Applying a moment

[lurks]

I am working with NX Nastran 4.1 in conjunction with UG NX4 and am trying to perform a finite element analysis on this bracket. There is going to be a moment on the outside face of this bracket as a result of a 26.5" lever arm being attached there. My question is how do I apply a moment to that face in order to get a fairly accurate result? I have attached a screen shot of what I am working with. Any help with this matter would be greatly appreciated.

Thanks in advance,

lurks

 

[rb1957]

with respect, IMVHO, not the most efficient way to transfer moment (and shear) ... but you know your design constraints, and why you've come to this design.

think of how the structure is going to apply the moment ... probably a "heel and toe" loading ... the bolt will provide the tension 1/2 of the moment couple, and the "toe" of the brkt will provide the compression.

if the attached brkt has webs, you could use the most extreme edge of the brkt flange; which minimises your couple forces; otherwise you'll have a small moment arm (between the couple forces) and large forces.

don't forget the bolt is also carrying the shear load. also, the bolt May be able to take alittle of the moment itself, how you apply this depends on how you're modelling the brkt (2D or 3D).

i'm alittle surprised that you're resorting the FE to solve what Looks like a sheet metal brkt ...

lots of things to check (by hand) ... flange bending (of the angle applyiing the moment), bolt (interaction of shear and tension)

 

[prost]

Sometimes you need the FEA just to get the pretty pictures and impress the big bosses.


Anyway, is the stress in the area where you are applying moment important? If not, you can apply a moment first by defining a coordinate system aligned with the face (Xp,Yp,Zp) where you are applying the load, and then apply a normal traction with a formula

S=Smax*zp/H

where Zp='z-prime' is aligned with the surface of this face where you applying the load, Xp is aligned with xc, and Yp is perpendicular to this face. "H" is the length of the area, in the Zp direction.

 

[prost]

I forgot to say, put this local coordinate system (Xp,Yp,Zp) in the very center of that face where you applying the moment. The length of the face in the Zp direction is actually 2H.

The Moment you are applying is then

Mo=(Smax*thick/3)*H^2

If you know the Mo, then you back out the Smax of course. 'thick' is the length of this face in the Xc direction.

 

[GBor]

Another option is to tie the center of the hole to the nodes around the hole with rigid beams, then apply the moment to the node at the center of the hole. This artificially stiffens the hole, but if the stress in that area is not important, you should be OK. There are ways to manipulate the stiffness of the "rigid elements" using springs instead so that the hole stiffness enhancement is minimized, depending on the software that you are using.

 

[lurks]

For the software that I am using there is a tool for applying a moment, but the problem is that it is saying that it is an incompatible mesh. See attached.

Thanks,

lurks

 

[GBor]

It looks like you put the beam in, but you modeled the bracket with tets (not sure that is appropriate and you need more than 1 tet through the thickness). If there is a beam through the center, you probably have Degree of Freedom issues unless you extended the beam not only to the rim of the hole, but penetrate the structure by one element. Beams are 6 DOF elements and tets are 3...that may be the problem, but I'm not familiar enough with NXNastran.

Garland E. Borowski, PE
Star Aviation

 

[prost]

If the tets are quadratic, one should be enough for most of the web sections--any connection point would have 3D stresses, so 1 tet through the thickness is not nearly enough (not that I would ever recommend tets for anything, since they are so squirrely numerically).

Are you applying those forces as point loads? These are illegal within the finite element formulation--you cannot use them and get numerical convergence. Better to use a distributed load, a normal traction that varies like the moment on an Euler Bernoulli beam.

It might be an illusion, but it looks like the holes at the top and bottom are not round. Are those true representations of the actual holes?

Gbor..or anybody for that matter, how can you tell there's a beam in the hole (another apparent violation of the formulation, since point constraints are not allowed).

Regardless of whether you think point loads are allowable or not (easy to show mathematically they are not, and the logic, though not mine, is nevertheless flawless), it makes little sense to add singularities (which result from point loads and point constraints) to a problem where singularities do not exist. Surely the plane where you are loading this bracket does not connect to another structure with a few spot welds; therefore, point loads or constraints are poor representations of the real connection and interaction.

 

[GBor]

Prost,

I may be seeing two opposing force vectors running through the middle of the hole...it just looked a little like a beam. Not really sure, and don't really want to reload that HUGE picture! If it is just forces, then I have the same problem you did with the point loads. If it is a beam, then I am concerned about the DOF mis-match. Either way, I don't like tets...as you also mentioned.

 

[corus]

Perhaps the incompatibility is due to using solid elements rather than shells? If you use shell elements then you'll have rotational degrees of freedom and be able to apply a moment directly. If you use shells then fill the hole in as results will be meaningless around there with a point load. You won't get the stress concentration at the radii with shells but then do you need to know what that is?

You'll also have problems defining the correct restraints at the bracket supports. The assumptions you make there will probably be as good as the assumptions you'll make at applying the load. For this reason I'd be wary of making a model that goes to extremes of definining shape when at the end of the day you're only guessing at how it's restrained and loaded.

You could go the whole hog and model the connection that is applying the load and use contact between the bracket and the connection. Do the same at the bracket supports too but perhaps use rigid bodies for the contact.

Frankly for the time and effort of modelling the bracket wouldn't it have been cheaper just to make a bracket and bolt it down and apply a moment? If you're not bothered about fatigue then have a look at it after and if it looks bent then it's yielded and failed.

corus

 

[crisb]

There may be a load/mesh mismatch. Pressure loads are normally applied to areas. Line loads to lines, and point loads to points.
In 3D models its usually best to use pressures. Alternatively define a point on the axis of the hole, tie it to the bore with a rigid link, and then apply a moment to the point (remember to have all 6 DOF active throughout the model).
4 Node tets are not recommended in a single thickness, so try to use quadratic elements with at least 10 nodes (if you arent doing this already).

 

[rb1957]

tet10s good, tet4s bad

i'm wondering if the "tool for applying moment" is trying to apply point moments to the grids ? these could be inconsistent with the FEA code (I'd suspect that the dofs of the tets are Fx,y,z, rather than all six) ?

i'm also not so sure about the loading ... there's a bar attached to the bolt (preloaded i'm sure). the bolt May take the moment in bending (but i'm sure it's not happy to do this) but then the bolt would load the brkt through it's head (there should be a couple on the inside face of the brkt, offset a little from the hole).