XANSYS Message: 93193 [Go back to message list] [bookmark on del.icio.us]
No rating yet Subject: Re: [STRUC] Bonded contacts Author: Odd Einar Lindøe Date: 2008-05-06 20:21:31Hi again. I still doesnt see the big fuzz. The bonded contact is like springs in the 3 directions and you need to adjust stiffness(force) to an acceptable relative movement between the contact elements. There will always be some movements for such a penalty/augumented contact since you apply an adjustment to the Force/Area^3 for the relative closing/opening/sliding between the elements. If you perform it perfect the stress distrubution over the interface should be without any sudden gradients (like it was meshed together without contact). All relative sliding/movements are just producing error.
I cannot help you with exactly how ansys connects a contact/target element and i guess you need to ask the question to one of the Ansys code people.
I suppose your implant is close to bonded in the beginning but moves to frictional when its disintegrating. Perhaps the de-bonding feature of the contact is more applicable?.
Brgds O.E.Lindoe,ImencoAS
----- Original Message ----- From: "Christiane Caouette" To: "ANSYS User Discussion List" Sent: Tuesday, May 06, 2008 9:36 PM Subject: Re: [Xansys] [STRUC] Bonded contacts
Yup, that's exactly the feature I was interested in using. The only problem is that I need to know how Ansys calculates its glued contacts before I use them; there are enough ambiguous papers of hip stem models with "bonded contacts" as it is... I built a small model to experiment with that feature; just two beams of different mesh size connected with bonded contacts and a cohesive zone material model. It works great, but I need to be able to justify using it; which means explaining how they work. "Glued", meaning a rule of no relative slinding is enforced, I suppose.
Regards, Christiane
> Just out of courosity... Are you comparing a standard (frictional) > contact with a bonded(glued) > contact ? (or did i miss something along the way). > > Perhaps the de-bonding feature of a bonded contact element could help > you? > > Brgds O.E.Lindoe,ImencoAS > > ----- Original Message ----- From: "Christiane Caouette" > > To: "ANSYS User Discussion List" > Sent: Monday, May 05, 2008 10:00 PM > Subject: Re: [Xansys] [STRUC] Bonded contacts > > >> 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 Doblaré. 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 École de Technologie Supérieure >> >>> 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 | >> ^-------------------------------------------------------- > > >
--
Christiane Caouette, ing. jr
/Doctorat Génie Biomédical/
/École de Technologie Supérieure/
/Institut des Matériaux Industriels - CNRC/
(450)641-5807
_Christiane.Caouette___at_cnrc-nrc.gc.ca_
^-------------------------------------------------------- | 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 | ^--------------------------------------------------------