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 The information provided may be out of date.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.
How do I simulate the stress distribution that result in shrink fit of a compond cylinder.
Posted 05.09.2012, 02:42 GMT-4 Structural Mechanics Version 4.3 12 Replies
Please login with a confirmed email address before reporting spam
Hi,
I model a compound cylinder, the inner cylinder has initial values before the shrink fit; inner radius, ri and outer radius (rc + delta) where delta is the interface displacement due to shrink fit. The outer cylinder has inner radius, rc and outer radius, ro.
I tried to simulate the problem using prescribed displacement using an initial value of delta on the compound cylinder boundary interface(where I place the value of u0=delta*cos(theta) and v0=delta*sin(theta) and the outer cylinder boundary. The result I obtained does not correspond with what I got from the analytic computation of the problem when I assume a value for delta.
Please, does anyone know the right approach that I can use to simulate the stresses in compound cylinder that can results from delta and the different material properties of the shrink fitted cylinders and diameters of the inner and outer cylinders when the value delta is unknown and is also dependent on the different materials of the compound cylinders.
I have attached my model. Any suggestion is greatly appreciated. Thanks
Daniel.
.
I model a compound cylinder, the inner cylinder has initial values before the shrink fit; inner radius, ri and outer radius (rc + delta) where delta is the interface displacement due to shrink fit. The outer cylinder has inner radius, rc and outer radius, ro.
I tried to simulate the problem using prescribed displacement using an initial value of delta on the compound cylinder boundary interface(where I place the value of u0=delta*cos(theta) and v0=delta*sin(theta) and the outer cylinder boundary. The result I obtained does not correspond with what I got from the analytic computation of the problem when I assume a value for delta.
Please, does anyone know the right approach that I can use to simulate the stresses in compound cylinder that can results from delta and the different material properties of the shrink fitted cylinders and diameters of the inner and outer cylinders when the value delta is unknown and is also dependent on the different materials of the compound cylinders.
I have attached my model. Any suggestion is greatly appreciated. Thanks
Daniel.
.
Attachments:
12 Replies Last Post 11.12.2014, 23:31 GMT-5
Please login with a confirmed email address before reporting spam
Posted:
1 decade ago
Hi Daniel,
In your model you have an inner cylinder of radii ri and rc, and an outer cylinder of radii rc and ro. You then apply delta displacement to the joint interface. That is not the same as an interference/shrink fit.
One way to model the interference fit is to give the inner cylinder an outer radius of rc + delta so that there is a geometric overlap. Then do a geometry Assembly instead of Union to keep the two cylinders separate and define contact between the two mating surfaces. The contact constraint will move both surfaces apart until it eliminates the delta overlap. You can instead of contact use a Boundary Similarity mapping (under Definitions, Model Coupling) between the two mating surfaces and prescribe the radial displacement on the inner surface of the outer cylinder to be equal to “delta + bndsim1(radial displacement of outer surface of inner cylinder)”, where bndsim1 is the name of the boundary similarity operator. There may be another simpler way in COMSOL, but I can’t think of one now.
Nagi Elabbasi
Veryst Engineering
In your model you have an inner cylinder of radii ri and rc, and an outer cylinder of radii rc and ro. You then apply delta displacement to the joint interface. That is not the same as an interference/shrink fit.
One way to model the interference fit is to give the inner cylinder an outer radius of rc + delta so that there is a geometric overlap. Then do a geometry Assembly instead of Union to keep the two cylinders separate and define contact between the two mating surfaces. The contact constraint will move both surfaces apart until it eliminates the delta overlap. You can instead of contact use a Boundary Similarity mapping (under Definitions, Model Coupling) between the two mating surfaces and prescribe the radial displacement on the inner surface of the outer cylinder to be equal to “delta + bndsim1(radial displacement of outer surface of inner cylinder)”, where bndsim1 is the name of the boundary similarity operator. There may be another simpler way in COMSOL, but I can’t think of one now.
Nagi Elabbasi
Veryst Engineering
Please login with a confirmed email address before reporting spam
Posted:
1 decade ago
Hi Nagi,
Thanks for the quick reply. I tried using the geometry assembly and creating a contact pair. but I got zero stress result from my simulation. I also tried using the second method you suggested but the result simulated was still far from alright. Please, check the two attached model if there is something am not doing right or any other idea on how to proceed is appreciated. Thanks.
Daniel.
Thanks for the quick reply. I tried using the geometry assembly and creating a contact pair. but I got zero stress result from my simulation. I also tried using the second method you suggested but the result simulated was still far from alright. Please, check the two attached model if there is something am not doing right or any other idea on how to proceed is appreciated. Thanks.
Daniel.
Attachments:
Please login with a confirmed email address before reporting spam
Posted:
1 decade ago
Hi,
I have a bit similar simulation but it doesn't have an inner hole. I applied uniform pressure on the boundaries and introduce similar initial pressure on the contact surfaces. Assembly method was applied. When I applied union method without introducing contact surfaces it almost gave me the similar result. In bothe method solid.sp1 has a lower value. For solid.sp2 &solid.sp3, It was given similar answer which is little above the applied pressure.
In theoritically solid.sp1=solid.sp2=solid.sp3=-p. Am'I wrong? can anyone explain this to me.
Please find the attached model.
Thanks
I have a bit similar simulation but it doesn't have an inner hole. I applied uniform pressure on the boundaries and introduce similar initial pressure on the contact surfaces. Assembly method was applied. When I applied union method without introducing contact surfaces it almost gave me the similar result. In bothe method solid.sp1 has a lower value. For solid.sp2 &solid.sp3, It was given similar answer which is little above the applied pressure.
In theoritically solid.sp1=solid.sp2=solid.sp3=-p. Am'I wrong? can anyone explain this to me.
Please find the attached model.
Thanks
Attachments:
Please login with a confirmed email address before reporting spam
Posted:
1 decade ago
Hi,
In response to Nithila's question; when I applied the Assembly method with contact pair to my model and I got a good result which when compared with my analytical result shows that the solid.sp1(is inner shaft z-component stresses and outer cylinder hoop-component stresses), solid.sp2(is inner shaft radial-component stresses and outer cylinder z-component stresses) and solid.sp2(is inner shaft hoop-component stresses and outer cylinder radial-component stresses).
But when I applied this same method to a hollow cylinder, the result wasn't consistent at the inner cylinder which means there is something missing like a proper boundary conditions.
Thanks
In response to Nithila's question; when I applied the Assembly method with contact pair to my model and I got a good result which when compared with my analytical result shows that the solid.sp1(is inner shaft z-component stresses and outer cylinder hoop-component stresses), solid.sp2(is inner shaft radial-component stresses and outer cylinder z-component stresses) and solid.sp2(is inner shaft hoop-component stresses and outer cylinder radial-component stresses).
But when I applied this same method to a hollow cylinder, the result wasn't consistent at the inner cylinder which means there is something missing like a proper boundary conditions.
Thanks
Please login with a confirmed email address before reporting spam
Posted:
1 decade ago
Hi Nithila,
The theoretical values you stated are for a uniform hydrostatic stress state. I can’t look at the model in details now, but I see that it’s a 2D plane strain model. The out-of-plane assumption for 2D plane strain, and plane stress too, both do not correspond to a uniform hydrostatic stress state.
Nagi Elabbasi
Veryst Engineering
The theoretical values you stated are for a uniform hydrostatic stress state. I can’t look at the model in details now, but I see that it’s a 2D plane strain model. The out-of-plane assumption for 2D plane strain, and plane stress too, both do not correspond to a uniform hydrostatic stress state.
Nagi Elabbasi
Veryst Engineering
Please login with a confirmed email address before reporting spam
Posted:
1 decade ago
Hi Nagi,
Thanks for the reply . If 2D plain strain and plain stress doesn't corrospond to hydrostatic stress which assumption I have to consider for the model? I thought when I applied plain strain condition it doesn't change the strain in the z direction. That's what I wanted. In the model two end faces don't affect by the pressure. I think that's why I got two different results . If I'm wrong please correct. Then how can I improve the model?
Thanks
Thanks for the reply . If 2D plain strain and plain stress doesn't corrospond to hydrostatic stress which assumption I have to consider for the model? I thought when I applied plain strain condition it doesn't change the strain in the z direction. That's what I wanted. In the model two end faces don't affect by the pressure. I think that's why I got two different results . If I'm wrong please correct. Then how can I improve the model?
Thanks
Please login with a confirmed email address before reporting spam
Posted:
1 decade ago
Hi Nithila,
Yes plane strain does not result in any strain the Z direction. Maintaining that zero strain requires a non-zero stress in the Z direction. For example, if the Poisson’s ratio is zero then the Z stress will also be zero, and it changes for different values of Poisson’s ratio. If your geometry is axisymmetric try that type of 2D model. Otherwise, you should create a 3D model.
Nagi Elabbasi
Veryst Engineering
Yes plane strain does not result in any strain the Z direction. Maintaining that zero strain requires a non-zero stress in the Z direction. For example, if the Poisson’s ratio is zero then the Z stress will also be zero, and it changes for different values of Poisson’s ratio. If your geometry is axisymmetric try that type of 2D model. Otherwise, you should create a 3D model.
Nagi Elabbasi
Veryst Engineering
Please login with a confirmed email address before reporting spam
Posted:
1 decade ago
Hi Nagi,
Thank you very much for the fast response. That comment is very helpful. I got a non zero stress in the z direction with non zero poisson's ratio.I think the result is resonable..I created 3D model and results are exactly the same. I have to try the one you have suggested as well.
I also created another 3D structure for applying a hydrostatic pressure on all the bounderies. The problem with the model is handling the bounderies because all are squeezing. So I created a quater of a cylinder. For that model stress on the all directions are similar(Theoritically ok). The second one is coated (polymer) cylinder . First I couldn't handle the bounderies. Then I have added more boundary condition to handle it. seems to be ok but I'm not sure the way I handle it. solid.sp2 &solid.sp3 are nearly3 times higer than the soid.sp1. I don't understant that. Any comment is appreciated.
Thank you very much for the fast response. That comment is very helpful. I got a non zero stress in the z direction with non zero poisson's ratio.I think the result is resonable..I created 3D model and results are exactly the same. I have to try the one you have suggested as well.
I also created another 3D structure for applying a hydrostatic pressure on all the bounderies. The problem with the model is handling the bounderies because all are squeezing. So I created a quater of a cylinder. For that model stress on the all directions are similar(Theoritically ok). The second one is coated (polymer) cylinder . First I couldn't handle the bounderies. Then I have added more boundary condition to handle it. seems to be ok but I'm not sure the way I handle it. solid.sp2 &solid.sp3 are nearly3 times higer than the soid.sp1. I don't understant that. Any comment is appreciated.
Attachments:
Please login with a confirmed email address before reporting spam
Posted:
1 decade ago
Hi Nagi.
I made a simulation using contact pair and assembly and the solid.sp1 obtained was a combination of z-component stress of the inner cylinder and tangential component of outer cylinder. similar cases occur in the solid.sp2 and solid.sp3 as well. From my understanding of Comsol. solid.sp1 is the z-component stresses, and solid.sp3 is the tangential component. Am I wrong?
Daniel.
I made a simulation using contact pair and assembly and the solid.sp1 obtained was a combination of z-component stress of the inner cylinder and tangential component of outer cylinder. similar cases occur in the solid.sp2 and solid.sp3 as well. From my understanding of Comsol. solid.sp1 is the z-component stresses, and solid.sp3 is the tangential component. Am I wrong?
Daniel.
Please login with a confirmed email address before reporting spam
Posted:
1 decade ago
Hi,
It just occur to me that the stresses I talked about are represented by the stress tensors solid.sx, solid.sy and solid.sz.
Thanks Nagi.
Daniel.
It just occur to me that the stresses I talked about are represented by the stress tensors solid.sx, solid.sy and solid.sz.
Thanks Nagi.
Daniel.
Please login with a confirmed email address before reporting spam
Posted:
10 years ago
Hi all,
It is really interesting problem!
I am trying to simulate the case that Mr. Iruikwu had done in his thesis, for two cylinders with a solid inner one.
I tried both contact pairs and boundary similarity, but non of them worked.The file size is big that I could not attach directly, however, please find it in this link!
cl.ly/0q0F190M3T0j
Any idea ?
It is really interesting problem!
I am trying to simulate the case that Mr. Iruikwu had done in his thesis, for two cylinders with a solid inner one.
I tried both contact pairs and boundary similarity, but non of them worked.The file size is big that I could not attach directly, however, please find it in this link!
cl.ly/0q0F190M3T0j
Any idea ?
Please login with a confirmed email address before reporting spam
Posted:
10 years ago
If you clear Solution and Mesh the file size should be much smaller and it can be attached directly.