trying to reproduce the results of a test 3

[PerKr]

I am testing a new version of an old handle for refrigerators. The handle is basically an aluminium pole with two brackets at each end holding it to the door. Changes have been made to both the handle and the brackets, so I try to test them separately, sort of. I've tested the new handle with the old brackets and am now testing the old handle with the new brackets.

The opening force, applied at the middle of the handle, is about 60 Newtons, possibly even lower due to the nature of the test.
After about 80,000 openings, the old bracket failed. I'm thinking this is either a matter of fatigue or something was a bit off with the test equipment.

With the FEA software we have, I can only look at separate parts, so when calculation the forces acting on the bracket I have considered the handle as being solidly mounted at both ends, resulting in a force of F/2 and a moment of F*L/8 acting on each bracket. The resulting Von Mises stress, as well as max principal stress, is above Rm for the zinc alloy used, which is about 330 MPa.

obviously, something is wrong with my analysis. I'm quite certain that it's the fact that I cannot take into consideration the flex of the door and handle which should be making life easier for the bracket. So what do I do? Reduce the applied forces and moments in the analysis until I get the desired max principal stress?

Also, does anyone know where I can find fatigue diagrams for zinc alloys? aluminum alloys?

 

[MikeHalloran]

People don't always apply force at the middle of handles.


Zinc info:

http://www.eazall.com/

Mike Halloran
Pembroke Pines, FL, USA

 

[prost]

Not knowing the aluminum alloy, I could only guess. If the alloy is used in airplanes, its fatigue diagrams (S/N) can be found in MIL-HDBK-5.

 

[rb1957]

i don't know if i understand what you've done ... it sounds like you have a handle with a bracket at each end and that you're assuming the brackets are fixed, and that the handle is also fixed to the brackets ... fixed assumptions are always easy but seldom Right (they're usually conservative as nothing is Truly fixed).

i'm not sure what "Rm" is as a strength.

personally i find the the force i apply to a fridge handle varies significantly, depending on the seal.

why can't you model a handle complete with it's brackets, and check that the loads the FEA is putting across the handle/bracket interface can actually be applied ?

 

[GBor]

I would recommend that you try to balance the load instead of applying fixed boundary conditions. You still have to apply a minimum of boundary conditions to stop rigid body modes. The other option is to model a portion of the refrigerator door and fix the edges of it. Ignore the stress in the door portion and concentrate on the stress in the handle and brackets...this would allow the load path to be a little better and give the flex that you need to properly apply the moment at the brackets, if I'm understanding correctly.

All the other suggestions are also well stated.

Garland E. Borowski, PE
Borowski Engineering & Analytical Services, Inc.
Lower Alabama SolidWorks Users Group
Magnitude The Finite Element Analysis Magazine for the Engineering Community

 

[PerKr]

MikeHalloran: Agreed, but I want to be as hard on the handle as I possibly can within the limits of the standards. Consider that a freezer handle can be subjected to more than 500N when running. I've seen handles pass the tests only to break in the hands of our customers and I want to avoid having that happen again.

rb1957: "Rm" translates to "ultimate strength" (thought it was "yield strength" first, but apparently not. glad I looked that up). If I happen to mention "ReL", that would translate to "yield strength".
I could try to model the handle and brackets as one part. didn't think of that. thanks. we only have the catia generative part structural analysis 2 module, so I was stuck thinking that I can't do assemblies.
The door opening force will depend on the seal, the type of magnet used and the opening speed. I've actually measured the impact of the opening speed on the opening force and for a slow opening (10mm/minute), I would expect an opening force as low as 25N. Higer speeds (1000mm/minute) would result in an opening force of at least 50N for a warm cabinet with a hole to reduce any vacuum. I've measured 150N on a normal opening and 78N for a careful first opening of a running cabinet. Always with a good seal of course. The cabinets placed in the machine won't have time to achieve a perfect seal, so maybe I should reduce the load to 50N for my analysis. wish I had equipment to measure the real world values. Maybe I should try to make something up for this.

GBor: not quite sure how I would model the bracket and door as one part. I've used a "contact virtual part" to simulate the door and no clamps (except for keeping the virtual parts in position) but maybe I could use forces instead.

Thanks for your helpful posts guys

 

[ProbaSci]

Do you have a previous analysis to compare to? A previous design that you can test under the same boundary conditions to compare with? Can you do a quick manual analysis to compare?

Are you approximating a dynamic load with a peak static load?

http://www.probasci.com

-
Implantable FEA for medical device manufacturers

 

[PerKr]

There are no previous analysis available as far as I am aware of. I am performing tests as we speak, comparing the current handle and bracket to the new handle and bracket.
We haven't had any FE software up until just recently and the designers generally don't seem interested in performing any calculations or analysis, which becomes really frustrating when they want me to test things which are almost certain to fail.

I am trying to determine the likelyhood of fatigue failure using a static load, so yes, I am trying to approximate a dynamic load with a peak static load.

 

[PerKr]

correct me if I am wrong, but as it's a pulsating load, I should probably be looking at the average stress (which would be approximately half the peak stress) instead of the peak stress, right?

 

[PerKr]

why can't we edit our messages? I'm making myself look pretty stupid now... We are talking about ductile materials, so I need to find Kt?

 

[Spirit]

PerKr,

when you restrain a model it is very likely to have high peaks of stress in the vicinity of the constrained points. What I would do as a first step is check where the experimental failure occurs and what stress is calculated in that location using your model, and then make some considerations about fatigue life.

Regards.


SD

'Ability is 10% inspiration and 90% perspiration.'

 

[johnhors]

Spirit,

"when you restrain a model it is very likely to have high peaks of stress in the vicinity of the constrained points"

Yes, that is why GBor suggested applying a balanced set of loads with minimal supports purely to prevent rigid body motions. Doing this correctly eliminates all spurious stress peaks.

 

[PerKr]

In the analysis I get stress concentrations along the break path. So it seems to be pretty close to what is happening, except that the stress in the analysis is higher than the ultimate strength of the material. So, I'm either misinterpretting the results or I have the wrong inputs.

 

[johnhors]

PerKr,

I hope that you are not using all the default settings of Catia GPS, it is tuned for speed and not accuracy. The element sizes it suggests produce a highly facetted model and have to be reduced considerably. It is possible to apply balanced loading and minimal supports using GPS, I have seen it done.

 

[PerKr]

I have reduced the size of the elements where it's necessary. I tried using balanced loads, but ran into some problems ("relative pivot too small", basically the part was moving around). Should be able to make it work, but I can't spend a whole day doing it, so for a quick fix I resorted to using a minimal number of "advanced" constraints (don't know why they call these constraints "advanced", maybe because they're a bit more advanced than just using the "clamp" constraints). The stress is still in the same area but was slightly lower (about 30MPa lower). The maximum stress occurs in a thin rib (2mm thick) and a cut-plane analysis shows that the von mises stress is 280MPa on the inside surface and about 160MPa in the middle of the rib.

 

[ProbaSci]

I'm not sure if you are doing an automated fatigue analysis within your package, but I'd start with a simple static load analysis at the peak load and see how that compares to the yield / failure stress.

Since your analysis of the previous design places peak stresses at the observed failure locations, that suggests your load model is good at least in terms of directions and locations of constraints. How does the applied load in your previous design compare with observed breaking loads (static if you have it or can test it?). This will help you determine if the stress magnitudes from your model are also correct.

Once the static model is working, then go after the fatigue condition.

http://www.probasci.com

-
Implantable FEA for medical device manufacturers

 

[PerKr]

Went out to the laboratory, grabbed a door, a handle and a set of brackets and did a simple test using a dynamometer. What happened was that I reached well over 500N (552N I think) and then aborted the test as the brackets were still intact and the instrument isn't supposed to be used above 500N.

What did I learn? well, for one thing, it seems that the screws loosened somewhat, resulting in virtually no movement at all of the bracket. This should mean that no moment is transferred to the bracket. All I have left then is a force which is equal to and opposite to the force pulling on the handle, divided between the two brackets. This should also mean that if I apply the force further towards either end of the handle, the bracket which is the closest should break sooner

another thing it seems I've been wrong about: I should be recieving the max moment acting on a bracket by applying the force at 0.35*L from that bracket, not by applying it at 0.5*L. or maybe I'm just tired and need to go home

 

[PerKr]

Just to keep the thread somewhat updated...

Having tried a number of different load cases and restraints, I have a few conclusions:

1) The bracket can not be considered to be rigidly fixed to both the door and the handle for the analysis. If this was the case, I would be breaking brackets all day long.

2) We have both a force and a moment from the handle (as the stress concentrations show when comparing the analysis to broken brackets).

3) The effect of the moment is lessened by the method of connecting the bracket to the door and to the handle. I don't know by how much though...

4) "contact virtual part" seems to be the best solution for simulating the screws and other parts keeping the bracket in position on the door (other alternatives I've tried tend to result in reaction forces in the opposite direction of what I expected)

5) I have found pores in our zinc brackets and considering the real-world experiences and test results so far (the aluminum brackets seem to be ok) something is not right about them. If it was simply a design error (I'm not saying the design couldn't be better) I would expect more brackets to fail, but it seems very random.

6) I have resorted to using linear elements as opposed to parabolic elements as my computer apparently isn't optimal for this.

 

[johnhors]

PerKr,

On your point 6), linear four node tetrahedral elements should NEVER be used ! They are simply not good enough, any results you get will be seriously inaccurate. You have no choice but to acquire a better computer.

 

[PerKr]

johnhors: not sure I can get a better computer. I could try to avoid using too small elements in combination with too many virtual parts though and see if that helps.