ABAQUS Example | 2D Concrete Beam (Concrete Damage Plasticity)
ฝัง
- เผยแพร่เมื่อ 15 ก.ค. 2024
- ABAQUS Example | 2D Concrete Beam (Concrete Damage Plasticity)
Thanks for Watching :)
Contents:
Introduction: (0:00)
Part Module: (1:44)
Property Module: (4:01)
Assembly Module: (18:46)
Step Module: (20:58)
Boundary Conditions/Interaction Module: (22:10)
Load Module: (28:05)
Mesh Module: (30:31)
Embedding the Rebar: (31:55)
Analysis: (34:04)
Hi Dr Clayton Pettit, is there any plan to provide a lecture explaining the derivation of the concrete plasticity parameters in CDPM? I hope you can do that, it would be very helpful for us. Thank you
Hello Dr. Clayton Pettit, I tried to follow your instructions on modeling this 2D concrete Beam. I get the same warnings and error, but the body did not deform in the results section and there were no stress values or contours. Can I please get your support?
I use abaqus version 17 and am trying to model a simply supported beam and always getting analysis aborted due to error, it's so frustrating
Can I add fly ash material property for 5% replacement
Good day Sir, how do I add stirrup along the rebars in 2D modelling? since the stirrups surround the rebars, I wonder if thats possible
Great question! If you are only concerned with shear resistance mechanisms, you can add stirrups as truss/beam elements in the same manner as the longitudinal reinforcement (just define the cross-sectional of the element to match the total vertical cross-sectional area of the stirrup - e.g. if we have a 2-leg stirrup with each leg having 100mm^2, define the cross-sectional area of the element as 200mm^2). I also recommend using the linear patter command adding stirrups to the assembly as all you will need to do is place a single stirrup then duplicate it by specifying the stirrup spacing. Now again this is solely if you are investigating shear mechanisms, if you are looking at more complex aspects such as confinement where the stirrup loop will impact the behaviour, you will have to switch to a 3D model (remember that 2D models essentially assume the behaviour in the 'thickness' direction is constant or negligible). The process of adding reinforcement in 3D however is identical as you can create the stirrup as a beam or truss wire, add it to the overall model in the assembly tab, then embed it into the beam using the same constraint procedure :) I hope this helps :P I plane to do a 3D concrete beam video later when I have time :)
When you will be doing this
1. Create Part “Concrete Beam” (2D Planar), deformable shell
2. Create Part “Steel Rebar” (2D Planar), deformable wire
3. Edit Steel Material
a. ElasticYoung’s Modulus 200000, Poisson’s Ratio 0.3
b. Plastic Yield Stress 400, Plastic Strain 0
4. Concrete Material
a. Elastic Young’s Modulus (f”c*2/sigma_p), 0.15 (varies)
b. Plasticity -> Concrete Damaged Plasticity (There are others)
i. Plasticity Tab... concrete does not conform to associated flow rule; it behaves more like a soil
1. Dilation Angle 30 eccentricity 0.1 typical
2. Fb0/fc0 is ratio of biaxial strength of concrete to uniaxial strength of concrete. Biaxial strength is stronger. Typical parameter is 1.16
3. K is relation between tension strength and compression strength in concrete. Typical is 0.666 for low confinement concrete (will likely change based on CSA)
4. Viscosity Parameter of 0 is the most accurate. Typically 0.0001 is used for accuracy
ii. Compressive Behaviour
1. Yield Stress and Inelastic strain. Inelastic strain = strain - stress/Ec. Prof used hognestad model
2.
3. Copies “yield stress vs inelastic strain” into ABAQUS compressive behaviour
a. Replaces stress at which inelastic strain starts at beginning
4. Uses modulus of rupture as yield stress, at cracking strain of 0
5. Adds stress and strain for after gradual degradation. For convergence, takes 10% of yield stress and 5x the original cracking strain, rather than 0.1 and 0000001.
c. Apply materials to parts
i. Create section “Rebar”. Beam -> Truss -> Steel (Add cross-sectional area)
ii. Create section “Concrete”. Solid -> Homogeneous -> Concrete -> Add beam thickness
d. Assign sections
5. Assembly
a. Create instance
i. Click concrete, then apply
ii. Click steel with auto-offset, then apply
b. Create sets
i. “Concrete”. Click concrete
ii. “Rebar”. Click rebar
c. Move rebar
i. Click set “rebar”
ii. Click translate instance.
iii. Select point. Move to be certain cover from bottom of concrete beam
6. Step
a. Create step “Applied load” (Static General)
b. Turn on automatic stabilization with defaults “specified dissipated enegy fraction
c. Increment changed to 5000
d. Increment initial to 0.01, min=1E-10, max=0.1
7. Create support parts (since points will cause stress concentrations at nodes)
a. Create part, 2d planar, analytical rigid
b. Arc starting at 0,0 with certain radius
c. Assembly -> Create instance -> Support -> Apply -> Support -> Apply
d. Translate instances
8. Interactions
a. Create reference point -> click centres of two supports
b. Create constraint named “Left Support” “Rigid body”. Select reference point and type “analytical surface”. Select side by concrete beam as support side
c. Repeat for right support
d. Create interaction properties -> Contact -> Mechanical -> Tangential “Frictionless” and normal as “hard-contact”
e. Create interaction in “Initial Step”. Named “left support”, surface-to-surface contact. Master and slave surface
9. Load
a. Apply Load Step
b. Set Pressure Load. Top of beam, set as 1 MPa
c. Change F-Output-1 and H-Output-1 frequency to every x units of time 0.01
10. Mesh
a. Mesh -> Concrete Beam -> Seed it -> Element type -> Plane stress linear non reduced integration
b. Mesh -> Steel Rebar -> Seed it -> Element type -> Truss
11. Create constraint between concrete and rebar
a. Create constraint -> Embedded region -> Click rebar set -> Click host region -> Click concrete set
12. Create boundary conditions -> Click RP1 and RP2 -> Fix against rotation and displacement
13. Create job “CBAnalysis” and submit job
hi, if i wont this file?
Plc its 3d model
Hello can i get excel for concrete material property