Discussion Forum

Hi,

To connect an assembly, you need two steps:

1. Create Identity pairs under Definitions. The automatic generation is useful.

2. Use the identity pairs in a Continuity pair feature in the Solid Mechanics interface.

The coupling algorithm is not symmetric, so for optimal accuracy you should put the boundaries with the finer mesh on the destination side of the pairs.

Regards,
Henrik

Dear Henrik,

Thank you for the prompt reply. May I ask when is it recommended t use identity pairs and later define rigid connections? Is this determined as a kinematic link of coordinate systems of each doamin and is more suitable for MBD?

Contiuity pairs return the same results (which is great), however the first eigenfrequency is defined only as imaginary value. Based on the eigenfrequency theory each frequency for a fixed structure should be composed from a real and an imaginary value.

Copy/paste from documentation:
----
If damping is included in the model, an eigenfrequency solution returns the damped eigenvalues. In this case, the eigenfrequencies and mode shapes are complex. A complex eigenfrequency can be interpreted so that the real part represents the actual frequency, and the imaginary part represents the damping. In a complex mode shape there are phase shifts between different parts of the structure, so that not all points reach the maximum at the same time under free vibration.

It is possible to compute eigenfrequencies for structures which are not fully constrained; this is sometimes referred to as free-free modes. For each possible rigid body mode, there is one eigenvalue which in theory is zero.
----

So if I understand correctly, when results for (let's say) 6 eigenfrequencies are obtained and some of them include imaginary part and some not, this means that the real values are not affected by damping of the fixation? Ansys works in a differetn way and always returns only real values, that's why I am confused... I guess these values already include the imaginary part...


--
Kind regards,

Matej

Hi,

1. An Identity pair+Continuity will provide a transition which is 'soft'. The results will be the same as with a union, except for local disturbances caused by the fact that the meshes on the two sided to not match. Typically, the stiffness of the structure is well represented, while the stresses show significant oscillations one or two elements away from where the boundaries are 'glued together'.

You could choose to connect the two matching boundaries with a Rigid Connector, but that will significantly stiffen the structure, since both boundaries are now infinitely stiff and move together like a rigid body.

2. Unless you have explicitly entered damping in your model, all eigenfrequencies should be real. With a reasonable amount of damping, the imaginary part should still be smaller than the real part.

If there are possible rigid body motions, then the corresponding eigenfrequencies are theoretically zero. Numerically they will however appear as a very small number which may be placed in an arbitrary direction in the complex plane. To me, it sounds like the first eigenfrequency in your model may be such a rigid body mode.

See also the discussions in

www.comsol.com/community/forums/general/thread/42331

and

www.comsol.com/community/forums/general/thread/31634

Regards,
Henrik

Dear Henrik,

I can follow the discussion here since I had the same experience when I switched to Comsol from Ansys.

There are two points which may be confusing:
1- The imaginary Eigen frequencies
2- Application of identity pair

We are used to interpret the imaginary part of the Eigen frequency as the displacement of the peaks and the nodes as a function of time in the presence of damping. It confused me at the beginning till I have realized that the identity pair setting was introducing “damping” into my system since the mismatch of the finite element solution points over the boundaries. In Ansys, there are no surface contacts, but finite element node point contacts, therefore such “loss” is avoided by default I guess.

Application of identity pairs, although it may be as straight forward as it may be, sometimes introduces inconsistencies depending on how they are defined. Again, when we defined a “pair” in Ansys, there was no definition of a “direction” as in “Source” and “Destination”. Despite the clarification in the manual, this can be overlooked quite often and can give different results, depending on the model, when the source and destination boundaries are exchanged within each other.

I just wanted to share my experience on this topic.

Regards,
Onur

Dear Matej and Onur,

Complex valued eigenfrequencies should in structural mechanics only appear in the following cases

a) There is explicit damping in the model (e.g. by adding a Damping subnode to the material, by entering complex valued stiffnesses, or by entering damping data in a Spring Foundation)

b) The model is not fully constrained, so that there are rigid body modes in the problem

c) The problem is numerically ill posed, e.g. when the stiffness matrix is almost singular.

d) It is a multiphysics model, where other physical phenomena contribute to the damping.

The use of continuity pairs should not introduce any artificial damping. The choice of Source and Destination in the pair will not affect the eigenfrequencies significantly, unless the difference in mesh density between the two boundaries is very large. A rough way of explaining the effect in that case is to think of it as if there are spot welds at the nodes on the destination side.

If you (or someone else) experience complex valued eigenfrequencies in other situations than the ones listed above, please submit the model to support.

Regards,
Henrik

Thank you for all yor responses and replies.

--
Kind regards,

Matej