'Propane Tank Burst Analysis' simulation project by ggiraldo


#1

Propane Tank Burst Analysis


This is a burst structural analysis of a 20 lb propane tank, like the ones used in BBQs and stoves.

The basic idea is to apply an increasing internal pressure to the vessel to find the safe operation pressure and the pressure at which rupture occurs. Some parameters for the simulation are:

  • Tank Material: Steel with yield stress 410 MPa and ultimate stress 610 MPa (real stresses)
  • Pressure Range: 0 - 6.9 MPa (0 - 1000 psi)
  • Material Model: Elastic / Perfectly Plastic (constant ultimate stress, as currently simscale doesn’t include fracture analysis)

CAD


The vessel was modeled in Onshape, using basic dimensions from a manufacturer catalog. The document is shared as public, you can find it in this link.

The geometry was directly imported to Simscale through the import app:

Mesh


The geometry was meshed using the Automatic Tetrahedralization algorithm. When using tetrahedral meshes, it is always advised to use quadratic elements (second order) to have correct accuracy (to avoid the infamous shear lock). The consequence of this is an increase in computational cost, but I see it as a trade-off for the simplicity in mesh setup and computation. As you will see further, there is currently a bug in simscale regarding quadratic meshes, so the analysis was carried out using a linear mesh.

The resulting mesh had the characteristics:

  • 172.442 nodes
  • 516.070 elements
  • 517.325 degrees of freedom

To simplify boundary conditions definition, face sets were created for the support face (bottom) and where the pressure is to be applied (internal faces). To select the internal faces, I first hid the external faces by selecting them, right click and select ‘Hide Selection’ option.

Simulation

Preliminary simulation


Before the intended burst analysis, A preliminary linear statics analysis was performed. This was to serve the purpose of checking rough values of the intended loads, stress levels and mesh integrity.

The basic statics analysis was selected:


With the material defined according to the elastic parameters:


For boundary conditions, the bottom is fully fixed and a pressure of 6.9 MPa applied on the internal faces, making use of the previously defined face sets:



At first attemp the simulation crashed with the following error:

*ERROR in e_c3d: nonpositive jacobian
determinant in element 357144
*ERROR in e_c3d: nonpositive jacobian
determinant in element 396625

Which means that there is a problem with the mesh. I suspected this to be related to the second order mesh, so posted on the forum, where it was confirmed. Then it was necessary to revert to a first order mesh.

Results


Here we can see the stress result. Blue areas are under yield stress and red areas are over ultimate stress:


We can see that plastification actually occurs, in the edges of the vessel. That justifies the non-linear analysis, so we will carry on. Take notice that because of the yield stress limit violation, this results are not valid. That is because we are outside of the linear range. We will see that the actual behavior is very different to the portrayed in this result, and also much more interesting.

Burst simulation


As this is a non-linear simulation because of the material model, the static advanced simulation was chosen, with non-linearity turned on:


This type of simulation is called pseudo-static, which means that there is a marching “time”, but inertia effects are not taking into account. The pseudo-time “t” controls the advancement of the simulation, and in this case was made to run between 0 and 1. This was taken advantage of to apply the pressure load in an incremental fashion, from 0 at t=0 until the maximum value at t=1.

The base constraint is constant in time, and defined just like the linear case. The pressure is defined as a function of t:

P(t) = 6.9e6 * t


The numerics were left as default, and the Simulation Control configured to meet our goals:

  • Timestep definition: Auto
  • Simulation interval: 1 [s]
  • Initial timestep: 0.05 [s] to aim to 20 steps, also the intervals at which solution is written
  • Write control definition: initial timesteps
  • Computing cores: 32
  • Maximum runtime: 14400 [s] / 4 hours

Results

This is the deformation of the vessel at maximum pressure at real scale, original is left. Quite large deformations! First indication of plastification:


As expected, plastification occured first on the top and bottom edges of the vessel. We can see this by looking at the Von Mises stress evolution of a point in the exterior face of the top edge:


We can see that plastification started at about 25% of the simulation, or for a pressure of 1.7 MPa (250 psi). Also it is important to notice that the ultimate stress was not reached. We can also see this if we look at the Von Mises stress distribution at maximum pressure state:


The blue zones are under stress below yield, and red zones (note that there is none) would be over ultimate stress. This happens because the plastification allows great deformations, consuming more energy, and causing the stresses to be redistributed to nearby areas. This phenomena is known as a “plastic hinge”. Maximum stress was 554 MPa.

Conclusion


A burst analysis was carried over for a propane gas vessel, using the Finite Elements Method. For this purpose, a non-linear simulation was built with an elastic-perfectly plastic material behavior (also called bi-linear). It was found that plastification occured at the vessel top and bottom edges, and that the resulting plastic hinges prevented the material from reaching ultimate stress levels. Plastification began to occur at a load pressure of 1.7 MPa (250 psi), but at the maximum of 6.9 MPa (1000 psi), ultimate stress levels were not reached in the material. Maximum estimated stress level was 554 MPa.


Original Automatic Post

I created a new simulation project called 'Propane Tank Burst Analysis':

Burst pressure analysis of a steel 20 lb propane tank.


More of my public projects can be found here.A


#2

Hi @ggiraldo,

Great write up, thanks for sharing! I hope your going to share the rest of your results.

Christopher


#3

Hi @cjquijano,

Thanks for your comment! I’m really glad you liked it.

The version you had read was a draft, but now you can check it and find full results and commentary.

Greetings.


#4

Hi @ggiraldo,

Thanks for the excellent tutorial. I wonder how your results compare to the governing standards in regards to strength and factor of safety.

The one thing I would change in your write up would be to change this:

to this.

It is so important to remind engineers (and management) that pretty pictures do not mean accurate results.

Thanks again!
Christopher


#5

You are welcome @cjquijano,

About industry standards, I think that in this case (because the vessel is not cylindrical) you would have to rely on the simulation for the stress level determination. The code gives you the strength level for the rated material and operation temperature, factor of safety included. Further strength level reductions would depend on manufacturing confidence and quality assurance tests. So, you would have to be very confident in your simulation if you are going to sign the design (and make tests, always test!).


#6

Excellent tutorial! I am still new to SimScale, but have run FEA for pressure vessels using other software, does SimScale have the capability to do a stress linearization through the wall thickness? I have seen a number of excellent tutorials and examples but have yet to see that feature demonstrated.

Thanks!

CMach


#7

Hi @cmach,

I’m really glad you liked it!

About the stress linearization, as Simscale is a general purpose FEA, it doesn’t have this kinds of posprocessing tools as a pressure vessel specialized tool would have. Anyway, this could be achieved using other posprocessing tools such as Paraview, extracting the stress data from the line of interest and analyzing.

If you have interest in making this, please write me a private message and we can talk.