Learning Forum

[rodmarti]

Hello guys,

 

I am a engineering professor and I am starting to use ANSYS as a pedagogical tool.

 

I performed the same exemple using other software (NASTRAN) and didn't find any difficulties.

The problem is very simple! It's a cylinder with R = 1000mm, L = 8000mm, t=1mm and an internal pressure of 1MPa.

 

Here we go: I want to model a thin walled pressure vessel and find the well know formulas S_1 = pr/t and S_2 = pr/2t. 

 

I then created a 1mm thick surface geometry, and meshed as shown in the figure below.

 

 

I applied a simply support to both sides and  a 1MPa pressure to the cylinder.

 

To my surprise, when I measured the stresses in the center of the cylinder, only S_1 converges to the right value.

 

 

The S_Y converges to 1000MPa but S_X converges to something close to 300MPa (instead of 500MPa).

 

What am I doing wrong?

 

Best Regards,

 

Rodrigo Martins

 

 

 

 

 

[jj77]

Well the same value as ansys is obtained in Strand7 (1000 MPa for hoop, and ~250 MPa for longi. stress).

 

To use the pressure vessel formula here we would need to apply the cap force ((Pressure*PI*d^2)/4) on the two edges of the cylinder to be strictly correct. If that is done it gives then 500 MPa in the long. direction (see ZZ stress below - Z is along the cyl.), as expected.

(The pinned edges must be free to stretch since we apply an axial cap force on these two ends, thus we can not restrain axial movement)

 

 

 

[rodmarti]

Thank you, 

It worked!

I had the impression that if I simply restrict the displacements in the ends, it would be equivalent to apply the force. Turns out that it is not the case.

 

Best Regards!

 

Rodrigo Martins

[jj77]

No worries - happy to help