FEA - result validation 1

[amorphous]

Hello Group,

I have a frame 24,000 lbs hung over two jigs aproximately 400" apart. I am trying to analyse the job in ansys and the results I am getting are rediculous (I think). Please see the attached .pdf file to understand the problem better and results from ansys. As the jigs are equally spaced from the frame CG, I am analysing Just one jig. I am applying 24,000/2=12,000 lbs as a remote load at 200" from the load application center. The stresses in the support are very very high. I am using 50 ksi steel plates and 45 ksi tubes. These two jigs are in service for long time and still working good. If stresses in my calculation are correct this jig would have broken first time the frame is hung on it and which is not the case.
Do you think I am doing anything wrong in applying load???
Any suggestions would be great of help.

Thank you all....

 

[GregLocock]

Well, what do your hand calcs give you?

Cheers

Greg Locock


New here? Try reading these, they might help FAQ731-376

http://eng-tips.com/market.cfm?

 

[GregLocock]

Incidentally, unless the thing in the middle you couldn't be bothered to model is made of bubblegum, no, I don't think that is a very good model of what is going on at all.

Cheers

Greg Locock


New here? Try reading these, they might help FAQ731-376

http://eng-tips.com/market.cfm?

 

[rb1957]

it looks like you've modelled 1/2 the frame, which is ok; but what boundary condition have you applied at the break ?

 

[patswfc]

Looks like no supports at the end thus its acting as a cantilever beam and not a single/continuous? span beam

 

[rb1957]

exactly ...

 

[Twoballcane]

I am not allowed to open files on line, but are you sure you are not seeing singularities? Refine your mesh to see if the stress comes down. But, as GregLock has posted, what does your hand calcs come out to? You should be correlating between your hand calcs and FEA. For hand calcs, keep in mind if you are basing your results in VM stress in FEA, you have to do your hand calcs in VM to make sure you are comparing apples to apples. And also, if you are using failure theories, you have to compare the VM to yield and ultimate stress of the material.



Tobalcane
"If you avoid failure, you also avoid success."
“Luck is where preparation meets opportunity”
"People get promoted when they provide value and when they build great relationships"

 

[rb1957]

it looks like he's "just" cut the structure into two, and didn't provide the correct boundary condition at the cut

 

[GregLocock]

2BC= basically he's modelled the situation as a hangman's gibbet, when the real structure more closely resembles two upright poles with a beam laid across them. Consequently he is seeing cantilever root stresses associated with a 12000 lb *200" arm, instead of 12000 lb*6 inches or so.

Quite why in this day and age anyone relies on dodgy symmetry assumptions is a bit of a mystery to me, perhaps his screen isn't wide enough for the full structure.

Cheers

Greg Locock


New here? Try reading these, they might help FAQ731-376

http://eng-tips.com/market.cfm?

 

[crisb]

I can't see anything in the original post to suggest this was modelled with symmetry. In fact it might be difficult to hang the piece on it if each jig had two legs. I think the problem is you are applying the load 200" from the jig, whereas the piece will be relatively rigid. It would be more realistic to apply the load close to or at the centreline of the jig.

 

[rb1957]

"I am analysing Just one jig. I am applying 24,000/2=12,000 lbs as a remote load at 200" from the load application center"

the model pix look like 1/2 of the full frame sketch.

 

[mmar2087]

I agree with crisb, a force applied at the centerline of the jig would be more accurate (or a simple P/A). The hangman's gibbet is a good analogy and the stress gets very high due to the unrealistic twisting of the tube. Look at the deformed result and this should be obvious. (the red areas on the short sides of the tube gives a hint in your stress picture)