FKT), micromotions (contact sliding > distance) drop to almost nothing. That is the behavior I need to explain > mathematically. > > Paris: I had no idea LSDyna could do that sort of stuff, I will look > into it, because damage control/induced is exactly what I need. As for > papers on this subject, most of them focus on primary stability and try > to reproduce lab experiments with composite femurs; there's no > osseointegration, it's simple classic contact mechanics, so they do it > with contact elements, most of the time not saying what values they used > as parameters. You'll find those all over the place (just type something > like "hip stem model"...), but primary stability is the easy part. > > I found only a couple of papers dealing with osseointegrated implants: > the most interesting is a series of paper by Moreo and Doblar?. They use > what they call an "interface element", but I think they programmed it > themselves, it has little to do with Ansys inter20X elements. It's based > on the same principles, but they use the damage variable d as a bonding > degree, with their own behavior law (I can only use bilinear or > exponential models in Ansys). > > So, to summarize: Paris seems to have the key to my problem, I'll go > look in LS-Dyna, and give the list an update when I know more... > probably a couple weeks from now! > > Thanks everyone! > Christiane Caouette > PhD Student at ?cole de Technologie Sup?rieure > >> Hi Christiane, >> If ANSYS is not an option due to limitations of its contact >> algorithms you may want to try LsDyna that has different contact >> types that account for separation under controlled situations. >> The LSDyna may be an overkill but the types of contact algorithms >> it offers are more appropriate for your type of problem. You want >> erosion-type or damaged-induced/controlled contact resolutions >> that I know LsDyna can help. It appears that your problem is not >> centered in the contact interface per se but more so in its the >> existence or absense and the effect it has to the parts at the >> interface. >> >> Having said all that, I know that pretty soon I'll run into a >> paper/work by someone in your field for the very similar problem >> that was done in ANSYS. >> >> Incidentally, what is the literature search showing as far as >> handling problems like yours ?? What other codes engineers in your >> field use for similar problems ??? >> >> Regards, >> Paris Altidis >> Belcan Corp. >> 630-786-0008 >> >> >> > ^-------------------------------------------------------- > | XANSYS - www.xansys.org | > | The Discussion List for users of ANSYS, Inc. Software | > | Hosted by PADT - www.padtinc.com | > ^--------------------------------------------------------
^-------------------------------------------------------- | XANSYS - www.xansys.org | | The Discussion List for users of ANSYS, Inc. Software | | Hosted by PADT - www.padtinc.com | ^--------------------------------------------------------