Local Stress / Hot Spot / Stress Concentration??? problem

[amorphous]

Hello All,
I am a rookie to FEA world. I am using ANSYS14 to perform stress calcualtion on a steel structure. This is static analysis.

I have a 3" thick 50 grade steel plate solidly welded to the tubular structure behind. It takes a concentrated load of 5614 lbs and a large moment. The analysis show local stress/ hot spot of very high magnitude. I cannot eliminate this stress with any design modification as the load is acting on a small area (3/4" X 2" section).

See attached images for clear picture...

As you can see I do not have any problems else where in the frame as it is very thick plate and has 1" thick gussets.

Is this hot spot something to worry about? Can I ignore these peak stress as they are caused only in may 2" section and spread?

Any body encounter these peak stress? and how do you proceed in this situation?


Any help in this issue is greatly appreciated.

Thank you in advance
amorphous...

 

[SWComposites]

Have you applied the load over the 3/4" by 2" area or at a single node? If at a single node, try spreading it out over the actual area. What is the physical mechanism that is applying the load over the small area?

 

[inline6]

how have you applied the force and moment? how is the load applied in reality and what does the load represent?

it looks like you have shell and solid elements have these been connected appropriatelty and also the incompatible meshes have these been glued?

 

[amorphous]

SWComposites:
Yes, I have applied the load over 3/4" X 2" area. I have 10,000 lb force supported between two points. The current point is at 19.2" from the load, so it creates a load of 5614 lbs and a moment of 108080 lb-in. The other end is at 24.6" and is spread over large cross-section so I don't have no problems at the other end.
The nature of the support is such that I cannot increase the support area.

inline6:
Mesh has been created automatically by the program and they are all solid elements on the plate.

I would like to know is the local stresses created on the small area are dangerous? can I ignore them? or do I need change my design drastically in order to eliminate these peak stresses???

Thank you

 

[rb1957]

your picture isn't very clear to me.

it looks like you're applying a force and a torque to the beam.

i'm not sure you're answered the question posed ... are you applying loads to the minimum number of nodes ? is this loading real ? ... it might be, you might have a limited loadpath to transfer the load (ie a couple of bolts) or not (eg, a weld).
is the high stress near the load ?

the mesh may be automatically generated (using default settings) but the user should have control over it (to add mesh refinement in a critical area).

 

[amorphous]

rb1957:
I am sorry if the picture is not very clear and I thought I answered the posed question - I may not have clearly understood the question.

I am applying the load to the geometry. There are at least 8 nodes and 7 elements which take the load. I could refine the mesh and increase the number of nodes taking the load and that will increase local stress.

 

[Twoballcane]

Have you done some hand calcs yet? Did it correlate with the FEA? Due to company policy, I cannot open the file, but this sounds like you have singularity issues. Basically a few nodes in the area may be calculating un-realistic high stresses which can be ignored (or talked away as “local” plastic deformation). However, you will need to do the hand calcs to make that determination.

Tobalcane
"If you avoid failure, you also avoid success."
“Luck is where preparation meets opportunity”

 

[rb1957]

mea culpa ... only looked at the first pic.

how physically is the load being applied ? a discrete attachment ? or distributed ? are there fasteners involved, which have a finite stiffness (as opposed to an infinitely stiff model) ?

if you are truly applying a moment to the edge (as modelled) then yes expect a high stress. but i'd expect the moment to be applied at two (at least) locations, ie something like a couple.

 

[SWComposites]

if you are accurately modelling reality, then yes your high stresses probably will lead to premature failure.

since many of us question how the load is really applied - can you post some pictures of the actual structure / assembly?

 

[inline6]

do a hand calc for the Force use Sigman = P/A

for the moment use Sigma = M/Z (try assume Z= 2nd moment area of area which the moment is applied over in the model)

If this is a linear static analysis apply the force and moment seperate in FEA to see which causes the high stress. i suspect it is the moment and how it is applied in the model

how did you aplly the moment to the nodes of solid element?

 

[Twoballcane]

Actually I would calculate out to max principal stresses and then to Von Mises stresses so that you can use the failure theories. Just calculating the normal stress and moments will give you a partial picture.

Tobalcane
"If you avoid failure, you also avoid success."
“Luck is where preparation meets opportunity”

 

[jean15paul]

I 100% agree with the advice to do some hand calcs to validate your results. Assuming you hand calcs don't reveal a problem with your model, then I'd say you probably do have a real problem that you need to solve. If you're asking HOW to solve your problem, then I don't think anyone hear can give you an easy answer. This is why stress analysts get paid the big bucks!

I will try to pass along some advice. Generally we start with a simplified problem that makes some conservative assumptions. When you find a problem (like this may be) then you have to "sharpen your pencil" and do a more complex analysis to try to show it good. Here are some things that I'd start with:

* Is there any extra thickness in your part that isn't represented in your FEM? For example fillets?
* Can you push back on the load? Who derived the load? What did they assume? Are the loads applied realistically?
* Did you make any conservative assumptions with your material properties? For example did you assume welded properties everywhere when you really just have welds in local areas?
* Are your constraints and connections accurately modeled? Are you using overly stiff connections like rigid elements? Do you have constraints near your area of interest (i.e. the hotspot)?

I'm sure there are more assumption you may want to re-evaluate, but this is what came to me immediately. If you don't find anything to push back on then you may have to consider a different material or increase your thickness.

Good luck

 

[racookpe1978]

Looking at your pdf file, image pg 2 (from above the curved plate) and image 3 (below the curved plate) shows a point load 10,000 lbs and a large moment applied to a single place on the curved plate.

But - unless you are actually pushing in/pulling out on that specific little area as if with a hydraulic ram, or pulling on a welded arm at that point that is welded to the curved plate, that loading can't exist.

Or if your configuration does exist that way, yes, you have established that much force and that much moment at that position will deform the plate.

For example, assume that load and moment is your actual force. Then, you need to model (?) the hole you are attaching the lifting rig or weight causing the 10,000 lb force that is acting on the plate: where is the hook attached?
How is the beam causing the welded moment to be created attached to the curved plate?