Nozzle to Vessel flexibility simulation

[mikycampo]

Dear all,

i'm analysing the flexibility of a petrolchemical plant using ansys piping capabilities. The model includes some vessels connected by piping systems. I've modeled the vessel and the pipes with PIPE16 and PIPE18 elements. My problem is how to simulate the beams connecting the axis of the vessel to the nozzle in order to take into account the nozzle-to-vessel flexibility.
Can someone give me some simple advises or formulas to calculate these equivalent beams?

Thanks a lot

Michele

 

[C2it]

I'm not familiar with ANSYS, however....

There is a simple approach in Kellogg's Design of Piping Systems, which gives a restrained pipe element, the length of which is intended to have flexibility equivalent to the vessel shell. However that method lacks accuracy appropriate to an ANSYS analysis.

A better approach would be to apply the methods of WRC 297 to establish directional spring rates. This is what software such as Caesar II does.

 

[C2it]

Second thought ... do a small ANSYS plate model of each nozzle region, establish the respective spring rates and include them in your piping model ?

 

[mikycampo]

thanks a lot for the answer.

Where I can find, in the web, the formulas to design the equivalent beam to simulate the shell/nozzle flexibility?
Or how I can use the bs5500 annex G formulas: i've red them a lot of times but i cannot understand how to evaluate the parameters to give to a beam element.

thanks again

Michele

 

[C2it]

Kellogg eq 3.29 ....

L = 0.017 * I *(R / (rm^2) * t)^(3/2)

L = 'virtual length of element (ft)
R = vessel radius (in)
rm= mean nozzle radius (in)
t = vessel thk. (in)

The 'virtual length' element would be fixed against all translations at the shell / nozzle interface, extend 'into' the vessel and then fixed against lateral movement at the far end. Good luck with this, as I said, it does not live up to FE acuracy at all.

PD5500 or WRC297 .... you are looking for spring rates, not anything to represent a beam element, so you should have a matrix or spring stiffness set for your nozzle node.

Why not use the power of FE and model a piece of vessel using plate elements ????

 

[mikycampo]

Thanks C2it,

I don't use a plate elements model, because i've more than 50 different nozzle / vessel connections and it will become too expensive for me to make a model for each nozzle.

Thanks for Kellogg formula, but same data lakcs:

- which section must have the virtual element?
- which material formulation ?

these two infos are the data to put in an ANSYS beam element.

thanks again Michele

 

[C2it]

Michele,

I don't use ANSYS, but I guess that you have a string of 'pipe' beam elements leading, say, to a particular nozzle. You would have your last element connecting to the vessel nozzle / shell intersection. Then the virtual element effectively poking inside the vessel in line with the preceeding pipe element. The material constants would be that of the vessel.

 

[mikycampo]

Thanks.

But in your formula I don't know what is "I" parameter!

Last question: from the end of the "virtual element" to the axis of vessel (simulated by beam/pipe elements) do you think I must provide a rigid element?

Bye Michele

 

[NozzleTwister]

To bad your not using CAESAR II since those capabilties are built in.

If you have access to a progam like NozzlePro, the flexibities can be calculated easily.

If you have an in-house vessel program, it probably has the capabilties to calculate accurate nozzle flexibities.

NozzleTwister
Houston, Texas

 

[MJCronin]

Why are you doing this...???

ANSYS is a powerful hammer tyically used for detailed analysis of unique piping/vessel geometries or bizarre loading conditions (wave action for example) on problems that the standard analysis tools ( AESAR II or AUTOPIPE) cannot handle.

Now, CII and AUTOPIPE are used for the other 99.99% of code related piping stress analysis and internally have the tools to handle almost all of the configurations commonly encountered in power plants refineries etc.....

As stated above, WRC 297 contains some of the information you may need on nozzle to pipe flexibilities.......and you may incorporate this in your work......but this methodology for modification to element stiffnesses is also contained within CII

Try posting your question on the

http://www.coade.com

website..

Cheers...!!

-MJC

 

[C2it]

Michele,

Sorry, the I value is the moment of inertia of the pipe.

The 'virtual element' must be fixed against traslations at the vessel shell / nozzle interface. At the other end, fixed against lateral translations and axial rotations only. Those restraints will provide the full set of boundary conditions that you need. A rigid element is not required. I have to agree with Nozzletwister and MJC's remarks above, and wonder why you are using ANSYS for this work ?