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 The information provided may be out of date.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.
Boundary conditions for 3 point bending measurement
Posted 09.07.2014, 10:37 GMT-4 Structural Mechanics Version 4.3b 2 Replies
Please login with a confirmed email address before reporting spam
Hello,
I want to simulate a simple 3 point bending test for a bulk sample using COMSOL. I want to use two rollers as the boundary conditions for boundaries 7 and 68 but I get convergence error. The simulation works if I choose either of the boundaries as fixed constraint and the other one as roller. Why can't I use just rollers which is how we do the experiment in practice?
Thanks in advance for your help
I want to simulate a simple 3 point bending test for a bulk sample using COMSOL. I want to use two rollers as the boundary conditions for boundaries 7 and 68 but I get convergence error. The simulation works if I choose either of the boundaries as fixed constraint and the other one as roller. Why can't I use just rollers which is how we do the experiment in practice?
Thanks in advance for your help
Attachments:
2 Replies Last Post 11.07.2014, 12:59 GMT-4
Please login with a confirmed email address before reporting spam
Posted:
1 decade ago
Because in practice the load that you apply will also constrain the movement of your beam in the x- and y-direction. To come closer to practice, you can put rollers at 7 and 68, and add a 'prescribed displacement' at the boundaries where you now also apply the load. Then, in the settings for this boundary condition prescribe the displacement in x- and y-direction as 0.
Please login with a confirmed email address before reporting spam
Posted:
1 decade ago
Hi Zahra,
There are several problems here:
1. Your model has three possible rigid body motions: Translation in the plane of the slab, and rotation around the normal. As long as these are not constrained, the model is singular in the numerical sense. In the lab, there is always some friction which keeps it in place. To cure it, you can for example fix one point + add some more constraints.
2. Using a roller condition on boundaries 7 and 68 makes the end essentially clamped, and you will compute a way too large stiffness. A better boundary condition for simulating a roller is to constrain an edge in the vertical direction. This will however give high local stresses, since it is a singular boundary condition.
3. Replacing the load by a prescribed displacement in the center as suggested is not a good idea. If the prescribed displacement is placed on the boundary, there will be a clamping effect, and placing it on a line will give singular stresses (as will a line load).
This seemingly simple test is actually non-trivial to give appropriate boundary conditions. But you should start by making use of the double symmetry, and model only one quarter. In that way you will automatically get rid of all rigid body motions except vertical translation. You can then use distributed self-equilibrating loads both at the center and at the end. You can then just constrain an arbitrary point in the vertical direction to avoid singularity.
Regards,
Henrik
There are several problems here:
1. Your model has three possible rigid body motions: Translation in the plane of the slab, and rotation around the normal. As long as these are not constrained, the model is singular in the numerical sense. In the lab, there is always some friction which keeps it in place. To cure it, you can for example fix one point + add some more constraints.
2. Using a roller condition on boundaries 7 and 68 makes the end essentially clamped, and you will compute a way too large stiffness. A better boundary condition for simulating a roller is to constrain an edge in the vertical direction. This will however give high local stresses, since it is a singular boundary condition.
3. Replacing the load by a prescribed displacement in the center as suggested is not a good idea. If the prescribed displacement is placed on the boundary, there will be a clamping effect, and placing it on a line will give singular stresses (as will a line load).
This seemingly simple test is actually non-trivial to give appropriate boundary conditions. But you should start by making use of the double symmetry, and model only one quarter. In that way you will automatically get rid of all rigid body motions except vertical translation. You can then use distributed self-equilibrating loads both at the center and at the end. You can then just constrain an arbitrary point in the vertical direction to avoid singularity.
Regards,
Henrik