Skip to main content
L
lfox1-Visitor
1-Visitor
July 6, 2015
Solved

Spreader Beam Analysis

  • July 6, 2015
  • 3 replies
  • 7152 views

I am having trouble getting believable results from simulate while analyzing a simple spreader beam.

I am new to simulate, so I don't know if I am constraining and/or loading it correctly. Any advise would be appreciated.

The beam is very simple. It is just a piece of 1" thick plate 147" long by 12" wide with 1-3/8" holes spaced 6" apart along both long edges for rigging.

2 pieces of 2" x 4" x 1/4" rectangular tubing will be welded to the sides for torsional support. See attached picture for a visual.

For the worst case scenario, the beam is to be picked at the top center hole with the load hung from the two outer most bottom holes.

It needs to hold 25,000 lbs, but so far my results have shown that it will not. Not even close. I don't believe these results because the man who suggested the design has been rigging for decades and would build this thing and use it without a second thought. I've been messing with constraints and loads - what kind to use, how to apply them, etc. Half of my attempts fail with "not enough constraints", and the ones that succeed show outlandish stresses over very small areas around the circumference of the holes. Pin constraints and bearing loads make the most sense to me for this, but I'm just not getting results. How do you do this?

And yes, all of my material properties are in good order.

Thanks, Luke


This thread is inactive and closed by the PTC Community Management Team. If you would like to provide a reply and re-open this thread, please notify the moderator and reference the thread. You may also use "Start a topic" button to ask a new question. Please be sure to include what version of the PTC product you are using so another community member knowledgeable about your version may be able to assist.
Best answer by 346gnu

Lucas,

You will get high stresses around all the holes. These are all stress raisers by an unscientific factor of 3-ish.

1. Do a hand calc to get max stress in outer fibre at centre support and approx. deflection of the ends

Assume half the beam is a built in cantilever, ignore the holes.

Suppress the holes (other than those required for loads and constraints). This will show whether your FEA is in the same ball park or whether something is very wrong.

2. The section is symmetric, you could use a sketched beam section and try beam elements. This is another quick and simple way of confirming hand calc/solid model is in the correct ball park.

3. Multiply the stress at the hole outer edge distance from the neutral axis by the unscientific factor. (Peterson's is more scientific) and compare with the solid model.

The above offers confidence but not refinement.

If you have a pin constraint in the centre with the rotation DOF set as free and an equal load at each end, then your model will tip like a see-saw and fail insufficiently constrained. This is a numerical method.

I would propose you consider a 'weak' ground spring at one end. Any numerical imbalance will be carried by this spring.

Your hand calc will tell you approx. how much deflection to expect. The spring should not exert more than say 1% of the applied load in the direction of the load at that end when fully deflected.

There are other methods for another day.

Regards

3 replies

L
lfox1-VisitorAuthor
1-Visitor
July 6, 2015

After digging further into my material properties, I am concerned. I opened up the text file for my steel plate material which was created long ago and not by me. The numbers would be correct if the units were in psi. Young's modulus for example is 2.9e7. However the units are in lbm/(in sec^2). I've been looking into this unit that Creo seems to use extensively, and I do not understand it. Is it the same thing as lbf/in^2 in which case the Young's modulus would be correct? Why is it presented in this way? I'm not feeling like a very good engineer today. I need to understand this stuff. Thanks for any help!!

3
346gnu13-Aquamarine
13-Aquamarine
July 6, 2015

Lucas,

Create a 1x1x1 cube.

Ensure that you are conscious of your model units (know where you are).

Assign your material.

Check the mass props and the numbers/units in the material definition form.

Note, you can enter material property numbers in any unit system by the drop down lists regardless of model units.

The software will perform the appropriate conversion behind the scenes.

Make sure it makes sense.

It is possible and interesting to look at and edit the info in the .mat files. Don't. Carry out this exercise via the UI being aware of your units from the pull down lists (defaults to you model units).

Regards

3
346gnu13-AquamarineAnswer
13-Aquamarine
July 6, 2015

Lucas,

You will get high stresses around all the holes. These are all stress raisers by an unscientific factor of 3-ish.

1. Do a hand calc to get max stress in outer fibre at centre support and approx. deflection of the ends

Assume half the beam is a built in cantilever, ignore the holes.

Suppress the holes (other than those required for loads and constraints). This will show whether your FEA is in the same ball park or whether something is very wrong.

2. The section is symmetric, you could use a sketched beam section and try beam elements. This is another quick and simple way of confirming hand calc/solid model is in the correct ball park.

3. Multiply the stress at the hole outer edge distance from the neutral axis by the unscientific factor. (Peterson's is more scientific) and compare with the solid model.

The above offers confidence but not refinement.

If you have a pin constraint in the centre with the rotation DOF set as free and an equal load at each end, then your model will tip like a see-saw and fail insufficiently constrained. This is a numerical method.

I would propose you consider a 'weak' ground spring at one end. Any numerical imbalance will be carried by this spring.

Your hand calc will tell you approx. how much deflection to expect. The spring should not exert more than say 1% of the applied load in the direction of the load at that end when fully deflected.

There are other methods for another day.

Regards

L
lfox1-VisitorAuthor
1-Visitor
July 6, 2015

Charles,

Thank you for your reply. I've moved on to another more urgent project for the time being, but I'll be back to try your suggestions in a day or two. I might have to dig out a text book to do stress and deflection hand calcs. It's been a long time, and that was never my specific area of study.

Thanks again and I'll get back to you,

Luke

L
lfox1-VisitorAuthor
1-Visitor
July 7, 2015

Thanks everyone for the advice. I was able to get results I'm comfortable with. I am eliminating the three center holes on top and bottom to assure that the beam is always picked in two places. This alleviates some of the shear stress on the pick points. Creo still wants to give me high stresses over small areas on the circumference of the pinned holes, but I'm not seeing the same effect on the load bearing holes, and my hand calcs are giving the holes more than enough safety factor. If anyone has experience with designing rigging, I'd love to know if you see the same thing, or if you have a preferred way to constrain a free hanging spreader beam such as this.

Thanks, Lukespreader beam3.JPG

spreader beam2.JPG

U
unickque1-Visitor
1-Visitor
July 8, 2015

Stresses always tend to get high near constrained points or areas.

What you can do in this case is do one analysis with constraints on the top holes and bearing forces on the bottom holes, and then do a second analysis with the constraints on the bottom holes and the bearing forces on the top holes.

Terms & ConditionsAccessibility statement