Simulation Mechanical Forums (Read-Only)
Welcome to Autodesk’s Simulation Mechanical Forums. Share your knowledge, ask questions, and explore popular Simulation Mechanical topics.
cancel
Showing results for 
Show  only  | Search instead for 
Did you mean: 
Reply
Message 1 of 18
yasmind
1055 Views, 17 Replies

surface contact

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.

17 REPLIES 17
Message 2 of 18
zhuangs
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

Message 3 of 18
yasmind
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.

 

 

Message 4 of 18
zhuangs
in reply to: yasmind

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

 

-Shoubing

Message 5 of 18
yasmind
in reply to: zhuangs

Hope these help!

Message 6 of 18
yasmind
in reply to: yasmind

and this is a typical resulting displacement graph..

Message 7 of 18
AstroJohnPE
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.

Message 8 of 18
yasmind
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? 

Message 9 of 18
yasmind
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.

Message 10 of 18
AstroJohnPE
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.)

 

Message 11 of 18

Message 12 of 18
yasmind
in reply to: ilyas_drawbridge

Hello,

Thank you for your messages. 

The major problem now is that the stiffness values assigned to those weak springs between the parts that only depend on friction do not affect my results to a large extent. However, the coefficients of friction do not have any effect at all. So, I believe my contacts still do not work properly.

Message 13 of 18
AstroJohnPE
in reply to: yasmind

Hi,

 

"the stiffness values assigned to those weak springs ... do not affect my results". I think that is good! The springs are not suppose to "change" the results other than to create a statically stable model. If you make the springs too stiff, then part of the load is transmitted to the ground through the springs, and that makes the model inaccurate compared to reality.

 

"the coefficients of friction do not have any effect at all". What motion is the friction supposed to affect?

 

I think we will not know for sure what the results are showing until you provide an archive of the model (amazing that no one suggested an archive before now, see Create, Post, or Provide an Archive of your model) or some results images that show the legend.

 

Thanks Ilyas. You found the thread regarding "rotation results" that I could not find.

Message 14 of 18
yasmind
in reply to: ilyas_drawbridge

Hi,

Again thank you very much for your replies. John, yes, it was a displacement graph, just to give you an idea how the things were going.

I have different loading schemes to simulate, one of which is an out of plane load, applied on one face of the top horizontal element. In this case I changed the option in the 3d springs, assigned to the model for surface contacts to work, from translation to rotation, but once again, I experience my initial problem (pins go out of their places, please see the attached figure). I tried to increase the stiffness values even excessively, but the results do not change.

Thanks.

Message 15 of 18
yasmind
in reply to: AstroJohnPE

By the way, while saying that the value of friction coefficient does not effect the results, I meant that I change the friction between different parts in my model, i.e. pins and other elements, etc, but I always get the same results. The coefficient of friction should make a difference, as the frame displaces, i.e. as the pins rotate in the mortices, and different parts rub against each other. Right?

Message 16 of 18
AstroJohnPE
in reply to: yasmind

It could be that the friction force is not large enough to prevent motion. Since the analysis type is static, and because their is no sliding coefficient of friction (at least not in linear static stress), the friction force goes to 0 if the friction force is not large enough to prevent motion.

 

By the way, did you specify a "shrink fit" type of contact for the mortice joints? Without that, would there be any loads that create a normal force needed to create a friction force?

Message 17 of 18
AstroJohnPE
in reply to: yasmind

Rotational constraints have no effect on brick elements (or tetrahedron elements). So essentially your pins had no constraints, and you were back to the original problem.

 

Three points (not in a straight line) held in X, Y, and Z translation (with weak springs in this case) are sufficient to prevent rigid body motion. Hopefully, this will give better results.

 

Message 18 of 18
yasmind
in reply to: AstroJohnPE

Hi,

Sorry for my late reply.

Again for my frame under out-of-plane loading:

I changed my weak springs so as to have translational constraints rather than radial ones as you said, and I changed all my contact options into shrink fit with an automatic interference. 

However, if I leave the stiffness values as s I used in in plane lateral loading case, the pins do not move together with the rest of the frame, which gets displaced in the out of plane direction (see the last attached figure). And if I increase the stiffness to prevent this, then the whole model becomes extremely and unrealistically rigid.

Another problem is the interference value. A very small change in interference change drastically all the results.

Do I have to carry out a nonlinear MES analyses in order to make sure that sliding works correctly?

 

 

Can't find what you're looking for? Ask the community or share your knowledge.

Post to forums  

Autodesk Design & Make Report