Application of point loads 1

[CameronE]

I have a question regarding applying loads taken from one analysis to another (higher level) analysis.

From a beam element FEA package (Autopipe) the forces and moments acting on a nozzle were determined in the form Fx, Fy, Fz, Mx, My, Mz. These are all obviously forces and moments at a single point.

To analyse the nozzle the forces and moments were acting on, I created a plate element model of the nozzle and the vessel it was attached to, as there were other attachments and stress concentrators on the vessel which could cause problems.

My question is this; how do you best apply the point loads/moments from the beam element model to the 3d plate element model?

I created a dummy node at the centre of the nozzle and used rigid links to connect it to the flange of the nozzle. All the loads were applied to the dummy node. Naturally this created some local stress concentrations around the flange which would not be present in reality. Is there a better way of doing this?

 

[GBor]

It depends on the FEA package that you are using, but the forces could be distributed as a pressure over the face of the surface. Some packages will take point loads like the ones that you mention and develop the equivalent pressure loads...sounds like something that would be very helpful to you. Moments can also be distributed, but it is, obviously, more analytically intensive if you don't have one of the packages to which I referred in the previous sentence.

Using pressures alleviates that problems that you are seeing with the rigid elements.

 

[GregLocock]

Another approach I've used is to apply the point load to a relatively soft 'load application structure' that then mounts to the main structure. Since that is a very accurate model of a rubber bush mounted to a car it gives reasonable results in my case. Obviously you don't worry about the stresses in the interfacing structure. If I was feeling posh I'd call it St Venant's principle.

Lots of people use 'spiders' of rigid elements to do this. Fail.

Cheers

Greg Locock

SIGlease see FAQ731-376 for tips on how to make the best use of Eng-Tips.

 

[CameronE]

GBor,

I am using Strand7 which allows forces to be applied as both face and edge pressures. I wasn't sure how to use them in this case however. The axial force is easy; an edge pressure applied at the edge of the nozzle.

The x and y components leave me a little lost to be honest. Since the nozzle is basically a pipe, so its not as simple as applying an edge or face pressure to once side of the nozzle. I thought about summing the x and y components into a radial force, but the y force is towards the centre of the nozzle and the x force is outwards.

GregLocock,

Thanks. If I understand your post correctly, you create your interfacing structure and simply apply the loads as point loads on selected nodes?

 

[jhardy1]

CameronE,

I use Strand7 also. The approach I generally adopt for applying flange loads to a plate / shell model of a pipe system is to look at each load component, and then apply an equivalent face pressure or face traction to all of the elements comprising the flange itself.

Note that Strand7 has "equation input" mode when entering numeric data, which means when entering a pressure load for example, you can either enter a discrete numeric value, or an expression which is evaluated at all selected elements, to derive a unique value for each element. In addition to the usual complement of trig functions etc, there are also a couple of handy shortcuts, including "x", "y", "z" etc (being the global coordinates of the centroid of each element), "TA" (for the Total Area of the selected plate elements or faces of brick elements), "TL" (for Total Length of a group of selected beams, or the total length of the selected edges of plate elements, etc), as well as numerous others.

(Check out the On-line Help section on "Entering Numeric Data", found under the top-level heading "Essentials", for more information.)

For example, to apply a lateral load of 20 kN to the flange, you would select all elements making up the flange, then apply a Global Traction in the appropriate direction. Instead of calculating the actual traction stress required to generate a 20 kN load, you would simply enter:

20000/TA

(assuming you are in base SI units), and Strand7 will calculate the applicable traction stress.

For a bending moment of 100 kNm on a 200 OD / 100 ID flange, using your knowledge that

Bending Stress = M y / I

you would apply a normal stress, and then type in something like the following expression:

100000 * y / (pi * (0.2^4 - 0.1^4) / 64)

and Strand7 will generate a normal pressure distribution which varies linearly with respect to the y-coordinate of each element.

Hope this helps!

 

[CameronE]

Thanks Julian, that is a massive help.

 

[Hurricanes]

I have come across a similar problem. We had point loads from a beam model which we needed to apply to a 3D plate/shell model. After talking to some senior guys here I modelled the point loads using rigid elements.

I am interested to hear why this is considered such a bad idea.

I also use Strand7, their latest newsletter actually shows a point load moment being applied to a channel section. They use rigid elements to do this. The newsletter can be found on the main page of their website, strand7.com.

 

[johnhors]

A rigid element is by definition infinitely stiff and thus unreal. By using them to apply loads to your model your are introducing false infinite stiffnesses into the model, this is very artificial and will most definitely result in some degree of corruption in the model results. Whether this is significant or not is up to you, but if, as is possible the rigid elements change the load paths then you have real problems. If your area of interest is at or adjacent to the rigid element then you must come up with a better solution.

Moments can be (and should be!) applied to 3D solid or shell models via a pressure distribution. There are products on the market that can do this. Also see the 3-2-1 thread for some related information on why rigid elements are bad.