B32 element with Dynamic displacement under gravity report an error

1

Hi ,every one
I am trying applying dynamic displacement on one end of a suspended beam under gravity,but I meet the error in the picture.

L%%(QVEUWJ~LPK~@BR@2K0
L%%(QVEUWJ~LPK~@BR@2K0840×163 16.9 KB

This is my file, I do not know how to solve it.Could you give me some advices? Thank you very much for your time!

*Amplitude, name=Amp-1
             0.,              0.,             0.1,        0.0000125581,             0.2,        0.0000250666          
*NODE, NSET=Nall
       1, -1.49012e-08,  0.00000e+00,  0.00000e+00 
       2,  1.00000e+00,  0.00000e+00,  0.00000e+00 
       3,  5.00000e-01,  0.00000e+00,  0.00000e+00 
       4,  2.00000e+00,  0.00000e+00,  0.00000e+00 
       5,  1.50000e+00,  0.00000e+00,  0.00000e+00 
*ELEMENT, TYPE=B32, ELSET=Eall
     1,      1,      3,      2
     2,      2,      5,      4
*BOUNDARY
1,1,6
4,1,6
*MATERIAL,NAME=EL1
*DENSITY
7850.
*ELASTIC
2100000.,.3
*ELSET,ELSET=SET1
1,2
*BEAM SECTION,ELSET=SET1,MATERIAL=EL1,SECTION=RECT,OFFSET2=-.5
0.05, 0.08
0.d0,1.d0,0.d0
*STEP,nlgeom
*STATIC
0.001,1,0.00000001,1
*Dload
Eall, GRAV, 9.8, 0., -1., 0.
*NODE PRINT,NSET=Nall
U
*EL PRINT,ELSET=Eall
S
*NODE FILE
S,U
*EL PRINT,ELSET=EALL,TOTALS=ONLY
ENER
*END STEP
*STEP,nlgeom,INC=2000
*DYNAMIC
1.E-2,0.2,,1.E-2
*boundary, amplitude=Amp-1
4, 2, 2,1
*END STEP
2

I also find that there is no error When I remove the gravity

3

It also works if you replace:

*BOUNDARY
1,1,6
4,1,6

with:

*BOUNDARY
1,1,6

Try with more elements.

5

Tank you very much for your reply,

but I found that it exited the calculation automatically in the picture after I replaced the statement according to your suggestion,I also found that it have a good running when I remove the gravity.

Could you give me some advise?

2UT8Z1TN)D1EH9NE8$4IBNQ
2UT8Z1TN)D1EH9NE8$4IBNQ755×266 17.8 KB

6

The model itself is correct, it works in Abaqus. So this must be a bug in CalculiX. Unfortunately, remeshing doesn’t help. Maybe switching to a different beam element type will work but it’s rather unlikely.

7

What are your Young Modulus units?
Try increasing your Young Modulus Value. to 210.000.000.000 Pa.
Probably the large initial displacement due to small Young’s modulus might be giving some problem.

9

Thank you for your suggestion,but it also could not work after I improve Young Modulus Value.
But I find that it could work when I change the first step(gravity step) from static to dynamic.So I want to apply gravity in a dynamic step .
Could you give me some advise?

10

Thank you very much !
I also think it a bug in calculix,but I have to simulate a catenary with dynamic displacement, dynamic step and gravity are both necessary.
I find that it could work when I replace STATIC with DYNAMIC,so I want apply gravity in dynamic step,but I find the displacement are change all the time under gravity after I had removed other load in dynamic step.
Could you give me some advise in applying gravity in dynamic step?

11

Hello David,

¿Have you look at beamnldy.inp, beamnldye.inp, beamnldyp.inp, beamnldype.inp files available in the example folder.? They should be very similar to what you are looking for.

Density is mandatory in Dynamic analysis as there is inertia involved.

My recommendation is that you use Calculix with a pre-procesor like Prepomax, Mecway, FreeCad or any other.

They help you and normally warn you about some points that are not properly defined. Once they work you can save it as .inp to check it.

Check this post. Pendulum - Forum

Your chain is like the pendulum example with both extremes fixed.

12

Hi,

This is the .inp and Video file generated with MECWAY.
There is no damping. You can check if you find any difference.
Solved with Calculix (v2.18 Pastix) Nonlinear Dynamic 3D.
I found that in 3D you need some rotation BC constrains to help the solver and make it work.

6m long cable section rectangular beam 8mmx8mm.
Young’s 210 GPa
Poison .33.
Density 7850 Kg/m3

NOTE : I have added four “small birds” having fun on it, 100 grams each one ( to add some asymmetry in the oscillatory pattern).

14

Hi Disla,
Thank you very very much for your reply,your suggestions are great helps to me!
Besides,I want to consult you how to implement parallel computation by setting environment variables in windows?
Best wish to you.

15

Type this in the command window and you should be able to run CalculiX analyses in parallel:

setx OMP_NUM_THREADS=n

where: n - number of available CPUs.

16

Hello David.

It’s a pleasure. There is no bug with B32 in Calculix but there is probably a bug with ONLY_TENSION material in dynamic we are investigating (it seems it is not reading density)

Some more recommendations:

-Theoretically the Catenary problem assumes infinite Stiffness and no bending load capacity.

-Time step in Dynamic should be small enough to capture waves propagating on the line.

-Add some damping to get rid of them as soon as possible or they will ruin the convergence as they reflect on both sides and make the system a mess.

-Rotational BC are required to avoid out of plane strain.

-Model keeping in mind how would be the experiment in real life.

It would help if you start to move just some time after the gravity has been applied. This would allow damping to calm down the initial perturbation before you start to move.

-There are not horizontal lines under gravity. That would require starting with infinite stiffness. Start with a mesh shape close to the expected one in repose. Parabolic may be enough.

-Probably stretching the chain is a more stable process than shrink the chain. (not tested) . Think in real life and how moving the extremes closers would induce more swinging on the chain than opening the extremes.

-Make some numbers to see what your expected results are. You can’t reproduce a catenary behaviour in real life with only 3/4 links (elements) in the chains. Start with real life constants of thinks you have seen.

-Set “Save solution every X time steps” large at the beginning. It doesn’t affect the convergence but reduce the computation time (less frd writing).

Regarding multithread you have a dedicated posts in both Mecway and Calculix. Check the one regarding Pastix Mixed Precision.

18

Thank you very much !

19

Hello，Disla.
Thank you very much for your suggestion !
The Catenary in my model is about 2400m ,I noticed that B32R element will be expanded into C3D20R in the lecture note ,so I think is there are possibilities to simulate catenary with solid element? That is what I am trying to do.
Best wish !

20

I have posted a validation file with B32 elements which is around 100 Nodes (can be run with the free version) . 5 min to run on my Laptop.
You will be surprised about the accuracy than can be achieve with just 50 elements.