Calculating safety factor on gear box support 2

[Muaath123]

Hello guys,

I want to calculate the safety factor on container support design of gear box and I need your tips

The actual mass = 1600 kg

I assumed the mass to be = 2500 kg
= 2500 X 9.8 = 24500 N

The material is Steel A36 (Structure Steel)

So, I choose static structure, performed the mesh and remote force (24500 N) to be applied in the center.

and the result is:

Total Deformation

Equivalent Stress

and the F.O.S equation will be:

F.O.S = max. strength / Design load
= 2500 (kg) / 668.73 (MPa)
= 3.73 > 1

I'm hope my calculation is right

Please if you have any tips or comment, share it with us

Thank you so much for your time

 

[aerostress82]

You need to check a previous similar analysis on this type of loading and structure (gear box).
And what do you mean by FOS equation?
Best action you can take now is to remove the force fron your model, apply a 9.8N/kg gravitational acceleration in the gravity direction. and check the von mises stress by dividing your Ftu (ultimate tensile material allowable) by the von mises stress you get from the analysis:
Ftu/vonmisesstress

This is what you are trying to achieve and you may be a atudent

Spaceship!!
Aerospace Engineer, M.Sc. / Aircraft Stress Engineer

 

[Muaath123]

Thank you for replying

No I'm not student, I'm mechanical engineer who is working as quality assurance for period of time, so I may forget some information about mechanical design

FOS is Factor of Safety

I'll try gravitational acceleration and post the result today

And where I can find similar analysis?

 

[Dave442]

You're predicting stresses above the yield stress of the material (~250 MPa).

For a static load, the factor of safety is ultimate stress / working stress. Not sure why you include mass? If you don't want your part to deform permanently, your ultimate stress should equal the yield stress. Then your factor of safety is 250/669 = 0.37.

This all assumes that your mesh is adequate and your loads/BC's are appropriate.

 

[Muaath123]

Thank you Dave for replying

 

[Muaath123]

Guys you are all right

I don't know why I divide the weight over max. stress

I saw a solved example from engineering design book and the weight was the same value as the yield stress, so I took it and it was totally OFF

and part of me was not sure about it and that's why I asked for your help.

Now,

I agree with you Dave >> Factor of Safety = ultimate stress / working stress = 250 / 668.72 = 0.37

What does that tells me? Is the design not safe at all? OR the load will cause permanent deformation and can be usable?

Because I copy the design of the finder (original Manufacturing) same design, material and thickness.

Also, in my company they used this support for long time without an issue (talking about more than 20 years)

but in short of the quantity, we're trying to fabricate a new one

So I'm waiting for your input guys

Thank you

 

[Dave442]

Hey,

According to google, the ultimate tensile stress for your material (steel a36) is 400-550 MPa. If you have full confidence in your FEA model (geometry, mesh, element formulation, constraints, loads, application of loads, solver controls, assumptions etc.) then your FEA results indicate that this device will fail in service.

In reality, this part has been used for a long time without issue. This suggests that there are issues with your FEA model and the 668.72 MPa peak stress that you are predicting is non-physical. This could be caused by any number of modelling assumptions/errors.

Before you trust your FEA results you need to perform some validation. Load the device in a lab and measure the deflection at a specific point. Repeat this test with an FEA model and see do you produce the same force-displacement. This will give you confidence in your FEA results (or confirm that your model has issues).

Good luck,
Dave

 

[Dave442]

I guess there are multiple things I would also check prior to attempting to validate your FEA model:
[ul]
[li]Check your dimensions are correct[/li]
[li]Check your geometry is discretized using an adequate number of elements[/li]
[li]Check your geometry is discretized using an adequate element formulation[/li]
[li]Check you have assigned an appropriate material model[/li]
[li]Check are the material parameters consistent with the assumed dimensions[/li]
[li]Check is the loading representative of that observed in reality[/li]
[li]Check is the loading consistent with the assumed dimensions[/li]
[li]Check are the constraints representative of those observed in reality[/li]
[li]Check is the type of solution you have used appropriate (static/dynamic etc.)[/li]
[li]Check influence of stabilization/damping if present[/li]
[li]Check for post-processing errors[/li]
[/ul]
Dave

 

[cowski]

In addition to the static load (weight) of the gear box, don't forget to check the dynamic load. A torque will be applied to the gearbox when it is in use which may/will add to the load on your support frame.

 

[Muaath123]

I checked for the analysis again

The assumed weight I think is much higher (2500 kg)

In the Technical Manuel the gear box weight is 1117 kg

So I will assumed 1400 kg (The whole weight of the container + Support + Gear Box = 1400 kg per to TM)

So, The results are:

Factor of Safety = 250/231.11 = 1.08

and the max. working stress on this spot:

In reality it will stand on rubber absorber base which its size is twice bigger than the hole size

so maybe the max point are nonphysical.

What do you think?

 

[Dave442]

Hi again,

Its hard to comment on your results without knowing all the details of your model. One thing I would suggest is to run a mesh sensitivity study. From your images your mesh/contours look quite coarse. It looks like your primary loading mode is bending and you only have 2 elements through the thickness of the member with the peak deflection. Depending on the element formulation you have used, more elements may be required in this region to adequately capture bending effects. Also, I would try to perform some validation.

Good Luck,
Dave