QU8E with *PLASTIC and bug

I have two parts,
connected with one node, one part is only *ELASTIC (cube) and the another one is with *PLASTIC.
so for the result both material have for one common node plastic results.
you have these also with common node and *SURFACE INTERACTION,NAME=contact
you have these also without common nodes and *SURFACE INTERACTION,NAME=contact

if i have elements only with *elastic, there should be no plasticity as result?

wbr

As in the other thread, let’s clarify what these strange elements are first. The behavior observed here might be limited to them.

these are quadrangle plain strain elements,
generated with “elty all QU8E” you get *ELEMENT, TYPE=CPE8, ELSET=Ecircle

circle_fix.fbd

7.5° = 16 E

PNT ! 0 481 0
PNT ! 0 473 0

LINE ! D001 D002 104

seta L001 l L001
swep L001 A001 rot z -75 160

seta L002 l L002
swep L002 A002 rot z -15 32

seta L005 l L005
swep L005 A003 rot z -15 32

seta L008 l L008
swep L008 A004 rot z -75 160

seta D007 p D007
swep D007 L00E tra 0 70 0 16

seta L00E l L00E
swep L00E A005 tra 140 0 0 32

seta L00G l L00G
swep L00G A006 tra 0 -70 0 16

seta circle s A001 A002 A003 A004
comp circle d

seta cube s A005 A006
comp cube d
flip cube

flip all

merg p all
merg l all

elty all QU8E
mesh all

seta fix_01 l L001
seta fix_02 l L00B
seta displc l L00F L00K
seta mast_l l L009 L006
seta slav_l l L00J L00E
seta fix l L001 L00B
seta monitor p D00K

comp fix_01 d
comp fix_02 d
comp displc d
comp slav_l d
comp mast_l d
comp mast_l d
comp fix d

plot n fix_01
plus n fix_02
plus n displc
plus n slav_l b
plus n mast_l g

prnt se

send circle abq
send cube abq
send fix_01 abq nam
send fix_02 abq nam
send displc abq nam
send slav_l abq nam
send mast_l abq nam
send slav_l abq sur
send mast_l abq sur
send fix abq nam
send monitor abq nam

circle_fix.inp

*HEADING
**Model: Structure circle fix

*INCLUDE, INPUT=circle.msh
*INCLUDE, INPUT=cube.msh
*INCLUDE, INPUT=fix_01.nam
*INCLUDE, INPUT=fix_02.nam
*INCLUDE, INPUT=displc.nam
*INCLUDE, INPUT=slav_l.nam
*INCLUDE, INPUT=mast_l.nam
*INCLUDE, INPUT=fix.nam
*INCLUDE, INPUT=monitor.nam

*MATERIAL, NAME=steel_el
*ELASTIC
210000,0.3
*SOLID SECTION, Elset=Ecube, Material=steel_el

*MATERIAL, NAME=steel_pl
*ELASTIC
210000,0.3
*PLASTIC
235,0
*SOLID SECTION, Elset=Ecircle, Material=steel_pl

*STEP, NLGEOM

*STATIC

*BOUNDARY
Nfix_01,1,2,0
Nfix_02,1,2,0

Ndisplc,1,1,-15

*NODE PRINT, NSET=Nfix, TOTALS=ONLY
RF

*NODE PRINT, NSET=Ndisplc, TOTALS=ONLY
RF

*NODE PRINT, NSET=Nmonitor, TOTALS=ONLY
U

*NODE FILE, OUTPUT=2D
U

*EL FILE
S, PEEQ

*END STEP

This is due to the fbd file format with the nodal results always being averaged over the contributions of adjacent elements. You need to separate the mesh topology in order to avoid the problem. You still can couple the meshes using appropriate equations.

See CalculiX-Examples/Linear/Separate at master · mkraska/CalculiX-Examples · GitHub

There, nodal averaging is completely suppressed in order to reveal the discontinuities between the fields at element borders. The required equations are generated by a very generic helper script.

The script could be modified to separate element sets only (ABAQUS doesn’t average over elements belonging to different materials by default).

In your case, there are just 3 equations required.

However, nothing is wrong with the result, it is just an averaging artefact which you could well ignore.

Martin Kraska

2 Likes