Ultimate strength determination of box girder

[mon1299]

HI Everyone,
I am modeling a steel box beam with shell181.Beam is subjected to two point vertical loading which will produce constant moment region in the middle of beam.I want to know the utimate load carrying capacity of the beam. As the thickness of beam is very less like .0451in,it will be subjected to local buckling.Material properties are E=29000ksi, Yield stress:50ksi. I am considering bilinear isotopic material model asuming Et=0 and von misses yield criteria.I am doing large deflection analysis with stress stiffness option on. I want to know the ultimate strengh of beam. I tried with applying arbitary displacement at the location of load and monitored the midspan node vertical deflection.After some time I am getting increased deflection with less load. I thought that this load is the ultimate srength of beam. But I am surprised that this load is 20% higher than the actual test result which is impossible. Is there anyone who can help me? I realy want to know wheather my procedure is right or wrong?Shall I have to define any failure criteria for this? By the way in he middle of analysis I got warning message " small slver equation pivot terms" but still the analysis was running and converged for several time steps.
Is there anyone who can help me? I am really stucked with this problem for long time..
Thanks
Mon

 

[SKJoe]

Hi,

Can you provide some more informanion ? Did you use full N-R, or arc-lenth ? - I read that arc-lenth is more suitable when you use displacements as loading (not sure, check that). Do you fully understand this process of solving in Ansys ? The substep 999999 is not the last converged step, but it is the one before. Did you create full model, or only a half or a quarter ? Did you make some tensile srenght tests of material for each thicknesses ? If The thicknesses of the plates are very small ressidual stresses due to welding were not important ? geometrical imperfections measured/included to model ? Was the deformation the same as by test ?

Regards,
Lubo

 

[mon1299]

HI,
Thaknks for your reply.yah I know that 999999 is not the right result.I tried both newton raphson and arc length method. Both are giving almost the same result. I also tried applying displacemnt instead of load. But the result doesnt vary a lot.I create half model with symmetric boundary condition provided by ansys.Yah, for each thickness tensile strength test were done and yield stress value from that test are using in the material property.Yah you are right, residual stresses and geometric imperfection have influence on the capacity of the beam.But as it is a flexural member, I think imperfection will not a big factor. I am not considering these two factors. And I also dont know how to incorporate residual stresses and geometric imperfection. By the way the box beam is created by two C sections face to face and connected by self drilling screw along their top and bottom flange.I am not modelling the screw because there are total 24 screws along top and bottom. I coupled DOF ux,uy and uz at the bolt location.Material property and thickness are also different for two C sections.The load deflection curve initially can follow the same trend like test and also value. But after some time the FEM model behave more stiff than test model because the ultimate load is higher than the test load a lot, but the mid span deflection is almost same.One thing I want to mention that I am giving the yeild strength and Et=0 with BISO. When I checked Von misses yield stress for node, I found some elements have stress higher than the yield strength for material with low yield stress.The highest von misses stress is almost equal to the highest yeild stress of these two material.I cant understand why these things happening.I think I answered all of your question. If you want I can send my model also.Hope these can help you to understand the problem Please help me if you can.
Thanks
Mon

 

[SKJoe]

Hi,

How configuration of bearing was used in the model and by the test ? Was bearing modeled correctly according to test ? I presume that by the test the beam was put on roller bearings on both ends, right ? If it so then only a quarter of the beam could be modeled. Your model is supported on both ends only in vertical direction, or on one end you applied horizontal constraint as well ? You metioned that, you used coupling...did you ment CP ? If it so CP can not be used with nonlinear analyse. And why only ux,uy and uz ? Shell181 have 6 dof for each node. I think you can use nummrg,node,,,,low command instead by selecting only coincident nodes in bolt location.

Regards,
Lubo

 

[mon1299]

Hi Lubo,
Thanks for reply.I am modelling the section along the mid plane. So actually between the two sections there are little bit gap. When I consider the thickness of the shell then they will be perfectly in contact. So I cant use NMURGE as I think. So I tried CP. I also tried with connecting the two nodes directly by link8 elements. But the ultimate result is more or less same. Now about the support condition. Yah you are right. I am constraining the end only in the vertical direction. But inorder to restarin the lateral movement of the beam, in the experiment they provided lateral support at two ends and also 1/4th point both top and bottom flange. So I am restaining ux=0 in the middle node of top and bottom flange at those locations.So I think support condition is ok. Is there any way I can define that the material von misses stress cannot exceed the yeild stress as one material von misses is greater than that? Or can I restrict the plastic strain to a certain value?
Thanks again for your concern.
Regards
Mon