Gmsh2.5.1(lator?)  (it will not work 2.5.0 )

Gmsh 3DMesh  --->  Export Abaqus inp ---> Calculix inp

Make Geometry
with Gmsh

and define Physical  groups
cl1 = 5;
Point(1) = {10, 0, 0, cl1};
Point(2) = {50, 0, 0, cl1};
Point(3) = {100, 0, 0, cl1};
Line(1) = {1, 2};
Line(2) = {2, 3};
Extrude {0, 10, 0} {
  Line{1, 2};
}
Extrude {0, 0, 20} {
  Surface{6, 10};
}
Physical Surface(183) = {31};
Physical Surface(184) = {49};
Physical Volume(181) = {1};
Physical Volume(182) = {2};

Mesh with 3D-2order

Mesh 3D
set Order 2

Mesh save
Save as gmsh.inp (Mesh -- Abaqus INP)

Mesh Convert to Calculix
>python gi2ci2.py gmsh.inp calc.inp 3 C3 1) gmsh.inp ---- input file (gmsh's abaqus format )
2) calc.inp ---- output file (calculix format , surface elements are converted to node group  )
3) 3 ---- 3D
4) C3 --- PreWord   'C3' will make Element Type 'C3D10'   , if  'F3' --> 'F3D10'
Check and make BC
with calculix
>cgx -c calc.inp


prnt set
comp SURFACE184 down
plot e VOLUME181 g
view elem on
view edge off
frame
plus e VOLUME182 b
plus n SURFACE183
plus f SURFACE184
send all abq names
send  SURFACE184 abq pres 1.0

make solver file
(sol.inp)
*INCLUDE, INPUT=calc.inp
*INCLUDE, INPUT=all.nam

*MATERIAL, NAME=STEEL
*ELASTIC
 200000  ,  0.3

*MATERIAL, NAME=PLA
*ELASTIC
 1000    ,  0.3

*SOLID SECTION , Elset=VOLUME181 , Material=STEEL
*SOLID SECTION , Elset=VOLUME182 , Material=PLA
*STEP
*STATIC
*BOUNDARY
SURFACE183,1,3,0
*DLOAD
*include,input=SURFACE184.dlo
*NODE PRINT,NSET=Nall
U
*EL PRINT,ELSET=Eall
S
*NODE FILE
U
*EL FILE
S
*END STEP



solver start
>ccx sol

view result
>cgx -v sol.frd


Max Displacement = 9.90[mm]




Return



inserted by FC2 system