Note: This discussion is about an older version of the COMSOL Multiphysics® software. The information provided may be out of date.
Discussion Closed This discussion was created more than 6 months ago and has been closed. To start a new discussion with a link back to this one, click here.
structural mechanics: rotation w/ rigid connector - unexpected behaviour
Posted 31 ott 2014, 11:07 GMT-4 Structural Mechanics Version 4.3a 3 Replies
Please login with a confirmed email address before reporting spam
Hi all,
attached you'll find a 2D model where I attempt to rotate a quarter circle around its centre.
With a
- rigid connector that rigidly connects it outer perimeter with the origin and centre
- a prescribed rotation of 2*pi*t[1/s] radians
- and a time range from 0 to 1 s,
I expect the section to revolve around its centre. Instead, it does only rotates a little less than 0.5*pi radians, while growing in radius.
What causes this problem? Is something wrong with my assumptions or definitions? Or is this expected behavior, perhaps due to linearisation of the rotation matrix? Is there any work-around?
This thread deals with pretty much the same problem, but no solution is offered:
www.comsol.com/community/forums/general/thread/23995
All help appreciated. Regards, Rolf
attached you'll find a 2D model where I attempt to rotate a quarter circle around its centre.
With a
- rigid connector that rigidly connects it outer perimeter with the origin and centre
- a prescribed rotation of 2*pi*t[1/s] radians
- and a time range from 0 to 1 s,
I expect the section to revolve around its centre. Instead, it does only rotates a little less than 0.5*pi radians, while growing in radius.
What causes this problem? Is something wrong with my assumptions or definitions? Or is this expected behavior, perhaps due to linearisation of the rotation matrix? Is there any work-around?
This thread deals with pretty much the same problem, but no solution is offered:
www.comsol.com/community/forums/general/thread/23995
All help appreciated. Regards, Rolf
Attachments:
3 Replies Last Post 3 nov 2014, 11:21 GMT-5
Please login with a confirmed email address before reporting spam
Posted:
10 years ago
Hi,
You have forgotten to select "Include geometric nonlinearity", so your suspicion about linearization was right.
Regards,
Henrik
You have forgotten to select "Include geometric nonlinearity", so your suspicion about linearization was right.
Regards,
Henrik
Please login with a confirmed email address before reporting spam
Posted:
10 years ago
Hello Henrik,
thank you, this solved this issue. The follow-up question is about the attached model.
With the 'Rigid domain' and 'Quasi-static' options checked I expect no stresses. However, the solution shows a mesh-dependent and time-dependent stress state, so it is rigid nor quasi-static. Any help on specifying
- rigidity, and
- ignoring inertial terms
for structural element?
Again, any help much appreciated.
Regards, Rolf
thank you, this solved this issue. The follow-up question is about the attached model.
With the 'Rigid domain' and 'Quasi-static' options checked I expect no stresses. However, the solution shows a mesh-dependent and time-dependent stress state, so it is rigid nor quasi-static. Any help on specifying
- rigidity, and
- ignoring inertial terms
for structural element?
Again, any help much appreciated.
Regards, Rolf
Attachments:
Please login with a confirmed email address before reporting spam
Posted:
10 years ago
Hi Rolf,
The 'Rigid Domain' subfeature in the 'Rigid Connector' only computes the inertial properties for the domain(s) selected, and adds them to the properties of the Rigid Connector. It does not automatically make the domain rigid though. The elastic equations are still solved in that domain. To avoid that, the domain must be deselected at the physics interface level. An example of this can be seen in the Model Library model 'rigid_domain'.
From version 4.4, there is a new material model called 'Rigid Domain', which behaves as what I believe you were looking for. It is not used in conjunction with a Rigid Connector. From version 4.4, the example 'rigid_domain' has also been changed, to instead make use of this new feature.
Now some comments to why you see stresses in what should be a stress-free rotation:
1. The numerical solution of your problem will only be accurate to some numerical precision. If you tighten the tolerances, the stresses will decrease. With large rigid body rotations, the displacements must be correct to a very high accuracy, in order to produce strains which are almost zero.
2. You are solving a quasistatic problem with a time-stepping solver. This is not wrong, but it is not optimal. The step size and convergence criteria of such a solver are tuned for looking at time derivatives. A problem like this should preferably be solved by using a stationary study with a parametric continuation solver.
3. If you still want to use a time dependent solver, the BDF solver is the preferred choice. The Generalized Alpha solver is best for problems having second order time derivatives, as a dynamic mechanical problem usually has.
In order to solve a problem like this with a time dependent solver, you should change some of the settings for the nonlinear solver. Allow more iterations (say 25), and use the Automatic Newton scheme. The default values are tuned for true structural dynamics. You you could look at the default settings generated for a stationary case to find good values.
Regards,
Henrik
The 'Rigid Domain' subfeature in the 'Rigid Connector' only computes the inertial properties for the domain(s) selected, and adds them to the properties of the Rigid Connector. It does not automatically make the domain rigid though. The elastic equations are still solved in that domain. To avoid that, the domain must be deselected at the physics interface level. An example of this can be seen in the Model Library model 'rigid_domain'.
From version 4.4, there is a new material model called 'Rigid Domain', which behaves as what I believe you were looking for. It is not used in conjunction with a Rigid Connector. From version 4.4, the example 'rigid_domain' has also been changed, to instead make use of this new feature.
Now some comments to why you see stresses in what should be a stress-free rotation:
1. The numerical solution of your problem will only be accurate to some numerical precision. If you tighten the tolerances, the stresses will decrease. With large rigid body rotations, the displacements must be correct to a very high accuracy, in order to produce strains which are almost zero.
2. You are solving a quasistatic problem with a time-stepping solver. This is not wrong, but it is not optimal. The step size and convergence criteria of such a solver are tuned for looking at time derivatives. A problem like this should preferably be solved by using a stationary study with a parametric continuation solver.
3. If you still want to use a time dependent solver, the BDF solver is the preferred choice. The Generalized Alpha solver is best for problems having second order time derivatives, as a dynamic mechanical problem usually has.
In order to solve a problem like this with a time dependent solver, you should change some of the settings for the nonlinear solver. Allow more iterations (say 25), and use the Automatic Newton scheme. The default values are tuned for true structural dynamics. You you could look at the default settings generated for a stationary case to find good values.
Regards,
Henrik