## General Mechanical

#### Modelling constraints

• francescone96
Subscriber

Hi everybody,

i'm performing a 3D analysis on Ansys Transient Structural. The geometry is made up of 2 concentric tubes of a certain length, the inner tube is made of steel while the external one of aluminum.

• SaiD
Ansys Employee
Hi,nDo you want to prevent thermal expansion of the Aluminum tube in the radial direction? You can use Cylindrical support, scope it to the outer surface of the Aluminum tube and set Radial to be Fixed. If thermal expansion is not constrained in Tangential and Axial directions, set them to be Free.nHope this helps,nSainn
• francescone96
Subscriber
Thank you for the fast reply Sdeogeka. nThe radial expansion is not totally blocked, because this is just a simplified model, but around the external tube there is other aluminum. The constraint i want to apply is in between the fixed support and the free-surface. nAnyway thank you very much for the attempt!n
• peteroznewman
Subscriber
nFrom your description, it sounds like you have a very large block of aluminum with a hole in it. Inside that hole is a steel tube. The OD of the steel tube is equal to the diameter of the hole in the aluminum at the zero strain reference temperature of say 20 C. You want to compute the stress in the parts when the temperature is 800 C.nIf you don't need to simulate the time history of the heating up, this could be a Static Structural analysis. I don't see the benefit of solving it in Transient Structural.nDo you need to solve the problem in 3D to get the edge effects of the steel tube at the free surface of the aluminum block? I expect the stress will be lower there because of the free surface. The stress will be higher deep down in the hole away from the free surface.nTo get the maximum stress far from the free surface, you would solve this problem as a 2D plane strain problem. The simplest boundary conditions would be 1/4 symmetry, so you have two planes where X=0 on the edges along the Y axis and Y = 0 along the X axis. Make the aluminum tube have a very large OD.n
• francescone96
Subscriber
Thank youpeteroznewman nAbout the static analysis i agree with you, it should decrease a lot the computation time. I just need the transient module for a further analysis i'll have to perform if, after heating up, i apply a displacement on the steel part in order to remove that from the contact with the aluminum (for this reason i need also the frictional contact).nStill, i don't know which condition can i implement to the external surface of the aluminum. As you said it's like a large amount of aluminum is around the steel tube. I was wondering if there is a way to apply a spring for each node of the external surface, which has the same stiffness of the aluminum. I have tried the elastic support, but the stiffness is unknown and i think that ansys can compute it. For this reason i think that symmetry could fit with my problem. I tried symmetry but a simmetry normal is requested. n
• peteroznewman
Subscriber
nYou can apply a displacement on the steel part using a Static Structural analysis, you don't need transient to do that.nIf you do a quarter model in 3D, and the tube is running along the Z axis, then one cut plane is XZ that has Y as its normal and the other cut plane is YZ that has X as its normal.nIt is okay to have no support on the outside of a very large aluminum tube. Make the OD of the aluminum tube 4 times the diameter of the hole and get that solution. Then make the OD of the aluminum tube 8 times the diameter of the hole and get that solution. Do 16 times the OD of the hole. Make a plot of stress vs radius. Overlay those three plots. Look at how much the peak stress at the hole changes between the three models. You should find that the stress at the hole doesn't change much as the OD is increased.n
• francescone96
Subscriber
Thank you again, i'll try that. n
• mzhossain2001
Subscriber
If you apply 800 C - I suppose, it shall be a nonlinear analysis. You may check applying hand calculation.nAnd why do you need to apply constraints to the outer tube? That is not clear. If the outer tube is supported by any external support - then constraints of the outer tube shall simulate to that boundary condition of the support that will be applied to.nIf the temperature is applied - I suppose it will be applied gradually. You may not apply all 800 C at a time. Even if you apply all 800 C at a time - the tubes will take time to absorb that whole 800 c, from the practical point of view. So, I suppose it shall be a transient analysis. Hence, from that pretext, you need to do a Nonlinear transient analysis.nnI understand, what I am saying is not matching up with the other comments above. But, the way you described your problem, I suppose this is the only solution that you may opt to sooth your need. n