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.
Asymmetric strain with symmetric materials, geometry and load. Where is the problem?
Posted 12.02.2016, 02:14 GMT-5 Geometry, Materials, Modeling Tools & Definitions, Parameters, Variables, & Functions, Structural Mechanics Version 4.4, Version 5.2, Version 5.2a, Version 5.3 5 Replies
Please login with a confirmed email address before reporting spam
I modeled a round diaphragm (a thin disk) in Comsol 4.4 with two different materials: one isotropic and the other anisotropic. For the latter I will need to explore different crystal cuts, therefore I defined a rotated system for the material. The boundary conditions I am applying are:
1. prescribed displacement on the bottom edge (displacement 0 in all directions)
2. a certain pressure on the backside surface
The problems start already with the isotropic material: if the displacement is invariant with respect to an arbitrary in-plane rotation, the strain is not. I need to evaluate the engineering strain (relative increase/decrease of the distances) at the top surface in the normal directions (no shear). I am therefore evaluating the Strain tensor (Material): solid.eXX, solid.eYY. According to Comsol Reference Guide this should be the correct one. Am I right?
What disturbes me is that sqrt(solid.eXX^2+solid.eYY^2) is not invariant with respect to an arbitrary in-plane orientation, even for the isotropic material. So either I am programming something wrong, or I am evaluating the wrong variables, as the strain in the radial direction has to reflect the symmetry of the object if the material and the load are isotropic.
Thank you very much.
1. prescribed displacement on the bottom edge (displacement 0 in all directions)
2. a certain pressure on the backside surface
The problems start already with the isotropic material: if the displacement is invariant with respect to an arbitrary in-plane rotation, the strain is not. I need to evaluate the engineering strain (relative increase/decrease of the distances) at the top surface in the normal directions (no shear). I am therefore evaluating the Strain tensor (Material): solid.eXX, solid.eYY. According to Comsol Reference Guide this should be the correct one. Am I right?
What disturbes me is that sqrt(solid.eXX^2+solid.eYY^2) is not invariant with respect to an arbitrary in-plane orientation, even for the isotropic material. So either I am programming something wrong, or I am evaluating the wrong variables, as the strain in the radial direction has to reflect the symmetry of the object if the material and the load are isotropic.
Thank you very much.
5 Replies Last Post 18.02.2016, 11:03 GMT-5
Please login with a confirmed email address before reporting spam
Posted:
9 years ago
Hi,
Why do you expect sqrt(solid.eXX^2+solid.eYY^2) to be invariant?
sqrt(solid.eXX^2+solid.eYY^2+2*solid.eXY^2) is invariant for an axisymmetric case.
A probably easier way of checking the axial symmetry is to add a local cylindrical coordinate system, and plot for example radial (solid.el11), circumferential (solid.el12). or shear (solid.el12) strains.
Regards,
Henrik
Why do you expect sqrt(solid.eXX^2+solid.eYY^2) to be invariant?
sqrt(solid.eXX^2+solid.eYY^2+2*solid.eXY^2) is invariant for an axisymmetric case.
A probably easier way of checking the axial symmetry is to add a local cylindrical coordinate system, and plot for example radial (solid.el11), circumferential (solid.el12). or shear (solid.el12) strains.
Regards,
Henrik
Please login with a confirmed email address before reporting spam
Posted:
9 years ago
Hello,
sqrt(solid.eXX^2+solid.eYY^2) should represent the radial component of the strain: that's why I expect it to be symmetric. Am I right? What does sqrt(solid.eXX^2+solid.eYY^2+2*solid.eXY^2) represent? And why it is invariant?
I of course tried to use cylindrical coordinates, but that generates the following error message:
"A transformed symmetric tensor is only symmetric if the transform is orthonormal."
All the best,
Andrea
sqrt(solid.eXX^2+solid.eYY^2) should represent the radial component of the strain: that's why I expect it to be symmetric. Am I right? What does sqrt(solid.eXX^2+solid.eYY^2+2*solid.eXY^2) represent? And why it is invariant?
I of course tried to use cylindrical coordinates, but that generates the following error message:
"A transformed symmetric tensor is only symmetric if the transform is orthonormal."
All the best,
Andrea
Please login with a confirmed email address before reporting spam
Posted:
9 years ago
Hi,
If we consider 2D only, then you can use Mohr's circle ( en.wikipedia.org/wiki/Mohr%27s_circle ) to compute the radial strain. As you will see, it contains also the shear strain component eXY. I think your problem is that you try to apply a vector transformation to a 2nd order tensor.
The expression sqrt(solid.eXX^2+solid.eYY^2+2*solid.eXY^2) is not really meaningful, but it is an invariant (again in 2D). It is the RMS of the principal strains. I suggested it because it was similar to your original expression.
As for the error message, something is wrong with the coordinate system used. My best guess is that you should select a material frame in your cylindrical system. In later versions of COMSOL Multiphyics it should not even be possible to select an inappropriate local coordinate system in Linear Elastic since they do not appear in the list.
Regards,
Henrik
If we consider 2D only, then you can use Mohr's circle ( en.wikipedia.org/wiki/Mohr%27s_circle ) to compute the radial strain. As you will see, it contains also the shear strain component eXY. I think your problem is that you try to apply a vector transformation to a 2nd order tensor.
The expression sqrt(solid.eXX^2+solid.eYY^2+2*solid.eXY^2) is not really meaningful, but it is an invariant (again in 2D). It is the RMS of the principal strains. I suggested it because it was similar to your original expression.
As for the error message, something is wrong with the coordinate system used. My best guess is that you should select a material frame in your cylindrical system. In later versions of COMSOL Multiphyics it should not even be possible to select an inappropriate local coordinate system in Linear Elastic since they do not appear in the list.
Regards,
Henrik
Please login with a confirmed email address before reporting spam
Posted:
9 years ago
Helllo.
My goal is not to determine the principal strains directions and magnitudes, so I don't see why Mohr's circles can be useful for me. I actually need simply to evaluate the strain in the radial and tangential directions at the disk surface. For this reason I still don't get where is the mathematical mistake behind my transformation. I know that tensors cannot be transformed with vectorial rules, but I don't want to evaluate the effects of a rotation at this stage (which will be done through the rotated coordinate system), I just want to change the type of coordinates (from cartesian to cylindrical).
Coming to the problem I set under the options for the cylindrical system the frame to be the material one (before it was spatial), but then I cannot choose to apply the rotation in the linear elastic material; and moreover under the available variables to plot the radial and tangential components did not appear.
I wonder if there is somewhere a tutorial on how to use the cylindrical coordinates in 3D models. Of course one natural way to handle this is to go for an axisymmetric model, but later on I want to add other components on the geometry which do not have this symmetry, and check their impact on the axial and tangential strain.
Thank you
Andrea
My goal is not to determine the principal strains directions and magnitudes, so I don't see why Mohr's circles can be useful for me. I actually need simply to evaluate the strain in the radial and tangential directions at the disk surface. For this reason I still don't get where is the mathematical mistake behind my transformation. I know that tensors cannot be transformed with vectorial rules, but I don't want to evaluate the effects of a rotation at this stage (which will be done through the rotated coordinate system), I just want to change the type of coordinates (from cartesian to cylindrical).
Coming to the problem I set under the options for the cylindrical system the frame to be the material one (before it was spatial), but then I cannot choose to apply the rotation in the linear elastic material; and moreover under the available variables to plot the radial and tangential components did not appear.
I wonder if there is somewhere a tutorial on how to use the cylindrical coordinates in 3D models. Of course one natural way to handle this is to go for an axisymmetric model, but later on I want to add other components on the geometry which do not have this symmetry, and check their impact on the axial and tangential strain.
Thank you
Andrea
Please login with a confirmed email address before reporting spam
Posted:
9 years ago
Dear Henrik
I found the problem. Thanks to your advice I put some effort to review some maths about tensors. Actually a very detailed and clear explanation on how to transform tensors can be found at this address:
www.brown.edu/Departments/Engineering/Courses/En221/Notes/Polar_Coords/Polar_Coords.htm
One should not confuse (as I was doing) transformation of points, vectors and tensors, as the second bring in addition to the first the concept of direction (which is a function of the position with polar coordinates, that is the problem) and the latter add one direction more.
By doing some algebra, the transformed tensors in cylindrical polar coordinate are the following:
radial component:
solid.eXX*cos(atan(Y/X))*cos(atan(Y/X))+2*solid.eXY*sin(atan(Y/X))*cos(atan(Y/X))+solid.eYY*sin(atan(Y/X))*sin(atan(Y/X))
tangential component:
solid.eXX*sin(atan(Y/X))*sin(atan(Y/X))-2*solid.eXY*sin(atan(Y/X))*cos(atan(Y/X))+solid.eYY*cos(atan(Y/X))*cos(atan(Y/X))
Shear components can be found easily as well. Out of plane is the same (solid.eZZ)
These are both symmetric as they should, and their physical meaning is perfectly defined without ambiguity. What I needed
Thank you very much for steering me on the right way.
I found the problem. Thanks to your advice I put some effort to review some maths about tensors. Actually a very detailed and clear explanation on how to transform tensors can be found at this address:
www.brown.edu/Departments/Engineering/Courses/En221/Notes/Polar_Coords/Polar_Coords.htm
One should not confuse (as I was doing) transformation of points, vectors and tensors, as the second bring in addition to the first the concept of direction (which is a function of the position with polar coordinates, that is the problem) and the latter add one direction more.
By doing some algebra, the transformed tensors in cylindrical polar coordinate are the following:
radial component:
solid.eXX*cos(atan(Y/X))*cos(atan(Y/X))+2*solid.eXY*sin(atan(Y/X))*cos(atan(Y/X))+solid.eYY*sin(atan(Y/X))*sin(atan(Y/X))
tangential component:
solid.eXX*sin(atan(Y/X))*sin(atan(Y/X))-2*solid.eXY*sin(atan(Y/X))*cos(atan(Y/X))+solid.eYY*cos(atan(Y/X))*cos(atan(Y/X))
Shear components can be found easily as well. Out of plane is the same (solid.eZZ)
These are both symmetric as they should, and their physical meaning is perfectly defined without ambiguity. What I needed
Thank you very much for steering me on the right way.