Discussion ClosedThis 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 3.5]coupled analysis and simmetry conditions
Posted 2009年9月22日 GMT+2 14:566 Replies
Please login with a confirmed email address before reporting spam
Hi
I have built a structural model made of a thin blade (thickness=t=0.14 mm) and a test mass(t = 24 mm).The blade is connected with its lower edge in the middle of the upper surface of the mass. I have modelled the blade with shell module and test mass with solid module; at the end I realized the connection between the two items with identity pairs.
Now I have two problems: the first problem is that I didn't find the eigenfrequencies that i was looking for( the entire geometry is connected with a fixed constraint along the upper edge of the shell), the second problem is that I wasn't able to use symmetry condition.
Now i try to explain better
FIRST PROBLEM
first step: I made a validation of model, correct mass and dimension
I think that the problem is about a coupled field analysis because i realized also the same geometry using only shell (3D mass like shell of 24 mm thickness) and i find the correct frequencies(I can't use this results because this geometry is only a small part of a more complex geometry), but when i made the coupled analysis(solid + shell solver) i find wrong eigenfrequencies (error of about 20Hz or more). I have a doubt on my procedure to put boundary conditions. First i put conditions on shell, so i select in Multiphysics menu shell model, after i go to physics and, in boundary settings, I select the right surface(surface modelled with shell)and i insert its conditions. Now i have one question: when i am in shell module what do i do with the other surfaces(mass surfaces) in boundary settings? are they active in shell domain or not? I select active in this domain(but i put very weak properties, density of 1 and thickness of 0.0001 mm)because if i put them inactive in shell domain i obtain an error during the processing. I put the conditions also in solid modeule and after i launch the analysis, in solver manager i select tll the voices, solid and shell variables.
SECOND PROBLEM
I have always blade and test mass geometry connected with identity pairs, i launch eigenfrequencies analysis of the entire model and I find the frequencies(2.5, 46,67 ). My model has two symmetry plane so slice it and i analyze only a quarter of geometry putting simmetry plane conditions in physics menu. In this way i thought to obtain the same wrong frequencies but the analysis return to me frequencies of about 1300 hz and beyond. I have two symmetry plane so i put symmetry conditions on one edge and the surface of the shell, and after i put symmetry conditions also on two surface of the solid.I slice along two surfaces, so i divide also the line that reproduces the connection between blade and solid, my question is: could i put some symmetry condition also for identity pairs?
I hope that my explanation is quite fair to obtain an answer.
thank you
Luca
I have built a structural model made of a thin blade (thickness=t=0.14 mm) and a test mass(t = 24 mm).The blade is connected with its lower edge in the middle of the upper surface of the mass. I have modelled the blade with shell module and test mass with solid module; at the end I realized the connection between the two items with identity pairs.
Now I have two problems: the first problem is that I didn't find the eigenfrequencies that i was looking for( the entire geometry is connected with a fixed constraint along the upper edge of the shell), the second problem is that I wasn't able to use symmetry condition.
Now i try to explain better
FIRST PROBLEM
first step: I made a validation of model, correct mass and dimension
I think that the problem is about a coupled field analysis because i realized also the same geometry using only shell (3D mass like shell of 24 mm thickness) and i find the correct frequencies(I can't use this results because this geometry is only a small part of a more complex geometry), but when i made the coupled analysis(solid + shell solver) i find wrong eigenfrequencies (error of about 20Hz or more). I have a doubt on my procedure to put boundary conditions. First i put conditions on shell, so i select in Multiphysics menu shell model, after i go to physics and, in boundary settings, I select the right surface(surface modelled with shell)and i insert its conditions. Now i have one question: when i am in shell module what do i do with the other surfaces(mass surfaces) in boundary settings? are they active in shell domain or not? I select active in this domain(but i put very weak properties, density of 1 and thickness of 0.0001 mm)because if i put them inactive in shell domain i obtain an error during the processing. I put the conditions also in solid modeule and after i launch the analysis, in solver manager i select tll the voices, solid and shell variables.
SECOND PROBLEM
I have always blade and test mass geometry connected with identity pairs, i launch eigenfrequencies analysis of the entire model and I find the frequencies(2.5, 46,67 ). My model has two symmetry plane so slice it and i analyze only a quarter of geometry putting simmetry plane conditions in physics menu. In this way i thought to obtain the same wrong frequencies but the analysis return to me frequencies of about 1300 hz and beyond. I have two symmetry plane so i put symmetry conditions on one edge and the surface of the shell, and after i put symmetry conditions also on two surface of the solid.I slice along two surfaces, so i divide also the line that reproduces the connection between blade and solid, my question is: could i put some symmetry condition also for identity pairs?
I hope that my explanation is quite fair to obtain an answer.
thank you
Luca
6 Replies
Last Post 2009年10月1日 GMT+2 11:17
Please login with a confirmed email address before reporting spam
Posted:
1 decade ago
Dear Luca,
I think that there is no need to employ indenty pairs to link the two appl. modes (shell and solid stress strain).
Draw you 3d geometry and than assign the Solid-Stress strain appl. mode to the subdomains. Then insert the Shell appl. mode using the same variable names as for the smsld case (that is: when you add such an application mode through the model navigator set in the dependent variable name field the same variables of the smsld appl. mode, that is u v w).
Then activate the shell module just on the boundary (i.e. surface) where you want it. Deactivate it on the other boundaries.
Use an unstructured mesh (tetrahedrals) for the 3d object since shell appl. mode does not allow a structured one.
I hope this help.
Alessandro
I think that there is no need to employ indenty pairs to link the two appl. modes (shell and solid stress strain).
Draw you 3d geometry and than assign the Solid-Stress strain appl. mode to the subdomains. Then insert the Shell appl. mode using the same variable names as for the smsld case (that is: when you add such an application mode through the model navigator set in the dependent variable name field the same variables of the smsld appl. mode, that is u v w).
Then activate the shell module just on the boundary (i.e. surface) where you want it. Deactivate it on the other boundaries.
Use an unstructured mesh (tetrahedrals) for the 3d object since shell appl. mode does not allow a structured one.
I hope this help.
Alessandro
Please login with a confirmed email address before reporting spam
Posted:
1 decade ago
Hi
First thanks for using the proposded application mode summary in the subject line.
Now I want to add, in addition to A. Ricci's comment, that when you have one symmetries BC in your model, and you want to get te eigenmodes, do not forget that at you have mostly 2 different modes set (calculated with symmetry and anti-symmetry BC's), further with 2 symmetry boundaries, you have mostly 4 sets, for the 4 different combinations of boundaries. It's often easy to forget some modes.
Good luck
Ivar
First thanks for using the proposded application mode summary in the subject line.
Now I want to add, in addition to A. Ricci's comment, that when you have one symmetries BC in your model, and you want to get te eigenmodes, do not forget that at you have mostly 2 different modes set (calculated with symmetry and anti-symmetry BC's), further with 2 symmetry boundaries, you have mostly 4 sets, for the 4 different combinations of boundaries. It's often easy to forget some modes.
Good luck
Ivar
Please login with a confirmed email address before reporting spam
Posted:
1 decade ago
Hello Alessandro
I have read your advices and i have tried to apply them, but i am new in the usage of comsol, and i suppose that i am also slow to understand, so forgive me if i have other questions about the problem.
I realize my geometry with comsol CAD, in particular I draw surface geometries of blade and test mass in 2D work plane, after that, I extrude test mass surface for 24 mm in 3D space, but for the blade i don't make the extrusion because i should make an extrusion of 0.14 mm and this very thin thickness creates problems of out of memory during analysis, because the mesh become too fine.
So I embed the surface.
At the end I find two split entities in 3D space, a block(test mass) and a surface(blade); i must create a phisical connection between them but i can't make coerce to solid because with this command the blade(surface) disappears because it is only a surface, I use identity pairs to connect physically these two entities.
Now I introduce the shell module, and i control that dependent variables have the same name of solid variables (in model navigator i have read u v w p for smsld and u v w thx thy thz smsh, so i suppose that i must change nothing).
Subsequently i put my constraints on blade edge and i launch my analysis but i find wrong results. If i put only the blade(i.e. embed surface) active on shell domain and i deactivate the test mass boundaries in shell domain I find other wrong results with the only deformation of blade, so to obtain a continuity solution between mass and blade i must model also mass boundaries with shell. I don't find where is my fault.
Thank you
Luca
I have read your advices and i have tried to apply them, but i am new in the usage of comsol, and i suppose that i am also slow to understand, so forgive me if i have other questions about the problem.
I realize my geometry with comsol CAD, in particular I draw surface geometries of blade and test mass in 2D work plane, after that, I extrude test mass surface for 24 mm in 3D space, but for the blade i don't make the extrusion because i should make an extrusion of 0.14 mm and this very thin thickness creates problems of out of memory during analysis, because the mesh become too fine.
So I embed the surface.
At the end I find two split entities in 3D space, a block(test mass) and a surface(blade); i must create a phisical connection between them but i can't make coerce to solid because with this command the blade(surface) disappears because it is only a surface, I use identity pairs to connect physically these two entities.
Now I introduce the shell module, and i control that dependent variables have the same name of solid variables (in model navigator i have read u v w p for smsld and u v w thx thy thz smsh, so i suppose that i must change nothing).
Subsequently i put my constraints on blade edge and i launch my analysis but i find wrong results. If i put only the blade(i.e. embed surface) active on shell domain and i deactivate the test mass boundaries in shell domain I find other wrong results with the only deformation of blade, so to obtain a continuity solution between mass and blade i must model also mass boundaries with shell. I don't find where is my fault.
Thank you
Luca
Please login with a confirmed email address before reporting spam
Posted:
1 decade ago
Hi Luca
If you are starting with COMSOL, I would advise you to try to stay, at the beginning, with one applicaiton mode, because if you mix shell and solids you also have to "sew" the degrees of freedom (DoF) together correctly, and you have to define a set og global variables to look at the results for the full system. This becomes quickly rather complex in COMSOL
I would be happy to hear the contrary, if someone out there has a "simple" method to propose, pls, come with it.
Basically the edges of a 3D shell (in a similar way any 3D euler beam) have 6 DoF's (u,v,w) as for a solid, but also (thx,thy,thz) which are not defined in the solids (they could have been, but are not currently in Comsol), you have to equate these rotations to the surface normal of the boundary linking the shell edge and the solid, otherwise you have a "free hinge" there along the common edge.
One can also have the shell surface overlap the 3D volume, this would force the rotation DOF to be coherent on the shell-volume boundary, but then you add stiffness and mass to your volume, as you have a shell element and the volume element overlapping.
If your problem is rather 2D like, I would suggest to start fully in shell mode, you draw your surfaces in a geometry and embedded them into a new 3D geometry where you define the shells, you can change the thicknesses for each surface. This assumes though that the neutral fiber is in the 2D plane and your volume extrude symetrically around this central surface.
The meshing is simpler and you will quicker get your results
Good luck
Ivar
If you are starting with COMSOL, I would advise you to try to stay, at the beginning, with one applicaiton mode, because if you mix shell and solids you also have to "sew" the degrees of freedom (DoF) together correctly, and you have to define a set og global variables to look at the results for the full system. This becomes quickly rather complex in COMSOL
I would be happy to hear the contrary, if someone out there has a "simple" method to propose, pls, come with it.
Basically the edges of a 3D shell (in a similar way any 3D euler beam) have 6 DoF's (u,v,w) as for a solid, but also (thx,thy,thz) which are not defined in the solids (they could have been, but are not currently in Comsol), you have to equate these rotations to the surface normal of the boundary linking the shell edge and the solid, otherwise you have a "free hinge" there along the common edge.
One can also have the shell surface overlap the 3D volume, this would force the rotation DOF to be coherent on the shell-volume boundary, but then you add stiffness and mass to your volume, as you have a shell element and the volume element overlapping.
If your problem is rather 2D like, I would suggest to start fully in shell mode, you draw your surfaces in a geometry and embedded them into a new 3D geometry where you define the shells, you can change the thicknesses for each surface. This assumes though that the neutral fiber is in the 2D plane and your volume extrude symetrically around this central surface.
The meshing is simpler and you will quicker get your results
Good luck
Ivar
Please login with a confirmed email address before reporting spam
Posted:
1 decade ago
Hi again,
here is an example of Shell to Solid DoF sewing, but it works only if:
1) coordinate systems are well aligned with sewing edge, if not you must redefine local coordinate and adapt the formulas
2) the edge surface shared with the 2D shell and the 3D volume is "in the middle" of a single 3D surface/ boundary, if not I'm not sure my formua for the rotations holds, as an edge sheared between two non-coplanar surfaces.
geom1 is the 2D initial geometry
geom2 is the shell - solid geometry
geom3 is a full solid model
2-3 are loaded by gravity along Fz
Note: if you run a eigenfrequency run on these you will mix your 2D and 3D frequencies, pls sort them accordingly, as everything is in one file
Good luck
Ivar
here is an example of Shell to Solid DoF sewing, but it works only if:
1) coordinate systems are well aligned with sewing edge, if not you must redefine local coordinate and adapt the formulas
2) the edge surface shared with the 2D shell and the 3D volume is "in the middle" of a single 3D surface/ boundary, if not I'm not sure my formua for the rotations holds, as an edge sheared between two non-coplanar surfaces.
geom1 is the 2D initial geometry
geom2 is the shell - solid geometry
geom3 is a full solid model
2-3 are loaded by gravity along Fz
Note: if you run a eigenfrequency run on these you will mix your 2D and 3D frequencies, pls sort them accordingly, as everything is in one file
Good luck
Ivar
Attachments:
Please login with a confirmed email address before reporting spam
Posted:
1 decade ago
Hi Ivar
I write this message with delay, but I want to tell you thank you for your help, you solved my structural problems.
Bye
Luca
I write this message with delay, but I want to tell you thank you for your help, you solved my structural problems.
Bye
Luca