PET Bottle pressurized 1

[nylas2u]

Strange problem on simulating a pressurized bottle .

On Abaqus/Explicit i'm using the folowings :

1. Density : 1.37E-009 tonne/mm3
2. Young's Modulus : 3100 MPa
3. Internal Pressure Load : 0.4 MPa

Now the strange thing is that I'm having a huge deformation.

In practice with a pressure of 0.4 MPa (4 athmospheres) i have around 0.5-1 mm deformation, but in abaqus the simulation results in a huge deformation and sometimes in errors without any result.

The strangiest part is that if i use 1.37 density (PET density in g/cm3) the results seems to folow the practice.

I'm new to abaqus is there a missed calculation of units or what is wrong ?

 

[nylas2u]

I didn't specified before, my model is in mm that's why i have to use SI (mm), and also the deformation varies according to the model shape of the bottle (0.5-1 mm).
The Poision Ratio is 0.37
Any ideea about this problem ?

 

[MechIrl]

Think your density units might be off, I would normally be in the region of 8e-6 kg/mm3 for stainless steel. Are you using any sort of mass scaling? I imagine you've got a pretty tiny time increment for a density of 1.37 e-9 if you're not?

It could also be the way in which you're applying the pressure? The default is instantaneous loading which isn't applicable for what seems like a quasi-static analysis. Are you using this or something like 'smooth step' loading?

 

[nylas2u]

Yes the incremensts are very tiny, but the pressure is instantaneous.

It could be a pressure problem !

 

[MechIrl]

o.k...seems as though I may have mis-judged what you're trying to model. Just to make sure - you're happy that the pressure should be applied intsantaneoulsy, as in some sort of shock or explosive loading of the bottle? I presumed you were doing some sort of quasi-static analysis where all you were interested in was applying the pressure gradually.

I'm afraid I can't help much with the former kind of analysis, haven't ever done any. Just recheck your units I guess and make sure the kinetic energy of the system is coming out roughly as expected.

 

[nylas2u]

The thing is that mainly i want to obtain the final deformation of the bottle after applyng pressure inside of 4 atm. Finaly to estimate the new volume after the bottle deformation under pressure.

It seems to me that the problem is much complex that i initialy thought.

 

[MechIrl]

Sorry, maybe I've confused you a bit, now I get what you're trying to do though. I suspect that things aren't working out as you expect because you're applying your loading instantaneously. For an Abaqus/Explicit analysis this is the equivalent of a shock loading.

What you should do is apply the load gradually. This will give you the final deformed shape of the container. The way to do this is to slowly ramp the load up to the desired final load through use of the *amplitude keyword.

The reason your analysis sort of worked when the material had a very high density is that the effect of the shock loading would have been lessened, resulting in a deformed shape that is close to what you expected.

 

[nylas2u]

1. Abaqus/Explicit keeps stoping in large displacement errors, tried to apply the pressure in 100 smooth steps, but there is no change (note that if i use automatic increment it is at E-008 order resulting in a huge computing time)

2. Tried the same problem in Abaqus/Standard and it gives a a fast result and it is running smoothly

MechIrl what do you think a Abaqus/Standard result is ok for this kind of problem ?

Thanks in advance

 

[MechIrl]

Yes it should be fine, in fact its more suited to this kind of problem as long as deformation doesn't get too large. I had presumed you were forced to use explicit for some reason, but if you're getting convergence ok in standard and the results look good then stick with it.

In terms of your model failing in explicit I don't really get what you mean by 100 smooth steps. Why not just apply the load in one smooth step (choose the 'smooth step' option with *amplitude). You will need to use mass scaling to increase the time increment size for a reasonable run-time.

 

[nylas2u]

My mastake, I ment this :

*Amplitude, name=Amp-1, time=TOTAL TIME, definition=SMOOTH STEP
0.01, 0.004, 0.02, 0.008, 0.03, 0.012, 0.04, 0.016
0.05, 0.02, 0.06, 0.024, 0.07, 0.028, 0.08, 0.032
0.09, 0.036, 0.1, 0.04, 0.11, 0.044, 0.12, 0.048
0.13, 0.052, 0.14, 0.056, 0.15, 0.06, 0.16, 0.064
0.17, 0.068, 0.18, 0.072, 0.19, 0.076, 0.2, 0.08
0.21, 0.084, 0.22, 0.088, 0.23, 0.092, 0.24, 0.096
0.25, 0.1, 0.26, 0.104, 0.27, 0.108, 0.28, 0.112
0.29, 0.116, 0.3, 0.12, 0.31, 0.124, 0.32, 0.128
0.33, 0.132, 0.34, 0.136, 0.35, 0.14, 0.36, 0.144
0.37, 0.148, 0.38, 0.152, 0.39, 0.156, 0.4, 0.16
0.41, 0.164, 0.42, 0.168, 0.43, 0.172, 0.44, 0.176
0.45, 0.18, 0.46, 0.184, 0.47, 0.188, 0.48, 0.192
0.49, 0.196, 0.5, 0.2, 0.51, 0.204, 0.52, 0.208
0.53, 0.212, 0.54, 0.216, 0.55, 0.22, 0.56, 0.224
0.57, 0.228, 0.58, 0.232, 0.59, 0.236, 0.6, 0.24
0.61, 0.244, 0.62, 0.248, 0.63, 0.252, 0.64, 0.256
0.65, 0.26, 0.66, 0.264, 0.67, 0.268, 0.68, 0.272
0.69, 0.276, 0.7, 0.28, 0.71, 0.284, 0.72, 0.288
0.73, 0.292, 0.74, 0.296, 0.75, 0.3, 0.76, 0.304
0.77, 0.308, 0.78, 0.312, 0.79, 0.316, 0.8, 0.32
0.81, 0.324, 0.82, 0.328, 0.83, 0.332, 0.84, 0.336
0.85, 0.34, 0.86, 0.344, 0.87, 0.348, 0.88, 0.352
0.89, 0.356, 0.9, 0.36, 0.91, 0.364, 0.92, 0.368
0.93, 0.372, 0.94, 0.376, 0.95, 0.38, 0.96, 0.384
0.97, 0.388, 0.98, 0.392, 0.99, 0.396, 1., 0.4

Exactly what you are sayng. It was just an expression mistake when i said 100 smooth steps

Thanks again for helping me

 

[Nileo2005]

Al your properties should be fine as well as your pressure. I would run it explicit with a .1s step time and a smooth step ramp. Shouldn't be too computationally extensive depending on the mesh size. I assume you're using shell elements, thickness of approx .3mm? If you do have mass scaling on, that could be the problem easy. I've had models scale 10 times their original mass before because I overlooked the MS factor when building. Thats a lot of inertia to carry deformation. What's Abaqus quote your stable time increment at?

 

[nylas2u]

Abaqus calculated increment is 2.865E-008. Today i want to make again a test using mass scale factor : semiautomatic, mass being scaled if the value is under 2.865E-006

Yes, you are right : the mesh part is huge (it's a botte having an complex design), and the thickness of the shell is .4 mm, varing to .75 - 1 mm at the bottom and on the neck

Abaqus Standard gives me a solution that follows the practice.

By the way, my interest is to calculate the final volume. Any ideea on how to do that. I have the displacement of elements but i don't have a clue how to calculate the final volume (after deformation).

Tried to export the result as VRML, import to CAD, converted to surfaces and calculate the volume.

But this method is too complex and i'm afraid that it could not be a relaible volume beaucause of the import and convert steps taking place.

You know anything about, how i could resolve this issue ?

 

[MechIrl]

Glad to hear it worked in Standard. You can get the volume of a part by using the query tool and selecting mass properties. I'm not sure if this will be approporiate for what you're doing but worth a look anyways. It only works in the pre-processor so you'll have to import the deformed mesh as a part from the odb.

Which CAD package did you use to import the VRML? It never seems to work out for me

 

[Nileo2005]

YOu can create a surface based fluid cavity and output the CVOL nodal history of the fluid reference node to obtain the volume.

 

[nylas2u]

PTC Pro/E but attention, i import the vrml as facet feature then with auto surface i convert this to a quilt in order to obtain the volum.

The main thing is that you have to convert the facet features in a solid or a surface quilt to do operations like cut/trim or manufacturing operations

You were not eable to import vrml ? or you just have difficulties after import of the model as vrml ?