Moment Calculation from Given Stress on Plate Element

[engamaid]

Hallo everyone,

I have run Beam as 2D plate on SAP2000, and have got the output as attached file. which gives me stress but i need to calculate the amount of moment at peak points so how can i calculate Moment from this stress at the point?

Regards,
Amaid

 

[KootK]

You, or the software, would need to integrate [stress x lever arm] over the cross section to arrive at the cross section moment. Normally, moment is calculated using 1D frame element (stick) models which makes the reporting of moments straight forward. What has led you to create a 2D FEM model here?

I like to debate structural engineering theory -- a lot. If I challenge you on something, know that I'm doing so because I respect your opinion enough to either change it or adopt it.

 

[engamaid]

this is the plate model of a beam incorporating connection where we have interaction of different materials like, column, beam, screed, and reinforcement at connection and we need to study the moment occuring at this point of -ve moment when we define all properties respectively and compare this moment with the one that can easily be calculated by line model, which is already done so.
i hope i clear the my question
so now cominng back to the answer, so could u elaborate what is means (Integrate stress x lever arm, over the x-section?
thanks

 

[KootK]

so now cominng back to the answer, so could u elaborate what is means (Integrate stress x lever arm, over the x-section?

1) Strip out any stresses due to axial loads.
2) Divide section up into a bunch of little areas.
3) Find the stress on each little area.
4) Find the distance from the centroid of each little to the reference axis.
5) Calculate the moment of each little area bout the reference axis as [area x stress x distance]
6) Add up all of the moment contributions from #4.


I like to debate structural engineering theory -- a lot. If I challenge you on something, know that I'm doing so because I respect your opinion enough to either change it or adopt it.

 

[engamaid]

1) the loads are verticle not axial,
2) division of section means meshing? that i have already done as am doing FEM
3) finding stress on each little area means, meshing again? okay i have stress in every square,
4) Reference axis?, considering that this plate model is for beam therefore by reference axis do u mean beam top at support in case of region for -ve moment??
5) got this point
6) moment contributed from point 5 not 4 if am wrong please correct, but have mention 4 instead of 5

THanks

 

[KootK]

Responding to your list:

1) You don't need axial loads to get axial stress. Think membrane action etc. There's a simple way to find out though. Just add up all of your cross section axial stresses and see if they sum to zero. If they don't, you've got some axial only stresses in there.

2) Division means looking at all of your stresses over whatever areas are convenient for you for calculation purposes. If that's just your FEM grid, then so be it.

3) Same as #2.

4) You need to figure out your moments about some reference axis in space. As long as you've stripped out any axial load only effects, you should get the same moment regardless of the reference point/axis that you select.

6) Agreed.

I like to debate structural engineering theory -- a lot. If I challenge you on something, know that I'm doing so because I respect your opinion enough to either change it or adopt it.

 

[engamaid]

okay one question, what will be my lever arm in this plate case? i mean for example i am checking stress box close to bottom for +ve moment then is my Y is from center of that particular box to bottom or from the centroid of the beam?

 

[KootK]

Your lever arm should be the distance from whatever reference axis you select.

I like to debate structural engineering theory -- a lot. If I challenge you on something, know that I'm doing so because I respect your opinion enough to either change it or adopt it.

 

[engamaid]

Reference point or reference axis?
i mean refernce point means from center or top or bottom but when u say reference axis i am kinna confuse because which axis i need to take i already know but for that lever arm for example if ai am checking moment at the bottom of beam then does it means my lever arm is from the center of the area i am checking moment at till the bottom most?
thanks

 

[BAretired]

Perhaps I am missing something, but if there are no axial forces, why isn't the stress at the top equal but opposite in sign to the stress at the bottom of the plate?

In any case, if the stress has linear distribution from top to bottom, the moment can be calculated from the difference between stress at top and stress at bottom.

Ordinarily, f = My/I where f is the stress, M is the applied moment, y is the distance from the centroid to the point in question and I is the moment of inertia of the plate. Given the stress at any point top and bottom, M = (f_t-f_b)I/2y. If y is taken as t/2 this reduces to (f_t-f_b)/I where f_t and f_b represent stress at top and bottom of plate respectively.

Of course, if the plate has been stressed beyond the elastic limit, the above method will not work.



BA

 

[rb1957]

SAP seems to "suck" if it won't tell you the internal loads in the elements (and only tells you the stress due to those loads).

another day in paradise, or is paradise one day closer ?

 

[KootK]

okay one question, what will be my lever arm in this plate case?

If your axial only stresses are stripped out, or not present to begin with, the reference point/axis will be arbitrary. You'll get the same value for the moment on the cross section regardless of where you take your reference point/axis. The process that I'me envisioning here is as follows:

1) FEM produces cross section stresses.
2) You or the software integrate the stresses into a cross section moment as we've been discussing.
3) You use the cross section moments to design and detail flexural reinforcing.

i mean for example i am checking stress box close to bottom for +ve moment then is my Y is from center of that particular box to bottom or from the centroid of the beam?

Per the process described above, this wouldn't make any sense. There's no "moment at the bottom" or "moment at the top". There's just the singular moment on the overall cross section. With that in hand, you'd switch to conventional reinforced concrete design assuming cracked concrete and a plastified section at ultimate capacity.

SAP seems to "suck" if it won't tell you the internal loads in the elements (and only tells you the stress due to those loads).

Agreed. Frankly, I'd be shocked if there isn't some way for SAP to report the aggregated cross sectional actions. Certainly, CSI SAFE can do that.

I like to debate structural engineering theory -- a lot. If I challenge you on something, know that I'm doing so because I respect your opinion enough to either change it or adopt it.

 

[BAretired]

Stress should vary linearly from a maximum tension on one edge to a maximum compression on the opposite edge. The neutral axis is at the middle of the plate where stress is zero.

The output file indicates that stress is positive (tension) in all locations which suggests to me that the output file is wrong.

BA

 

[engamaid]

hello guys thanks alot for your replies it waa a great help,
@BAretrued; so in case of nonlinearity what will be the method for calculating moment from stess??
thanks

 

[BAretired]

In the case of nonlinearity, you would need to know the stress profile between top and bottom of the plate. Then you could calculate moment as the sum of stress times area (force) times distance to the neutral axis. The upper limit would be the plastic moment capacity of the plate or Z.Fy where Z is the plastic modulus of the plate and Fy is the yield stress.

BA

 

[rb1957]

what stress (normal stress, principal stress, von Mises stress) is plotted on your first pic ? with a minimum stress of zero you've washed out the compression side.

Is this FEA non-linear ? or linear ?? if linear, then the high stresses are exaggerated 'cause the FEA doesn't appreciate yielding. but you could still use the stress profile to calculate a moment on the section (plot the stress across the thickness). If the stresses are real, then the FEA is saying you're in the process of developing a plastic hinge.

another day in paradise, or is paradise one day closer ?

 

[SAIL3]

not familiar with SAP pl elements so the following comment may be irrelevent....I would expect pl elements to develop membrane stress or in-plane tensile or compressive stresses which may be distorting the results....