Simulation Mechanical and Multiphysics

Reply
Contributor
yasmind
Posts: 23
Registered: ‎02-04-2013

surface contact

682 Views, 17 Replies
02-04-2013 09:03 AM

Hi,

I have a timber frame model with morticed pin connections and trying to run a linear analysis. I defined surface contact between mortices, pins and timber elements with a certain coefficient of friction. However, (1) although my geometry and loading scheme is completely symmetrical, one of the pins, located on one corner, comes out of its place, while the others stay, and (2) during the analysis I always get the error message saying that "the matrix is highly ill-conditioned/singular".

What should I do to improve my model?

Thanks.

Please use plain text.
Employee
zhuangs
Posts: 209
Registered: ‎10-04-2010

Re: surface contact

02-05-2013 12:12 PM in reply to: yasmind

 Whether the model is well constrained (no rigid body motion)?

 Or you can try to use the symmetrical model with symmetrical constrain set up?

 

-Shoubing

Please use plain text.
Contributor
yasmind
Posts: 23
Registered: ‎02-04-2013

Re: surface contact

02-05-2013 12:34 PM in reply to: yasmind

Hi,

Thank you for your message. 

The bottom timber element is fixed to the ground. So there must not be any rigid body rotation, except for the pins that might be rotate inside the mortices, as the system displace.

But what I get at the end of the analyses either the pins come out of their place (move longitunally rather than radially), or they get swelled, i.e. get larger in diameter.

I repeated my analyses by different surface to surface contact options (threshold tolerance, stabilization method etc.) but I still experience the same problems.

 

 

Please use plain text.
Employee
zhuangs
Posts: 209
Registered: ‎10-04-2010

Re: surface contact

02-05-2013 12:41 PM in reply to: yasmind

Please attach a figure of the model for me to take a look?

 

-Shoubing

Please use plain text.
Contributor
yasmind
Posts: 23
Registered: ‎02-04-2013

Re: surface contact

02-05-2013 12:50 PM in reply to: zhuangs

Hope these help!

Please use plain text.
Contributor
yasmind
Posts: 23
Registered: ‎02-04-2013

Re: surface contact

02-05-2013 12:54 PM in reply to: yasmind

and this is a typical resulting displacement graph..

Please use plain text.
Valued Mentor
AstroJohnPE
Posts: 490
Registered: ‎08-30-2012

Re: surface contact

02-05-2013 08:13 PM in reply to: yasmind

The rigid body motion or ill-condition matrix is most likely due to the pins. Surface contact in linear stress is an iterative solution. If there are not enough contact elements "engaged" on iteration N, then the pin can experience rigid body motion.

 

The solution is to follow the suggestions on this page in the documentation: Perform Analysis with Gap Elements.

John Holtz, PE
Mechanical Engineer
Pittsburgh, PA

16 years experience with Simulation Mechanical
Please use plain text.
Contributor
yasmind
Posts: 23
Registered: ‎02-04-2013

Re: surface contact

02-06-2013 02:21 AM in reply to: yasmind

The page solved my problems to a large extent.. Thank you! However, after a certain point, the situation got insensitive to stiffness change, and one of my pins seems still to get larger in diameter. Might this be a solely graphic problem? 

Please use plain text.
Contributor
yasmind
Posts: 23
Registered: ‎02-04-2013

Re: surface contact

02-06-2013 04:23 AM in reply to: yasmind

I also just realized that different  coefficient of friction values do not make any difference in my results. It seems that the contacts simply don't work.

Please use plain text.
Valued Mentor
AstroJohnPE
Posts: 490
Registered: ‎08-30-2012

Re: surface contact

02-06-2013 03:19 PM in reply to: yasmind

I do not know what result is shown in 4.png. But if that is the displacement contour, it looks like the results are correct -- most likely.

 

Keep in mind that you are doing a linear analysis. The displacements are usually so small that you would not be able to see any displacement at a 1-to-1 scale. So the displacements are exaggerated with the "Results Contours > Displacement > Show Displaced > Displaced Options" command.

 

Surface contact uses springs between the parts to create the contact force. Springs require compression to create a force. So if the spring compresses 1E-6 to create the reaction force, but the displacements are exagerated by 1E+5, then it will look as if there is (1E-6)*(1E+5) = 0.1 penetration (instead of 1E-6 penetration). I believe this is what you are seeing in image 4.

 

The "Results Contours > Other Results > Element Forces > Axial Force" will show if the contact elements are in compression (a negative force) or not (0 load).

 

About the rotation and the pin "blowing up like a balloon" (my description), this is also an artifact of linear stress and exaggerating the displacements. The software calculates a "rotation" of a pin by calculating how far each node on the surface translates. With the small displacement assumption, the nodes translate in a tangential direction. So when the tangential displacement is exaggerated by a large factor, the pin appears to swell in size. (I think there is an image of this somewhere, but I could not find it. It could be in the documentation or in another thread on this Discussion Group.)

 

John Holtz, PE
Mechanical Engineer
Pittsburgh, PA

16 years experience with Simulation Mechanical
Please use plain text.