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 The information provided may be out of date.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.
No convergence using Rigid Connector in simple beam
Posted Nov 14, 2011, 11:27 p.m. EST Studies & Solvers, Structural Mechanics Version 4.2 6 Replies
Please login with a confirmed email address before reporting spam
Hi all! I am having converge problems for even the simplest geometries when using the Rigid Connector element for applying forces and/or moments.
For instance, I tried to calculate the spring constants for a simple beam when used as a flexural and as a torsional spring. I applied a Fixed constraint to one face of the beam and a Rigid Connector to the opposite face. For the flexural case, I defined a unit Applied Force on the Rigid Connector, and a unit Applied Moment for the torsional case.
As you can see form attached projects, in neither case I am able to make the program converge to a solution. I have tried incrementing the number of iterations without success. Due to the simplicity of the models, I suspect I am missing something very basic about constraints!
Any ideas on how I could achieve convergence when using Rigid Connectors?
Thanks in advance for any help!
George.
P.S. For those who wonder, I am trying to use the Rigid Connector element in a more complex model in order to apply moments. I was not able to achieve convergence then, so I decided to try using first this element in some very basic model. I want to avoid having to apply explicit forces to the model to emulate the effect of moments, because of their potential effects on the points near the application points. Also, the Comsol documentation states explicitly that this is the element to use for defining applied moments.
For instance, I tried to calculate the spring constants for a simple beam when used as a flexural and as a torsional spring. I applied a Fixed constraint to one face of the beam and a Rigid Connector to the opposite face. For the flexural case, I defined a unit Applied Force on the Rigid Connector, and a unit Applied Moment for the torsional case.
As you can see form attached projects, in neither case I am able to make the program converge to a solution. I have tried incrementing the number of iterations without success. Due to the simplicity of the models, I suspect I am missing something very basic about constraints!
Any ideas on how I could achieve convergence when using Rigid Connectors?
Thanks in advance for any help!
George.
P.S. For those who wonder, I am trying to use the Rigid Connector element in a more complex model in order to apply moments. I was not able to achieve convergence then, so I decided to try using first this element in some very basic model. I want to avoid having to apply explicit forces to the model to emulate the effect of moments, because of their potential effects on the points near the application points. Also, the Comsol documentation states explicitly that this is the element to use for defining applied moments.
Attachments:
6 Replies Last Post Nov 18, 2011, 3:57 a.m. EST
Please login with a confirmed email address before reporting spam
Posted:
1 decade ago
Hi
I agree when you see the rigid Connector BC one believe it should be easy to implement a torsion like that, unfortunately it does not work always that way. A rigid connector is used primarily to connect two existing boundaries with a rigid link. In Your case you have made the end rigid but you have a singularity where it is supposed to rotate. (I'm actually fighting with something very similar and still not fully happy with my understanding of the RC behaviour either)
Then pls be careful with your force values, you have defined "force linear strain" but you apply Newtons and N*m on a 10um long, 1um section beam, in compression that is 1000[GPa] load. Your Silicon with not survive that ;)
Use rather 1[uN] for small displacements, and 1E-10 N*m instead of 1 for the moments
In case of your twist rotation you need to physically fix the centre of rotation (not to be confused with where the load is applied, nor the other variable defined from where moments are calculated )
With a rigid connector its cleaner to apply a twist angle (as you define the axis of rotation) and then measure the corresponding twist moment, but I avoid twist angle "0", I mostly apply a small angle to start with.
For moment loads you can also use the Global equation mean described in the 3.5 doc, I have also left some examples in the model exchange, but these are 3.5a versions
======= update ======
Sorry I have been too quick here, it should still work as you expected
i.e. Rigid Connector on the end of your beam, but you must ensure you use a user defined centre of rotation. The funny thing is that when I load your model it never solves for moments, but when I remake a new one I manage. Note the total moment load is only some 1E-10[N*m] for 100 [mrad] twist
Note 2: mine is a v4.2a model
--
Good luck
Ivar
I agree when you see the rigid Connector BC one believe it should be easy to implement a torsion like that, unfortunately it does not work always that way. A rigid connector is used primarily to connect two existing boundaries with a rigid link. In Your case you have made the end rigid but you have a singularity where it is supposed to rotate. (I'm actually fighting with something very similar and still not fully happy with my understanding of the RC behaviour either)
Then pls be careful with your force values, you have defined "force linear strain" but you apply Newtons and N*m on a 10um long, 1um section beam, in compression that is 1000[GPa] load. Your Silicon with not survive that ;)
Use rather 1[uN] for small displacements, and 1E-10 N*m instead of 1 for the moments
In case of your twist rotation you need to physically fix the centre of rotation (not to be confused with where the load is applied, nor the other variable defined from where moments are calculated )
With a rigid connector its cleaner to apply a twist angle (as you define the axis of rotation) and then measure the corresponding twist moment, but I avoid twist angle "0", I mostly apply a small angle to start with.
For moment loads you can also use the Global equation mean described in the 3.5 doc, I have also left some examples in the model exchange, but these are 3.5a versions
======= update ======
Sorry I have been too quick here, it should still work as you expected
i.e. Rigid Connector on the end of your beam, but you must ensure you use a user defined centre of rotation. The funny thing is that when I load your model it never solves for moments, but when I remake a new one I manage. Note the total moment load is only some 1E-10[N*m] for 100 [mrad] twist
Note 2: mine is a v4.2a model
--
Good luck
Ivar
Attachments:
Please login with a confirmed email address before reporting spam
Posted:
1 decade ago
Hi Ivar!
I cannot thank you enough for your help! I tried using the Prescribed Rotation approach, but still had problems. I then tried to open your working solution, but unfortunately I cannot since I only have access to version 4.2. Could you please save it in this version format, or (in case not) describe me literally how you were able to make it converge?
Thanks again for your kind help!
Regards,
Jorge.
I cannot thank you enough for your help! I tried using the Prescribed Rotation approach, but still had problems. I then tried to open your working solution, but unfortunately I cannot since I only have access to version 4.2. Could you please save it in this version format, or (in case not) describe me literally how you were able to make it converge?
Thanks again for your kind help!
Regards,
Jorge.
Please login with a confirmed email address before reporting spam
Posted:
1 decade ago
Hi
I have uninstalled my 4.2 so I'm stuck with 4.2a, works OK for me anyhow ;)
I did not do anything special, just remade it from scratch, but you need to load it with a reasonable load, try a quick hand calulation for the twist stiffness and then apply a loaed for some 10-100 mrad twist angle, and start gently ;)
--
Good luck
Ivar
I have uninstalled my 4.2 so I'm stuck with 4.2a, works OK for me anyhow ;)
I did not do anything special, just remade it from scratch, but you need to load it with a reasonable load, try a quick hand calulation for the twist stiffness and then apply a loaed for some 10-100 mrad twist angle, and start gently ;)
--
Good luck
Ivar
Please login with a confirmed email address before reporting spam
Posted:
1 decade ago
Hi
I finally understood what I was doing wrong on my side, I wonder if you are not doing partly the same error.
The Rigid Connector GUI is to interpreted as:
one make the selected boundaries RIGID (no deformation) and one define a CoR (either automatic = geometrical centre of selected boundaries, or user defined) and then all following tabs in the GUI apply only to the COR, so you can force the COR to stay fixed in space then you check all three X,Y,Z, or only one or two ...the same you can prescribe the rotations (i,.e. axis along X,Y,Z) or define your own rotation with corresponding axis.
I was getting confused as I applied, in my head, the prescribed motion directly to to the boundaries and not to the boundaries via the COR . In fact if you dig into the equations, now that we have explanations on what the different constraints apply to, and in which frame COMSOL works, you will see that the prescribed motion applies to a "Point1" that I now interpret to the COR, and not to the boundaries selected.
Note that the fact that the boundaries become rigid, makes the use of RC in TS (Thermal Stress) difficult as you are over stressing the rigid boundaries, there is a missing alpha(T) parameter for your equations.
--
Good luck
Ivar
I finally understood what I was doing wrong on my side, I wonder if you are not doing partly the same error.
The Rigid Connector GUI is to interpreted as:
one make the selected boundaries RIGID (no deformation) and one define a CoR (either automatic = geometrical centre of selected boundaries, or user defined) and then all following tabs in the GUI apply only to the COR, so you can force the COR to stay fixed in space then you check all three X,Y,Z, or only one or two ...the same you can prescribe the rotations (i,.e. axis along X,Y,Z) or define your own rotation with corresponding axis.
I was getting confused as I applied, in my head, the prescribed motion directly to to the boundaries and not to the boundaries via the COR . In fact if you dig into the equations, now that we have explanations on what the different constraints apply to, and in which frame COMSOL works, you will see that the prescribed motion applies to a "Point1" that I now interpret to the COR, and not to the boundaries selected.
Note that the fact that the boundaries become rigid, makes the use of RC in TS (Thermal Stress) difficult as you are over stressing the rigid boundaries, there is a missing alpha(T) parameter for your equations.
--
Good luck
Ivar
Please login with a confirmed email address before reporting spam
Posted:
1 decade ago
Dear Ivar,
Thanks again for your help; I finally was able to solve the problem (sorry for the delay in replying!). In the end it the problem was the magnitude of the applied force and moment. Careless as I am, I was using the same reasoning that I follow in linear simulators, where I usually set the excitation to unitary magnitude in order to ease the calculations of out/in ratios. So I basically thought that the simulation of the beam would be inherently linear, but I forgot that the elastic behavior is lost after a certain threshold in the magnitude of the excitation!
I just put some reasonable values for the applied forces and moments, and the simulation went like a breeze. :^)
Thanks again for all your suggestions!
cheers,
Jorge.
Thanks again for your help; I finally was able to solve the problem (sorry for the delay in replying!). In the end it the problem was the magnitude of the applied force and moment. Careless as I am, I was using the same reasoning that I follow in linear simulators, where I usually set the excitation to unitary magnitude in order to ease the calculations of out/in ratios. So I basically thought that the simulation of the beam would be inherently linear, but I forgot that the elastic behavior is lost after a certain threshold in the magnitude of the excitation!
I just put some reasonable values for the applied forces and moments, and the simulation went like a breeze. :^)
Thanks again for all your suggestions!
cheers,
Jorge.
Please login with a confirmed email address before reporting spam
Posted:
1 decade ago
Hi
I manage also, as I was stuck in parallel on something similar, finally the most of the RC page prescribed displacement rotations applies to the CoR centre of rotation and not to the selected boundary. I was also quite confused
Now its sorted out, and I have suggested to COMSOL that they improve the wording to make this unambiguous, we will see what arrives in next version ;)
--
Good luck
Ivar
I manage also, as I was stuck in parallel on something similar, finally the most of the RC page prescribed displacement rotations applies to the CoR centre of rotation and not to the selected boundary. I was also quite confused
Now its sorted out, and I have suggested to COMSOL that they improve the wording to make this unambiguous, we will see what arrives in next version ;)
--
Good luck
Ivar