Pipeline Loads applied to a nozzle FE model 1

[migliano]

I'm modeling a nozzle connected to a vessel using ANSYS SHELL93 elements. My great dilemma has been how to apply the pipeline loads to the nozzle. ANSYS offers no options to distribute the forces and moments around the edge of the nozzle.

I read the following suggestion on this forum:

"That said, my approach is to model the end of the pipe with a spyder arrangement and then apply the loads (forces and/or moments) to the single spyder node. Let me know if this is what you are after, and I will try to give you more details.
A spyder arrangement can be best described as a set of spokes on a bicycle wheel. These spokes are beam element, but with very special (non-physical) properties. You want them to offer no resistance in their axial direction, but to be infinitely stiff in bending. This can be accomplished by applying real constants of very high Ixx and Iyy, but very low cross-sectional area. What I do is create a node at the center of the end of the nozzle, and then connect this node with these beam elements to the nodes that make up the end of the nozzle."

The problem is that I got a considerable change on the stresses when increasing Ixx and Iyy one order of magnitude.

Can anybody shed some light on the topic?

Thanks in advance.

 

[corus]

Basically they're applying rigid links to nodes on the nozzle bu using very high values of inertia for the beam elements. I believe ANSYS has rigid links so you're better off using those than beam elements. Bear in mind that the rigid links will make the end of the nozzle rigidly circular and prevent any deformation so it's best to apply the rigid links well away from the area of concern. The method of beam elements tries to get round this problem by using a relatively low area so that the nozzle can deform from a circle. How low is low, however. It's best just to apply the beams or links well away from the connection, say about 6 wavelengths away.

corus

 

[migliano]

corus,

first of all thanks for the reply. Could you clarify what you mean by wavelength?

Yesterday I played a little bit with the rigid link element (MPC184 Multipoint Constraint Element: Rigid Beam) and it looks like that's the best way to go.

I'm still not confident on the results though. I have the results of the same problem ran with NozzlePro 5.2 and the two are quite different. First of all, NP52 gives you the results already split in Pl, Pl+Pb+Q, and so on. ANSYS as you know doesn't.

I'm trying to interpret the results according to a paper published on the ASME PVP-Vol. 336, "A Comparison of the Stress results from Several Commercial Finite Element Codes with ASME Section VIII, Division 2 Requirements" which can be found at this link. It looks pretty straight forward and uses the Stress Intensities on the top surface of the elements.

Any ideas are welcome...

 

[corus]

If you look in Roark, the wavelength of a thin cylinder is 1/lambda where lambda is the sqrt(sqrt(3*(1-v^2)/r^2.t^2)). It generally refers to the shape of the radial displacements along the length varying like a damped sine function. 6 x the wavelength (or 2.5xsqrt(rt) I think) is a good distance to apply loads as the variation in radial displacements are then negligible at that distance. Also, your element size should be related to one wavelength or less to get good results.

I think in the example in the link you gave there is a flange at the end of the nozzle and presumably they are assuming that that is stiff enough to apply loads to so that the infinite stiffness given by the rigid links there will give an insignificant error at the nozzle connection.

I don't know NozzlePro but a pressure vessel code will have analytical methods to calculate the stresses at nozzles. Your FE stresses will be the linear stress through the thickness as you're using shell elements. The surface stress will have bending components which can be either primary or secondary depending on the classification. The mean stress will be either primary local or primary membrane, if I remember. The link seems to be a better reference for classification purposes as it's a while since I did that kind of stuff, sorry.

corus

 

[migliano]

corus,

thanks again.

In mentioning the flange in the example in the link you may have given me another idea.

Actually NozzlePro is a FE software geared toward vessels and nozzles but with limitations. We made a first run with NP52 but what we're trying to model we can only do with a more powerful FE software.

Thanks for the help...

 

[vonlueke]

migliano: An RBE3 element will distribute loads without adding stiffness to your structure. Put the RBE3 master (central, dependent) node (node 1) at the centerpoint of your nozzle, and spoke it out to all desired so-called "independent" nodes (nodes 2 through n). Never use an RBE3 with less than three independent nodes; and don't create an RBE3 in which all nodes are only collinear. If Ansys gives you a warning about node 1 not being associated with an element (which you usually don't get in other programs), then also connect the RBE3 centroidal node to your nozzle using a "dummy" beam element having a very small circular cross section and a "rubber" modulus of elasticity.

 

[migliano]

vonlueke,

thanks for the input. It looks like your approach is the same used by ANSYS Workbench (applying what they call a Remote Force).

I'll give it a try. Thanks.

 

[cbrn]

Hi,
from the date of the latest post, I desume you have already come through the problem; however, here's other two small suggestions:
1- you can take advantage of the loading capabilities of Workbench by interoperating between WB and "Classical": you can either start your model processing in WB and then exit to Classical from within the WB interface, or write the .INP file and then read it into Classical; or, if you are familiar with APDL, there is almost nothing in Classical that you can not do also in WB, simply by adding "Commands" objects as needed. I never used it, but I seem to know that WB has a way to show the linearized stresses (but it can not do categorization, i.e. it's up to you to decide what is "primary" and what is "secondary", or "general" and "local")
2- There is an application which works as an add-on of WB, which allows to perform PV analyses quite easily: it's the "PEA" module, which conforms to european PED / EN 13445 as well as ASME VIII-2

Regards

 

[migliano]

cbrn,

thanks for the reply.

You've touched another subject with which I'm struggling a little bit right now: the stress categorization. There is some good reading material on this link.

I was not sure if WB had a linearization tool but your post implies that it has one.

I'm about to model a section of a skirt and reactor and I'm sure I'll run into more questions regarding categorization and linearization of stresses.

Regards...

 

[migliano]

I found this paper on ansys.net. It sheds some light on the use of the RBE3 element and mentions what is now the MPC184 (Multipoint Constraint Rigid Link and Rigid Beam Element). It includes an example of a load applied to the center of a hole on a plate.

Regards.