Abaqus B31 elements Excessive rotation error in explicit dynamics

[MOZER8]

Dear All,

I am doing a web catch analysis using abaqus dynamic explicit. An object with initial speed of ~50000mm/s is cought by a web which is built with B31 elements. B31 elements has hyperelastic properties. Contact between object and web was defined as general contact. Analysis duration is 0.6s with auto increament. (image 1 for we geometry)

After I ran the analysis, job aborted at around 0.19th second with an error: "Excessive rotation of nodes in node set ErrNodeExcessRotation-Step1." I checked the results and realized that most of the B31 elements started to rotate (check image 2,3 and 4). I made some research decided to reduce the B31 element size. Thus, element number on one line increased from 6 to 18.

I ran the second analysis with reduced element size and job aborted at around 0.23rd second with an error"The ratio of deformation speed to wave speed exceeds 1.0000 in at least one element. This usually indicates an error with the model definition. Additional diagnostic information may be found in the message file." Again I checked the rotational displacement and speed most of the beam elements are doing good but in one location beam element rotation and velocity increased dramatically. (check image 5, 6 and 7).

I have two ideas here:

1. This motion caused by insufficient rotational stiffness(J) of the beam element. I decided to keep the I11 and I22 same and increase Torsional constant(J). I made a generalized profile with higher J, however I'm not able to use generalized profile while section integration is selected as "during analysis, it only allows "before analysis". Thus I can not continue.

2. This motion caused by negative axial stress on B31 elements. In order to prevent this phenomenon, B31 axial stiffness values will be updated and a pretension will be defined for all B31 elements. Applied pretension will cancel out updated stiffness value (see image 8). However I don't know how to define all the B31 elements pretension, and how to implement it into explicit transient as initial conditions.

These are the ideas and questions for this problem. Thank you for your help in advance.

image 1:

https://files.engineering.com/getfile.aspx?folder=1680250e-b07c-4226-824e-c039188a3fc3&file=1.png

image 2:

https://files.engineering.com/getfile.aspx?folder=9ba22d1d-d5c2-4081-bd1d-a759c71f24f3&file=2.png

image 3:

https://files.engineering.com/getfile.aspx?folder=87646b14-b03f-40e0-8932-2e2357a098bb&file=3.png

image 4:

https://files.engineering.com/getfile.aspx?folder=9a6783c3-c81e-4a74-8914-ae9ec069778f&file=4.png

image 5:

https://files.engineering.com/getfile.aspx?folder=de5d96ae-42ca-4252-8883-b884e300b9cc&file=5.png

image 6:

https://files.engineering.com/getfile.aspx?folder=d76793f6-b3a0-4f80-8dd4-8a3a4c6f4cd8&file=6.png

image 7:

https://files.engineering.com/getfile.aspx?folder=1614aea6-d286-4f07-9cb9-995f605263cb&file=7.png

image 8:

https://files.engineering.com/getfile.aspx?folder=e39407da-3722-4390-9d9e-aeca7717d289&file=8.PNG

 

[Erik Panos Kostson]

By web I assume that these are not really beams, but more of a cable structure - if that is the case i would try using truss elements. Obviously they need to have a pretension to take the out of plane load. Using an implicit step before with some pretension and using that as initial condition for the explicit could be one way of doing this (alternatively one can have two steps in explicit one with a quasi static pretension, and then the impact).
This is a post on that with a small example:

https://www.eng-tips.com/viewthread.cfm?qid=454971

 

[FEA way]

Try using more beam elements and consider including damage with element deletion. Did you assign mass to impactor (I assune it’s rigid).

 

[Erik Panos Kostson]

That could be an idea (refinement), but how do you use beams/trusses and element deletion FEA way?

 

[MOZER8]

Thank you for the suggestion. It seems truss element solved my issue.

Now I need some damage criteria and element deletion for truss elements. Can I apply element deletion criteria for truss elements?

 

[Erik Panos Kostson]

I can not see that option anywhere when assigning element type to parts/instances (mesh module), there is no deletion option like it is when you have for instance a Hex 3D element (e.g., for C3D8R).

Not sure what FEA way meant or if he has another way of doing this,

In any way in the manual chapter about dynamic failure modes if beams (not sure trusses) are used with JC or VM strength models, then a shear failure criteria can be defined (based on plastic strain), which will then remove beams automatically. See that chapter for more info (now your material might not be a metal so then these criteria might not be correct)

I will try it tomorrow and see how it goes

 

[FEA way]

It should be possible to enable element deletion for beam (and probably also truss) elements using input file: *SECTION CONTROLS, ELEMENT DELETION=YES

 

[MOZER8]

Erik, FEA way,thank you for your interest to this topic.

I added "*SECTION CONTROLS, ELEMENT DELETION=YES" to input file even thought there is no element deletion option under truss element in GUI. In addition to that, I need an damage evaluation for my material. However, Stress fail and Strain fail are the parameters for linear elastic material. I need hyperelastic material with a failure criteria for element deletion.

 

[Erik Panos Kostson]

I saw that shear failure is not supported for future releases, so damage initiation+evolution is the way to do this - never used anything like that for hyper elastic material, so I do not know.
(also normally and I doubt that any hyper elastic models can be used on beams and trusses)

 

[MOZER8]

Okay, now I converted web material to linear elastic with an acceptable error. Then I tried to run it with truss elements it didn't allow me to set fail strain or fail stress criteria, thus I cconverted the elements to beam elements.
In summary, beam elements, linear elastic material with fail strain option is active, element deletion is active, explicit dynamic analysis.
When the analysis was run with above configuration, it doesn't give an error. However, even though LE(logarithmic strain) exceeded the defined fail strain limit, element deletion did not occur. Am I missing something or are there some limitations with beam elements for element deletion?

 

[Erik Panos Kostson]

Not sure exactly what failure model you use - as mentioned I tried shear failure (+deletion) which needs to be used with VM plasticity and it worked on trusses. Again though I am not sure if shear failure can be used in newer versions of abaqus.

Below is a small example where element 11 fails - I have set the plastic strain limit low so it can fail very close to yield.

*Heading
*Preprint, echo=NO, model=NO, history=NO, contact=NO
**
** PARTS
**
*Part, name=Part-1
*Node
      1,           0.,           0.,           0.
      2,  0.100000001,           0.,           0.
      3,  0.200000003,           0.,           0.
      4, 0.00999999978,           0.,           0.
      5, 0.0199999996,           0.,           0.
      6, 0.0299999993,           0.,           0.
      7, 0.0399999991,           0.,           0.
      8, 0.0500000007,           0.,           0.
      9, 0.0599999987,           0.,           0.
     10, 0.0700000003,           0.,           0.
     11, 0.0799999982,           0.,           0.
     12, 0.0900000036,           0.,           0.
     13,  0.109999999,           0.,           0.
     14,  0.119999997,           0.,           0.
     15,  0.129999995,           0.,           0.
     16,  0.140000001,           0.,           0.
     17,  0.150000006,           0.,           0.
     18,  0.159999996,           0.,           0.
     19,  0.170000002,           0.,           0.
     20,  0.180000007,           0.,           0.
     21,  0.189999998,           0.,           0.
*Element, type=T3D2
 1,  1,  4
 2,  4,  5
 3,  5,  6
 4,  6,  7
 5,  7,  8
 6,  8,  9
 7,  9, 10
 8, 10, 11
 9, 11, 12
10, 12,  2
11,  2, 13
12, 13, 14
13, 14, 15
14, 15, 16
15, 16, 17
16, 17, 18
17, 18, 19
18, 19, 20
19, 20, 21
20, 21,  3
*Nset, nset=Set-1, generate
  1,  21,   1
*Elset, elset=Set-1, generate
  1,  20,   1
*Nset, nset=Set-2, generate
  1,  21,   1
*Elset, elset=Set-2, generate
  1,  20,   1
** Section: Section-1
*Solid Section, elset=Set-1, material=Material-1
0.001,
*End Part
**  
*Part, name=Part-2
*Node
      1,           0., 0.00499999989,           0.
      2,  0.100000001, 0.00499999989,           0.
      3,  0.200000003, 0.00499999989,           0.
      4, 0.00999999978, 0.00499999989,           0.
      5, 0.0199999996, 0.00499999989,           0.
      6, 0.0299999993, 0.00499999989,           0.
      7, 0.0399999991, 0.00499999989,           0.
      8, 0.0500000007, 0.00499999989,           0.
      9, 0.0599999987, 0.00499999989,           0.
     10, 0.0700000003, 0.00499999989,           0.
     11, 0.0799999982, 0.00499999989,           0.
     12, 0.0900000036, 0.00499999989,           0.
     13,  0.109999999, 0.00499999989,           0.
     14,  0.119999997, 0.00499999989,           0.
     15,  0.129999995, 0.00499999989,           0.
     16,  0.140000001, 0.00499999989,           0.
     17,  0.150000006, 0.00499999989,           0.
     18,  0.159999996, 0.00499999989,           0.
     19,  0.170000002, 0.00499999989,           0.
     20,  0.180000007, 0.00499999989,           0.
     21,  0.189999998, 0.00499999989,           0.
*Element, type=T3D2
 1,  1,  4
 2,  4,  5
 3,  5,  6
 4,  6,  7
 5,  7,  8
 6,  8,  9
 7,  9, 10
 8, 10, 11
 9, 11, 12
10, 12,  2
11,  2, 13
12, 13, 14
13, 14, 15
14, 15, 16
15, 16, 17
16, 17, 18
17, 18, 19
18, 19, 20
19, 20, 21
20, 21,  3
*Nset, nset=Set-1, generate
  1,  21,   1
*Elset, elset=Set-1, generate
  1,  20,   1
*Nset, nset=Set-2, generate
  1,  21,   1
*Elset, elset=Set-2, generate
  1,  20,   1
** Section: Section-1
*Solid Section, elset=Set-1, material=Material-1
0.001,
*End Part
**  
**
** ASSEMBLY
**
*Assembly, name=Assembly
**  
*Instance, name=Part-1-1, part=Part-1
          0.,        2e-06,           0.
*End Instance
**  
*Instance, name=Part-2-1, part=Part-2
         0.1,       -0.005,          0.1
         0.1,       -0.005,          0.1,          0.1, 0.995000012688052,          0.1, 89.9999992730282
*End Instance
**  
*Nset, nset=Set-1, instance=Part-1-1
 1,
*Nset, nset=Set-2, instance=Part-2-1
 3,
*Nset, nset=Set-3, instance=Part-2-1
 1,
*Nset, nset=Set-4, instance=Part-1-1
 3,
*Nset, nset=Set-5, instance=Part-2-1
 2,
*Nset, nset=Set-10, instance=Part-1-1
 2,
*Nset, nset=Set-11, instance=Part-1-1
 2,
*Nset, nset=Set-12, instance=Part-1-1, generate
  1,  21,   1
*Elset, elset=Set-12, instance=Part-1-1, generate
  1,  20,   1
*Nset, nset=Set-13, instance=Part-1-1, generate
  1,  21,   1
*Elset, elset=Set-13, instance=Part-1-1, generate
  1,  20,   1
*Nset, nset=m_Set-6, instance=Part-2-1
 2,
*Nset, nset=m_Set-8, instance=Part-1-1
 2,
*Nset, nset=s_Set-6, instance=Part-1-1
 2,
*Nset, nset=s_Set-8, instance=Part-2-1
 2,
*Elset, elset=_Surf-1_, internal, instance=Part-1-1
 10, 11
*Surface, type=ELEMENT, name=Surf-1
_Surf-1_, 
*End Assembly
** 
** ELEMENT CONTROLS
** 
*Section Controls, name=EC-1,element deletion=yes
1., 1., 1., 0.95, 1.
*Amplitude, name=Amp-1
             0.,              0.,              1.,              1.
*Amplitude, name=Amp-2
             1.,              0.,             1.2,              1.
*Amplitude, name=Amp-3
             0.,              0.,            0.05,              0.,           0.055,             0.5,            0.06,              1.
          0.065,             0.5,            0.07,              0.,             0.2,              0.
** 
** MATERIALS
** 
*Material, name=Material-1
*Density
7800.,
*Elastic
 2e+11, 0.3
*Plastic
 1.5e+08,        0.
 0.00225, 1.545e+08
**
*shear failure, element deletion = yes
1E-4,
** INTERACTION PROPERTIES
**
*Surface Interaction, name=IntProp-1
*Friction
0.,
*Surface Behavior, pressure-overclosure=HARD
** ----------------------------------------------------------------
** 
** STEP: Quasi
** 
*Step, name=Quasi, nlgeom=YES
*Dynamic, Explicit
, 1.
*Bulk Viscosity
0.06, 1.2
** 
** BOUNDARY CONDITIONS
** 
** Name: BC-1 Type: Symmetry/Antisymmetry/Encastre
*Boundary
Set-1, ENCASTRE
** Name: BC-2 Type: Symmetry/Antisymmetry/Encastre
*Boundary
Set-2, ENCASTRE
** Name: BC-3 Type: Displacement/Rotation
*Boundary, amplitude=Amp-1
Set-3, 1, 1
Set-3, 2, 2
Set-3, 3, 3, 0.0001
** Name: BC-4 Type: Displacement/Rotation
*Boundary, amplitude=Amp-1
Set-4, 1, 1, 0.0001
Set-4, 2, 2
Set-4, 3, 3
** 
** OUTPUT REQUESTS
** 
*Restart, write, number interval=1, time marks=NO
** 
** FIELD OUTPUT: F-Output-1
** 
*Output, field, variable=ALL
** 
** HISTORY OUTPUT: H-Output-1
** 
*Output, history, variable=PRESELECT
*End Step
** ----------------------------------------------------------------
** 
** STEP: Dynamic
** 
*Step, name=Dynamic, nlgeom=YES
*Dynamic, Explicit
, 0.2
*Bulk Viscosity
0.06, 1.2
** 
** LOADS
** 
** Name: Load-1   Type: Body force
*Dload, amplitude=Amp-3
Set-13, BY, -1e+08
** 
** INTERACTIONS
** 
** Interaction: Int-1
*Contact, op=NEW
*Contact Inclusions, ALL EXTERIOR
*Contact Property Assignment
 ,  , IntProp-1
** 
** OUTPUT REQUESTS
** 
*Restart, write, number interval=1, time marks=NO
** 
** FIELD OUTPUT: F-Output-1
** 
*Output, field, variable=ALL, number interval=200
** 
** HISTORY OUTPUT: H-Output-1
** 
*Output, history, variable=PRESELECT
*End Step

 

[MOZER8]

Erik, FEA way,

Thank you very much for your help and support. I have fixed the model, element deletion is working, but I'm not sure if the modeling or parameters are all correct. I will make some research about the damage theories in abaqus.

In summary: truss elements, linear elastic material with ductile damage option is active, element deletion is active, explicit dynamic analysis.

Regards,
Mehmet

 

[FEA way]

If you want to learn more about damage modeling in Abaqus I think that the best resource will be documentation chapter „Damage and failure for ductile metals” that can be found in Materials Guide (in „Progressive Damage and Failure” part).