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 The information provided may be out of date.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.
Problems with structural mechanics model
Posted Mar 1, 2011, 3:42 p.m. EST Structural Mechanics Version 3.5a 9 Replies
Please login with a confirmed email address before reporting spam
Hi,
Unlike most users, I am not an engineer, I am a geophysicist and want to study stresses resulting from an earthquake!
I am trying to simulate a model related to slip between two subdomains. My model needs to involve 2 steps and I will describe it in some details without being too overwhelming.
My model is related to a geologic setting where 2 Earth "subdomians" (ocean crust and continental crust with different material properties such as Young's modulus and density) are in contact and the ocean crust slips against the continental crust; that makes it a structural mechanics problem with contact pairs. The model is 3 subdomians: the bottom subdomain is the earth mantle the middle is the ocean crust and the top is the continental crust. The boundary between the ocean and the mantle is identity pair because they should move together.
First, I need to simulate the pre-existing load/stress of the earth. To do this I applied the gravity and density as subdomain conditions and I used the parametric solver to apply this load gradually. I also introduced "springs" between the different subdomains and boundaries to hold the geometry together. This approach has been recommended to me by a previous COMSOL user who simulated a similar problem and this is known to be the appropriate approach (this has been the proposed solution to that user by comsol support representatives.).
The second step, is to apply displacement (3m) to the ocean crust and I want to study the stresses resulting from that slip. This slip is used to simulate slip resulting from an earthquake. This will be done using the "restart solver" option after running the first step (mentioned above).
My problems are several and I hope you can give me some insight. These problems are:
1) I get edge effects and even with refined meshes they don't go away. In some instances refining the mesh causes the model to fail.
2) Given that the boundary between the ocean and the continent is defined as a contact pair, can I apply a prescribed displacement on one side of this contact pair?
3) If I apply a load to a subdomain can I also apply prescribed displacement to that same subdomain? I am confused about that given what I have read in the manual.
4) I would like some insight on whether my contact pressure, contact penalty and manual scaling factors are appropriate and if not, why?
5) I use the parametric solver and when solving, the progress page shows a "finished" message but reaches 99% not 100%
I attached the model. Please feel free to suggest/make changes as necessary. I am a new user and FEM is not my field of expertise as I am a student in Earth Sciences. I really appreciate your time and help!
Thank you,
Maya
Unlike most users, I am not an engineer, I am a geophysicist and want to study stresses resulting from an earthquake!
I am trying to simulate a model related to slip between two subdomains. My model needs to involve 2 steps and I will describe it in some details without being too overwhelming.
My model is related to a geologic setting where 2 Earth "subdomians" (ocean crust and continental crust with different material properties such as Young's modulus and density) are in contact and the ocean crust slips against the continental crust; that makes it a structural mechanics problem with contact pairs. The model is 3 subdomians: the bottom subdomain is the earth mantle the middle is the ocean crust and the top is the continental crust. The boundary between the ocean and the mantle is identity pair because they should move together.
First, I need to simulate the pre-existing load/stress of the earth. To do this I applied the gravity and density as subdomain conditions and I used the parametric solver to apply this load gradually. I also introduced "springs" between the different subdomains and boundaries to hold the geometry together. This approach has been recommended to me by a previous COMSOL user who simulated a similar problem and this is known to be the appropriate approach (this has been the proposed solution to that user by comsol support representatives.).
The second step, is to apply displacement (3m) to the ocean crust and I want to study the stresses resulting from that slip. This slip is used to simulate slip resulting from an earthquake. This will be done using the "restart solver" option after running the first step (mentioned above).
My problems are several and I hope you can give me some insight. These problems are:
1) I get edge effects and even with refined meshes they don't go away. In some instances refining the mesh causes the model to fail.
2) Given that the boundary between the ocean and the continent is defined as a contact pair, can I apply a prescribed displacement on one side of this contact pair?
3) If I apply a load to a subdomain can I also apply prescribed displacement to that same subdomain? I am confused about that given what I have read in the manual.
4) I would like some insight on whether my contact pressure, contact penalty and manual scaling factors are appropriate and if not, why?
5) I use the parametric solver and when solving, the progress page shows a "finished" message but reaches 99% not 100%
I attached the model. Please feel free to suggest/make changes as necessary. I am a new user and FEM is not my field of expertise as I am a student in Earth Sciences. I really appreciate your time and help!
Thank you,
Maya
Attachments:
9 Replies Last Post Mar 18, 2011, 7:16 p.m. EDT
Please login with a confirmed email address before reporting spam
Posted:
1 decade ago
Hi
I do not have access to my COMSOL tool just now, so I cannot open your model (anyhow if I need the earth Science module I do not have that one). But I can give you a few thoughts.
a) the way to stress a structure, as you describe it, is very close to what I do regularly for my "standard" structural models, so I would also think that is the best approach
1) Edge effects, what do they come from? If it's because you load your model with "point" loads, then you cannot avoid them. You need to apply loads onto boundaries or at least edges of a finite length/area such to everage the pressure over several mesh elements, If not, it's by design a singularity, and refining the mesh will not solve it, as you say it might, or even will, make it worse !
2) I would believe so, but normally we prescriebe a displacement about perpendicular to the contact normal, I suppose you are more in "shear" mode, and you probably also have some friction in there then I'm no longer sure what is really allowed. You should try it out on a simple model you can estimate analytically. In 3.5 there is a friction contact sliding mass example somewhere, hat could probably give you some clues.
3) I would say no here, if you apply a prescribed displacement you apply in some way the force required to get the motion (not fully) so ading some load is in my view an overstressing case (and might give you some solver or model discretisation issues) One exception if the loadand the displacement are ar rightn angle, then their combination could make sens, to be checked carefully though
4) very pertinent remark, but I'm no longer sure how we ask COMSOL to dump it's scaling factors in v3.5 (in v4 you can ask for a more detailed log and then sometimes, you get also the effective scaling factor used ;)
5) indeed it's better to reach 100% ;) cannot say much more there
--
Good luck
Ivar
I do not have access to my COMSOL tool just now, so I cannot open your model (anyhow if I need the earth Science module I do not have that one). But I can give you a few thoughts.
a) the way to stress a structure, as you describe it, is very close to what I do regularly for my "standard" structural models, so I would also think that is the best approach
1) Edge effects, what do they come from? If it's because you load your model with "point" loads, then you cannot avoid them. You need to apply loads onto boundaries or at least edges of a finite length/area such to everage the pressure over several mesh elements, If not, it's by design a singularity, and refining the mesh will not solve it, as you say it might, or even will, make it worse !
2) I would believe so, but normally we prescriebe a displacement about perpendicular to the contact normal, I suppose you are more in "shear" mode, and you probably also have some friction in there then I'm no longer sure what is really allowed. You should try it out on a simple model you can estimate analytically. In 3.5 there is a friction contact sliding mass example somewhere, hat could probably give you some clues.
3) I would say no here, if you apply a prescribed displacement you apply in some way the force required to get the motion (not fully) so ading some load is in my view an overstressing case (and might give you some solver or model discretisation issues) One exception if the loadand the displacement are ar rightn angle, then their combination could make sens, to be checked carefully though
4) very pertinent remark, but I'm no longer sure how we ask COMSOL to dump it's scaling factors in v3.5 (in v4 you can ask for a more detailed log and then sometimes, you get also the effective scaling factor used ;)
5) indeed it's better to reach 100% ;) cannot say much more there
--
Good luck
Ivar
Please login with a confirmed email address before reporting spam
Posted:
1 decade ago
Thanks Ivar for your very prompt and helpful response, I need some more clarification please
I am actually using structural mechanics module.
1) I am applying the load as boundary. Is there a way to remove this or I just need to take it as is? I think the edge effect is masking my actual stress values.
2) May you please provide more explanation on this point?
3) The forces in the subdomain are due to gravity but I also need to the whole subdomian to slip so I was thinking of applying slip as a subdomain condition. But if this is incorrect, then how else can I make it move if I can't prescribe displacement on the contact pair.
I am still struggling with points 4 and 5, will deal with that later.
Thanks a lot
Maya
PS I can wait till you get access to COMSOL and have a look at my model...I am seriously struggling :(
I am actually using structural mechanics module.
1) I am applying the load as boundary. Is there a way to remove this or I just need to take it as is? I think the edge effect is masking my actual stress values.
2) May you please provide more explanation on this point?
3) The forces in the subdomain are due to gravity but I also need to the whole subdomian to slip so I was thinking of applying slip as a subdomain condition. But if this is incorrect, then how else can I make it move if I can't prescribe displacement on the contact pair.
I am still struggling with points 4 and 5, will deal with that later.
Thanks a lot
Maya
PS I can wait till you get access to COMSOL and have a look at my model...I am seriously struggling :(
Please login with a confirmed email address before reporting spam
Posted:
1 decade ago
Hi
I had a quick look this morning, nice model :)
To avoid the units red tag, you should multiply the body loads by the "thickness_smpn" which is 1[m] by default so its only a unit corrector. Or you chec the Body load is defined as force per area and COMSOL looks after the thickness for you, but then you need to correct the G*denisty taking into account the thickness
Your body load multiplicand is also 1E8[N/m^3] a force density. Using systematically consistent units helps to check the formulas
For your prescribed displacements, I would not block the items along X. To the left on boundaries 1 and 7 I would use symmetry (almost the same) and to the right I would add a "spring" or a pressure to allow the material to "flow" to the right. For me a Rx=0 is too restrictive on your right side
Then if you define two internal boundaries as identity pairs that means you have continuity, then you should not also add loads there, that hurts my understanding.
I would rather load the external surfaces/boundaries with pressures, and leave the internal boundaries float around to settle themselves
--
Good luck
Ivar
I had a quick look this morning, nice model :)
To avoid the units red tag, you should multiply the body loads by the "thickness_smpn" which is 1[m] by default so its only a unit corrector. Or you chec the Body load is defined as force per area and COMSOL looks after the thickness for you, but then you need to correct the G*denisty taking into account the thickness
Your body load multiplicand is also 1E8[N/m^3] a force density. Using systematically consistent units helps to check the formulas
For your prescribed displacements, I would not block the items along X. To the left on boundaries 1 and 7 I would use symmetry (almost the same) and to the right I would add a "spring" or a pressure to allow the material to "flow" to the right. For me a Rx=0 is too restrictive on your right side
Then if you define two internal boundaries as identity pairs that means you have continuity, then you should not also add loads there, that hurts my understanding.
I would rather load the external surfaces/boundaries with pressures, and leave the internal boundaries float around to settle themselves
--
Good luck
Ivar
Please login with a confirmed email address before reporting spam
Posted:
1 decade ago
Hello Ivar,
Thank you very much for your time and suggestions. I'm glad you liked my model :)
Regarding the red unit tags, I followed your suggestions but I didn't get rid of the red tags. For the subdomains, I am applying the load as (force/volume using thickness) and for the boundaries I am applying the load as (force/area using thickness). I defined the spring stiffness (-1e8) to have units of [N/m] and that did not solve the unit problem. I also tried multiplying the spring stiffness with "thickness_smpn" and still got the red tag. I think the problem is coming from the fact that I am using the variable "u" and "v". For e.g. the body load in Fy is defined as (gravity*density)*(-1e8*v)*(1-para) and in Fx is (-1e8*v)*(1-para). No matter what I do I still get the unit red tag UNLESS I remove the variable "u" or "v". Is there a way to overcome this problem.
For your prescribed displacements, thank you for this suggestion of using symmetry. I applied symmetry to the boundaries 1 and 7. I found that the problem of the edge effect is coming from the fact that the continental subdomain (top most subdomain) wants to move in the x-direction but since I was restricting it to be Rx=0 it resulted in the edge effect. I think that the idea of adding a spring to let it flow to the right is appropriate, but when I tried doing that, I got the edge effect again; so the problem is still not solved. How else might I get rid of this.
In this step, I should not be seeing relative displacement. I don't think that the subdomains should move in the x-direction because I am not applying loads in the x-direction. Its OK to move in the y-direction due to gravity*density; but why do I get displacement in the x-direction? Is it an effect of the springs on the boundary or is it an effect of the springs on the subdomians? Should I increase or decrease the springs?
I removed the boundary loads from the identity pairs and now these boundaries have 0 loads, but I kept the loads on the contact pairs; did I understand your suggestions correctly?
Thank you Ivar! I really appreciate your time and help
Maya
Thank you very much for your time and suggestions. I'm glad you liked my model :)
Regarding the red unit tags, I followed your suggestions but I didn't get rid of the red tags. For the subdomains, I am applying the load as (force/volume using thickness) and for the boundaries I am applying the load as (force/area using thickness). I defined the spring stiffness (-1e8) to have units of [N/m] and that did not solve the unit problem. I also tried multiplying the spring stiffness with "thickness_smpn" and still got the red tag. I think the problem is coming from the fact that I am using the variable "u" and "v". For e.g. the body load in Fy is defined as (gravity*density)*(-1e8*v)*(1-para) and in Fx is (-1e8*v)*(1-para). No matter what I do I still get the unit red tag UNLESS I remove the variable "u" or "v". Is there a way to overcome this problem.
For your prescribed displacements, thank you for this suggestion of using symmetry. I applied symmetry to the boundaries 1 and 7. I found that the problem of the edge effect is coming from the fact that the continental subdomain (top most subdomain) wants to move in the x-direction but since I was restricting it to be Rx=0 it resulted in the edge effect. I think that the idea of adding a spring to let it flow to the right is appropriate, but when I tried doing that, I got the edge effect again; so the problem is still not solved. How else might I get rid of this.
In this step, I should not be seeing relative displacement. I don't think that the subdomains should move in the x-direction because I am not applying loads in the x-direction. Its OK to move in the y-direction due to gravity*density; but why do I get displacement in the x-direction? Is it an effect of the springs on the boundary or is it an effect of the springs on the subdomians? Should I increase or decrease the springs?
I removed the boundary loads from the identity pairs and now these boundaries have 0 loads, but I kept the loads on the contact pairs; did I understand your suggestions correctly?
Thank you Ivar! I really appreciate your time and help
Maya
Please login with a confirmed email address before reporting spam
Posted:
1 decade ago
HI
sorry I believe thats my fault isnt it divide by thickness_smnp ? well it depends as part of your formula g*rho is in N/m^3 and part is in N/m^2 and you want either N/m^2 or N/m^3 dependin on what you select (Alwaysstudy the units carefully and write out the equations in case of a doubt, or even take a look at the COMSOL equations: Physics Equation settings ... Variables ...)
By the way the color should be orange for units issues and red for typos, missing ( or ) or *+-/ etc (or is that v4?, probably I'm getting lost 3.5 is oldish for me;)
Then, yes, you should get some motion in the X direction if you compress along Y, because you have the Poisson coefficient coupling the two directions (valid for solids)
why not add a boundary load along X on the right side boundaries of the type -K*u where K is the stiffness, again careful with the units the spring constant is in [N/m] but it is to be applied on each element touching the boundary so its again in [N/m^3] as its a "spring density" or "per area" constant we need, so if you know the [N/m] value then divide it further by the "boundary height*thickness_smnp"
You might want to add the load on the external top boundary, and what does the load on the contact pair mean ?
A contact pair are 2 boundaries, in which direction do they go ?
check your arrows of the boundaries, the normal is (if Iremember right) to the left if the arrow is pointing up, anti clock wise.
--
Good luck
Ivar
sorry I believe thats my fault isnt it divide by thickness_smnp ? well it depends as part of your formula g*rho is in N/m^3 and part is in N/m^2 and you want either N/m^2 or N/m^3 dependin on what you select (Alwaysstudy the units carefully and write out the equations in case of a doubt, or even take a look at the COMSOL equations: Physics Equation settings ... Variables ...)
By the way the color should be orange for units issues and red for typos, missing ( or ) or *+-/ etc (or is that v4?, probably I'm getting lost 3.5 is oldish for me;)
Then, yes, you should get some motion in the X direction if you compress along Y, because you have the Poisson coefficient coupling the two directions (valid for solids)
why not add a boundary load along X on the right side boundaries of the type -K*u where K is the stiffness, again careful with the units the spring constant is in [N/m] but it is to be applied on each element touching the boundary so its again in [N/m^3] as its a "spring density" or "per area" constant we need, so if you know the [N/m] value then divide it further by the "boundary height*thickness_smnp"
You might want to add the load on the external top boundary, and what does the load on the contact pair mean ?
A contact pair are 2 boundaries, in which direction do they go ?
check your arrows of the boundaries, the normal is (if Iremember right) to the left if the arrow is pointing up, anti clock wise.
--
Good luck
Ivar
Please login with a confirmed email address before reporting spam
Posted:
1 decade ago
Hi Ivar,
Thanks for your response.
- Following your suggestions, I have been able to get rid of the red unit tags; thank you!
- I have been trying many different ways to find a way to get rid of the singularities. One of these trials was to modify the geometry (new geometry attached).
I am still having trouble with the singularity though. In the new geometry (attached) i am getting gaps between between two contact pairs. That is, one side of the contact pair seems to be loosing contact with the other side of the contact boundary. I tried increasing and decreasing the contact pressure (Tn) and also the springs stiffness. But the result is either there no change or that the it fails.
Also, in the previous model (posted last week), I also tried following your suggestions and applying a spring to the right side of the model; still I got no improvements.
The problem is that the continent subdomain wants to move, if I leave it free the model fails. And if I constrain it (symmetry or anything else) the result is this singularity or that it also fails. I have exhausted all trials that I can think of. Please help me out with this. I don't know what to do or how to solve this problem.
Thank you
Maya
Thanks for your response.
- Following your suggestions, I have been able to get rid of the red unit tags; thank you!
- I have been trying many different ways to find a way to get rid of the singularities. One of these trials was to modify the geometry (new geometry attached).
I am still having trouble with the singularity though. In the new geometry (attached) i am getting gaps between between two contact pairs. That is, one side of the contact pair seems to be loosing contact with the other side of the contact boundary. I tried increasing and decreasing the contact pressure (Tn) and also the springs stiffness. But the result is either there no change or that the it fails.
Also, in the previous model (posted last week), I also tried following your suggestions and applying a spring to the right side of the model; still I got no improvements.
The problem is that the continent subdomain wants to move, if I leave it free the model fails. And if I constrain it (symmetry or anything else) the result is this singularity or that it also fails. I have exhausted all trials that I can think of. Please help me out with this. I don't know what to do or how to solve this problem.
Thank you
Maya
Attachments:
Please login with a confirmed email address before reporting spam
Posted:
1 decade ago
Anybody with suggestions or help please?
Maya
Maya
Please login with a confirmed email address before reporting spam
Posted:
1 decade ago
Hi
I had a new look, I believe its your right side symmetric conditions that is playing you a game, that means it cannot move, I tried an antisymmetric conditions but it's not much better. But have you tried a simple spring or pressure load, to allow your material to flow towards the right (with the symmetry you block the flow on the right side) Or just leave it free.
Anyhow, if you zoom in on the "hot spot" you notice that the edge is restricted in "y", but I haven't found out why so far, In fact yes, its the pressure force from beneath, I believe your spring constant is too tough, if you remove it on edge 23 (and free the right edge) you will see the flow, you could try 3 different spring forces here, better adapted to the lower "softer (?) layer". You should perhaps add the semi-fluid lower core layer ?
--
Good luck
Ivar
I had a new look, I believe its your right side symmetric conditions that is playing you a game, that means it cannot move, I tried an antisymmetric conditions but it's not much better. But have you tried a simple spring or pressure load, to allow your material to flow towards the right (with the symmetry you block the flow on the right side) Or just leave it free.
Anyhow, if you zoom in on the "hot spot" you notice that the edge is restricted in "y", but I haven't found out why so far, In fact yes, its the pressure force from beneath, I believe your spring constant is too tough, if you remove it on edge 23 (and free the right edge) you will see the flow, you could try 3 different spring forces here, better adapted to the lower "softer (?) layer". You should perhaps add the semi-fluid lower core layer ?
--
Good luck
Ivar
Please login with a confirmed email address before reporting spam
Posted:
1 decade ago
Hi Ivar,
Thank you very much for your help. Your suggestion was very helpful and made a significant improvement. Specifically, the problem was solved when I applied springs to the right and left boundaries rather than applying one of the roller or prescribed or fixed constraints on the boundaries. Also, an error on my behalf that was causing the enormous stress concentration and the boundaries to loose contact was that I was applying the spring on the bottom boundary as a force/volume rather than force/area. I am posting this just in case other users run into a same/similar problem.
Maya
Thank you very much for your help. Your suggestion was very helpful and made a significant improvement. Specifically, the problem was solved when I applied springs to the right and left boundaries rather than applying one of the roller or prescribed or fixed constraints on the boundaries. Also, an error on my behalf that was causing the enormous stress concentration and the boundaries to loose contact was that I was applying the spring on the bottom boundary as a force/volume rather than force/area. I am posting this just in case other users run into a same/similar problem.
Maya