Strain not rotating with dynamic NLGEOM

1

This is a short rod under constant tension and rotating. The strain is correct for the initial orientation (eXX = 1.0e-7), but as it rotates through 180 degrees, the strain doesn’t rotate, as if it’s small displacements. This doesn’t seem right and I think it should rotate so there’s strain YY = 1.0e7 when the rod is aligned with the Y axis. Stress does that, and strain does too with *STATIC. Does anyone know what’s happening? Could it be a bug or does strain mean something different in *DYNAMIC and *STATIC?

image
image704×448 6.48 KB

*NODE
1,0,-0.5,0
2,0,0.5,1
3,2,-0.5,1
4,0,0.5,0
5,2,-0.5,0
6,1,0.5,0
7,1,-0.5,0
8,2,0.5,0
9,2,0.5,1
10,0,-0.5,1
11,1,-0.5,1
12,1,0.5,1
*ELEMENT,TYPE=C3D8I,ELSET=DEFAULT
1,1,7,6,4,10,11,12,2
2,7,5,8,6,11,3,9,12
*SURFACE,NAME=PRESSURE_FACES(2)
2,S3
1,S5
*SURFACE,NAME=PRESSURE_FACES
2,S4
1,S6
*MATERIAL,NAME=MATERIAL
*ELASTIC,TYPE=ISOTROPIC
100000000000,0
*DENSITY
1000
*SOLID SECTION,ELSET=DEFAULT,MATERIAL=MATERIAL
*AMPLITUDE,NAME=A_1
0,100
0.994,100
1.001,0
70,0
*STEP,NLGEOM=YES,INC=700
*DYNAMIC,DIRECT
0.1,70,0,0
*DSLOAD,AMPLITUDE=A_1
PRESSURE_FACES(2),P,1
*DSLOAD
PRESSURE_FACES,P,-10000
*NODE FILE
U
*EL FILE
S,NOE,E
*END STEP
2

Here’s what I got from Abaqus:

image
image770×567 19 KB

image
image769×560 8.52 KB

1 Like
3

My strains does not change in STATIC either.

*NODE
1,0,0,0
2,-0.4,-0.6,-1.8
3,0.6,-0.6,-1.8
4,0.6,0.4,-1.8
5,-0.4,0.4,-1.8
6,-0.4,-0.6,-0.8
7,0.6,-0.6,-0.8
8,0.6,0.4,-0.8
9,-0.4,0.4,-0.8
10,0,0,-1
11,0,0,0
*ELEMENT,TYPE=C3D8I
1,2,3,4,5,6,7,8,9
*NSET,NSET=REF
1
*NSET,NSET=BASE
6
7
8
9
*ELSET,ELSET=ESET1
1
*SURFACE,NAME=PRESSURE_FACES(2)
1,S1
*SURFACE,NAME=BASE
1,S2
*ORIENTATION,NAME=O1
1,0,0,0,1,0
*MATERIAL,NAME=MATERIAL
*ELASTIC,TYPE=ISOTROPIC
100000000000,0
*DENSITY
1000
*SOLID SECTION,ELSET=ESET1,MATERIAL=MATERIAL,ORIENTATION=O1
*BOUNDARY
1,1,,0
1,2,,0
1,3,,0
11,1,,0
11,3,,0
*RIGID BODY,NSET=BASE,REF NODE=1,ROT NODE=11
*AMPLITUDE,NAME=A_2
0,0
0.1,0
1,6.28318530718
*AMPLITUDE,NAME=A_3
0,0
0.1,-100000000
1,-100000000
*STEP,NLGEOM=YES,INC=500,AMPLITUDE=STEP
*STATIC
0.01,1,0,0.01
*BOUNDARY,AMPLITUDE=A_2
11,2,,1
*DSLOAD,AMPLITUDE=A_3
PRESSURE_FACES(2),P,1
*NODE FILE,GLOBAL=YES
U
*EL FILE
S,NOE,E,ENER
*EL FILE,GLOBAL=YES
S,NOE,E
*EL PRINT, ELSET=ESET1
ME,S
*END STEP
4

Isn’t LE11 supposed to always be greater than LE22? Or does 11 mean xx? Do you know how those are defined?

5

11 means xx and 22 means yy in Abaqus (assuming default coordinate system). LE stands for logarithmic strain.

1 Like
6

@Disla Oh yes, *STATIC strain behaves the same. I was confused. Do you think this non-rotating strain is intentional or a bug? I suppose if you work out how the elements rotate, you could rotate it to follow them, but that seems like something CCX should be doing, I’d think.

7

I think it should be rotating as Stresses but maybe it’s intentional to speed up the result and save some disk writing.
Who would use those values?. I have request *El print (ME) and do not change either

8

Maybe it’s correct since the manual says both E and ME are Lagrangian strain, and it seems like Lagrangian strain is supposed to behave this way. It uses the global coordinate system in the initial state but rotates it with the elements as they rotate. It’s not the element coordinate system.

So that’s a surprising thing!

@Calc_em did Abaqus only output LE, not E with that input file? I wonder if this is still consistent with Abaqus just that it doesn’t automatically output LE when you ask for E.