Beam vs Solid - Plastcity 1

[marmilew]

Hello all

I model a simply supported beam with uniform pressure and rectangular cross-section. I use bilinear isotropic hardening model (Et=0) There are two cases:

1st case: to achieve elastic limit (load q=8*sigma_y*(bh^2/6)/L^2)

2nd case: plastic hinge, q=8*simga_y*(bh^2/4)/L^2

For solid model I achieve almost perfect results, and equivalent stress is only a bit bigger than yield stress (FE error i assume).

However, for the beam-model the the plastic-loading gives me stresses 150% bigger than yield stress!! For the 1st case sequential stress is almost yiled stress, but for 2nd case is 150% bigger than yield stress.

It looks like beam-model don't 'see' my bi linear hardening model but simple liner-elastic..

 

[rickfischer51]

Are you doing this in Workbench or MAPDL? Which beam and solid elements are you using?

If your beam results are wrong, consider the following. First, the solid model gets it's section properties implicitly from the solid geometry, but the geometry for a beam is a one dimensional stick, so you have to put in section data. Is the section data correct? the brick elements have three degrees of freedom, but the beans have six. Have your applied your boundary conditions correctly? If you are using a legacy beam formulation, does it support plasticity?

The current beam element is BEAM188, which gets it's section properties via the SECTYPE and SECDATA commands. I've never used this beam with a plastic material, but I checked the documentation and it looks like the SECTYPE command has beam types BEAM and GENB. GENB has subtypes ELASTIC and PLASTIC. Looks like your SECTYPE command should be SECTYPE,secid,GENB,PLASTIC.



Rick Fischer
Principal Engineer
Argonne National Laboratory

 

[petb]

Hi,

Apart from what Mr. Fisher already told you, plastic stress is evaluated at integration points and will be interpolated onto the nodes when you examine stresses. This can be, at leat when dealing with shell elements a little confusing, you'll find stresses well beyond the yield stress, not so sure about the beam elements in this regard though. I do believe they work the same way. Have you performed any mesh sensitivity analysis?

/PB

 

[marmilew]

Thank you rickfischer51 and petb for your answers.

I am working in a Workbench. I use default hex elements for solid and default beam elements for beam. However I 'midside nodes kept' option is on, so they are higher order elements.
I have checked boundary condition and section properties and they seem fine. Moreover, for the load within elastic range I get exact results so I think model is fine.

What I found in help module about beam188 element:
Linearized Stress

It is customary in beam design to employ components of axial stress that contribute to axial loads and bending in each direction separately; therefore, BEAM188 provides a linearized stress output as part of its SMISC output record, as indicated in the following definitions:

SDIR is the stress component due to axial load.

SDIR = Fx/A, where Fx is the axial load (SMISC quantities 1 and 14) and A is the area of the cross-section.

SByT and SByB are bending-stress components.

SByT = -Mz * ymax / Izz
SByB = -Mz * ymin / Izz
SBzT = My * zmax / Iyy
SBzB = My * zmin / Iyy


If I understand this correct, stress distribution is linearised so there is no way to represented nearly-plastic-hinge stress distribution. But it is also said that this element supports plasticity, so I am a bit confused right now. I can't imagine that software like ansys cannot represent plastic stress distribution.

 

[marmilew]

I think that the only way is to input an APDL command into WB. I tried but I am totally new to APDL. This is command in WB:

! Commands inserted into this file will be executed just after material definitions in /PREP7.
! The material number for this body is equal to the parameter "matid".

! Active UNIT system in Workbench when this object was created: Metric (mm, kg, N, s, mV, mA)
! NOTE: Any data that requires units (such as mass) is assumed to be in the consistent solver unit system.
! See Solving Units in the help system for more information.


sectype,1,genb,plastic ! Elasto-plastic response
bsax ,0.0000 ,0 ! Axial strain 0.0008, Force of 0
bsax ,0.0008 ,2e2 ! Axial strain 0.0008, Force of 200
bsax ,0.001 ,2.1e2 ! Axial strain 0.0008, Force of 210
bsax ,0.0014 ,2.12e2 ! Axial strain 0.001 , Force of 212
bsax ,0.01 ,2.15e2 ! Axial Strain 0.0014, Force of 213


Can you verify? After command WB returns error. It says that element 22 has zero stiffness.

 

[nodalDOF]

I am not sure about workbench but are you doing the same thing in the beam vs. solid element models?
Why are you using General beam section (SECTYPE,1,GENB,plastic)? How are ensuring that they have same geometrical properties? Did you check your solid and beam models have same moments and total element masses? why can't you use a simpler regular beam section with rectangular C/S defined using SECDATA and material properties separately?

You are saying that you used Bilinear-Isometric but your input in beam case looks multilinear-isotropic.

NodalDOF

 

[marmilew]

I have found out in HELP that there is no way that WB will show correct values of stress in beam elements in the elastic-plastic material. Tool used for display of stress value in beams (Beam tool>combined stress or beam tool>direct stress) is valid only in elastic range.
It looks like for plasticity in beams i must use APDL. Or model in WB and transfer to APDL afterwards.