roll bending
Altair Employeehi
i am doing simulation on 3 point roll bending in radioss solver
first step i applied displacement to the top roller in z direction then i applied peripheral velocity to 3 rolls then i stopped the velocity again applied top roller displacement and given velocity of the roll in different direction.
i am not getting the plastic strain value while the stress i am getting larger than then the yield value 
Answers
-
i used the material M36PLAS_TAB
0 -
Hi,
the issue is with the stress-strain curve: the first point of yield stress functions (plastic strain vs stress) should have a plastic strain value of zero at yield stress. In your case, the first s-s set should be 0 plastic strain at 152 stress (the second 0.002481 plastic strain at 228 stress and so on), while the linear elastic part is described by E parameter= 190000 (Young's modulus).
0 -
Hi ivan
Thanks for your reply i have made the changes for the stress strain curve that 0 strain is at the yield point of the material and the curve progresses as mentioned below. even though i am not getting plastic strain value.
<?xml version="1.0" encoding="UTF-8"?>
<?xml version="1.0" encoding="UTF-8"?>
0 -
You should subtract the elastic strain (0.000799994) to get only plastic strains. So the table should be:
0 @ 152
0.002481 @ 228
and so on
It is odd the plastic strain is not visible- can you share the model?
Attached is an example of law 36 with plastic strain.
0 -
Hi ivan
Sorry for late reply
i attached file please check.
0 -
The issue was with solid property parameter Isolid=12, which is an obsolete standard 8-node solid, full integration (no hourglass). Use Isolid =17 (H8C) or 24 (HEPH) instead.
I have edited stress-strain curve and set up advanced mass scaling to speed up computation.
0 -
thanks ivan
i am using older version v14 can u share me the .rad file please
0 -
sorry about that
0 -
thank you so much ivan
in 3 roll bending simulation can we do the simulation in stage wise (i.e) first step the top roller is moved down that boundary condition is specified for this stage and second stage rotation of rolls now boundary condition is differ from first stage
what is multi stage process in hyperform is that helpful for my case?????
i need to consider the spring back also
0 -
It is possible to carry out simulation in stages. There are various possibilities:
-most boundary conditions can be switched on/off through Tstart/Tstop parameter
-contacts can also be switched on/off (Tstart/Tstop parameter)
-rigid bodies can be activated or deactivated with a sensor or with the options /RBODY/ON and /RBODY/OFF in the Engine files
-multiple engine files can be defined with different simulation controls
I am not (yet) familiar multi-stage process in Hyperform so I can't comment on that. But given HF uses Radioss solver it should be possible to set up a similar simulation.
Check Example 24 – Spring-back:
http://altairuniversity.com/wp-content/uploads/2012/08/Example_25.pdf
0 -
hi ivan
can u explain me briefly about Tstart/Tstop parameter
i need to fully constrain the plate at the specific time i have created constrain for this as in the image is that an appropriate way. when i am running this i am getting the warning as a incompatible kinematic condition and it simulated is get stopped.
thanks
<?xml version="1.0" encoding="UTF-8"?>
0 -
Tstart/Tstop parameters on /BCS card are used for /INTER/TYPE21 mapping, so it will not switch on/off boundary condition.
To release DOFs, you need to use BCSR/TRA, BCSR/ROT engine cards. Please go through following examples, where this functionality is used:
RD-E: 4200 Rubber Ring: Crush and Slide
RD-E: 5501 Fan Blade Rotation Initialization
0 -
hi ivan
is type 21 is for shell element in type21 unable to select the slave as brick element
for arresting the dof's i try one method
i created an second engine file to arrest DOF's of the component at a specific time by adding these commands
/BCS/TRA/XYZ
node numbers
simulation get terminated because of mass error
releasing the dof's is fine works well is there any similar way for arresting the dof's
0 -
hi @Ivan
i am simulating the manufacturing process 3 roll bending process in radioss, early i used 3D model now i am trying with a 2D model, since plate thickness 3 mm
For that i extracted the midsurface of the plate and assign the thickness of the plate as 3mm. i used P1_shell ishell=24 N=5 thick=3 Istrain=1.
i assigned the material property to roll and plate, boundary condition, contact every thing as same.
shell is bending only in the region inside the rolls, region outside the roll is not bending i have marked in the image .
does i have used any shell parameters wrongly.
i having problem in imposed velocity also that the rotation of roller. the roller is not rotating in both the direction i have assigned negative sign(-) to change the direction of roller in curve editor.
i have attached my file pls check
thanks
0 -
Hi,
the region outside the roll is not bending because you had constrained the rotational DOFs of the plate. Only Y translations should be constrained so plate remains centered.
The shell formulation is correct- I would add Ithick=1 so thickness change is taken into account.
Note however the thickness (3mm) to length (10mm) ratio of plate elements is 0.3.
Thick shells are used when thickness to length ratio is between solid and thin shell recommended range:
When h/L is large, shear deformation is at its maximum importance and the user should use solid elements. When h/L is small, transverse shear deformation is not important and thin shell elements are the most effective choice.
The initial downward displacement of the top roller happens in 5ms. Such a rapid loading induces inertial effects, which might be unwanted if you are trying to simulate a quasistatic event.
The negative sign will reverse the rotation- check the model attached. If you have trouble visualizing rotation in HV, use Shaded elements and mesh lines view, hide just one element of roller, contour velocity or show undeformed shape in wireframe mode. Be careful when defining curves; when simulation goes outside the defined range it will extrapolate the slope- in your case the velocities would keep increasing after 155ms.
0 -
Hi @Ivan
thank you, its clear......
energy error% it is goes on increasing
CYCLE TIME TIME-STEP ELEMENT ERROR I-ENERGY K-ENERGY T K-ENERGY R EXT-WORK MAS.ERR
2447500 2985. 0.1239E-02 NODE 27 -89.9% 230.2 9.932 5.925 2448. 0.000
ANIMATION FILE: 2D_SHELL_A5972 WRITTEN
2448000 2986. 0.1239E-02 NODE 27 -90.0% 229.3 10.88 5.927 2449. 0.000
ANIMATION FILE: 2D_SHELL_A5973 WRITTEN
ANIMATION FILE: 2D_SHELL_A5974 WRITTEN
2448500 2987. 0.1239E-02 NODE 27 -90.0% 228.4 11.67 5.930 2450. 0.000
ANIMATION FILE: 2D_SHELL_A5975 WRITTEN
2449000 2987. 0.1239E-02 NODE 27 -90.0% 227.7 12.38 5.935 2450. 0.000
ANIMATION FILE: 2D_SHELL_A5976 WRITTEN
2449500 2988. 0.1239E-02 NODE 27 -90.0% 227.0 12.98 5.919 2451. 0.000
ANIMATION FILE: 2D_SHELL_A5977 WRITTEN
i didn't specify any mass scaling /DT/NODA/CST or /DT/AMS
0 -
Negative Energy Error represents energy dissipated from the system and this can be from many sources including plastic deformation and Hourglass energy.
If you have included coefficient of friction then the energy error is due to coefficient of friction which is justified. If this amount of energy error is there when no coefficient of friction is defined, then it may be a case of penetration which is problematic.
0 -
hi @Ivan
simulation works fine but the plate (2D shell model) is vibrating much. i have applied load gradually. what might be the issue in the model . refer the
video i have attached.
0 -
Hi,
The vibrations are due to loading being applied using step (jagged) functions. If we differentiate the displacement and velocity functions we get high accelerations leading to large forces and vibrations. To avoid vibrations the functions should be smooth and/or Dynamic relaxation (/DYREL) or Rayleigh damping (/DAMP) could be used.
0 -
hi @ivan
thanks for your reply.
In Rayleigh damping (/DAMP) how to find the values of alpha & beta.
And if i apply the values for alpha and beta means the time step which i imposed through Advance Mass Scaling (/AMS) is not taken into consideration.The simulation runs on with the actual time step... What is the reason behind this issue.
0 -
The Rayleigh damping coefficients can be obtained experimentally or calculated (see attached) However, in practical applications they are estimated and adjusted based on engineering intuition. I got good results on some models using Beta=10 and leaving Alpha blank. Rayleigh damping will reduce the timestep so adjust timestep controls accordingly.
http://ejge.com/2003/Ppr0318/Ppr0318.pdf
https://www.researchgate.net/post/Any_suggestions_on_Rayleigh_damping_coefficients
0 -
hi @Ivan
i will do some iteration on this Rayleigh damping coefficient and lets u know if i had any difficulties.....
i having doubt in the spring back i used the implicit spring back option as mentioned in the example 25 but my results are not that much correlating .
In implicit spring back what kind of solver should we use in tutorial it mentioned /IMPL/SOLVER/2 but in the file which is mentioned in the tutorial DBEND_44 they mentioned /IMPL/SOLVER/1
i have attached the tutorial and file from tutorial for reference.
0 -
Hi,
you should first smooth the loading functions and only then reduce any remaining vibrations with damping.
I don't have enough experience with implicit spring back to be able to give useful advice.
0 -
hi,
if we use the damping for controlling the vibration in the plate, does it affect the spring back???
0 -
Springback results are sensitive to the magnitude of damping factor, especially when unphysically high damping is used.
Check the following papers for details:
https://www.sciencedirect.com/science/article/pii/S0924013604003577
https://www.sciencedirect.com/science/article/pii/S1000936113001751
0 -
thanks your reply i will read those journals.
i am having a doubt does MAT36 will used for the springback analysis??
0 -
In Example 24 – Spring-back Anisotropic elastoplastic Hill material model /MAT/LAW43 is used.
0 -
Hi @Ivan
i facing problem during running the job that my simulation remaining time is keep on increasing with error percentage. i attached the text file for reference. does the model have any issue in the contact??
i have attached my model file please check
0 -
Hi,
Looks like the contacts are causing the large negative energy error. But the root cause is the too high timestep imposed by AMS. First, run with DT/NODA mass scaling until you get reasonable negative energy (15%) and mass error (2%) throughout the simulation. Then set up the AMS run trying to hit the energy error % of DT/NODA run (as well as stress and displacements). Set the Iflag=2 and Nprint=1000 to output the number of iterations before the convergence of the conjugate gradient in the out file (less than 30 is good). There should be only a few cycles where INTER is controlling the timestep.
It is recommended to use Iform=2 with contact friction.
0
