3D Gmsh Assembly -> Calculix   (via msh)

• INCOMPLETION version
• 3D mesh only
• cannot convert Gmsh's Type18(18-node second order prism )
  cannot convert Gmsh's  Type 12(27-node second order hexahedron )
  (Type18 and Type 12 will be made when using  Recombine and mesh oder 2)
  

gmsh -- gmsh

Calculix -- Calculix    WindowsVersion

You need Python2.* . if you don't have it , please get and install it.
(I don't know the script will run with Python3. )

• get g2c3.py from here
  
  
• extract zip file
  

// Gmsh project created on Wed Aug 17 15:55:39 2011 lc = 5; Point(1) = {0, 0, 0, lc}; Point(2) = {50, 0, 0, lc}; Point(3) = {50, 10, 0, lc}; Point(4) = {0, 10, 0, lc}; Point(5) = {100, 0, 0, lc}; Point(6) = {100, 10, 0, lc}; Line(1) = {1, 2}; Line(2) = {2, 3}; Line(3) = {3, 4}; Line(4) = {4, 1}; Line(5) = {2, 5}; Line(6) = {5, 6}; Line(7) = {6, 3}; Line Loop(8) = {4, 1, 2, 3}; Plane Surface(9) = {8}; Line Loop(10) = {2, -7, -6, -5}; Plane Surface(11) = {10}; Extrude {0, 0, 20} {   Surface{9, 11}; } Physical Surface(101) = {20}; Physical Surface(201) = {46}; Physical Volume(301) = {1}; Physical Volume(302) = {2};

• Mesh 3D  and set order 2
  
• Save as gmsh.msh  (don't check any option )
  
  
•  
• Run convert script

 gmsh.msh   is input file name ,   sol.inp  is output inp file name

g2c3.py gmsh.msh sol.inp C3 --->  C3D10

g2c3.py gmsh.msh sol.inp F3 --->  F3D10

g2c3.py gmsh.msh sol.inp F3  R --->  F3D10R  (although nonsense )

• Run calculix
   

  cgx   -c   sol.inp

• 
  
• display mesh

plot elem all view elem on view edge off frame

• check set
  

prnt set 1     all stat:o n:1595 e:838 f:440 p:0 l:0 s:0 b:0 L:0 S:0 se:0 sh:0 2     N101 stat:c n:31 e:0 f:0 p:0 l:0 s:0 b:0 L:0 S:0 se:0 sh:0 3     N201 stat:c n:165 e:0 f:0 p:0 l:0 s:0 b:0 L:0 S:0 se:0 sh:0 4     E301 stat:c n:0 e:420 f:0 p:0 l:0 s:0 b:0 L:0 S:0 se:0 sh:0 5     +C3D10 stat:c n:0 e:838 f:0 p:0 l:0 s:0 b:0 L:0 S:0 se:0 sh:0 6     E302 stat:c n:0 e:418 f:0 p:0 l:0 s:0 b:0 L:0 S:0 se:0 sh:0

display and check each sets

plot n N101 (fix nodes)
plot n N201 (load nodes)
plot e E301 (Material1)
plot e E302 (Material2)

• then make surface set and element sets form these node sets

comp N201 down plot f N201 ( LOAD is face sets )
plot e E301 plus e E302 plus n N101 plus f N201  (confirm each sets )
send all abq names send N201 abq pres 1

• solsol.inp    is  like this

*INCLUDE, INPUT=sol.inp *INCLUDE, INPUT=all.nam *MATERIAL, NAME=STEEL *ELASTIC  200000  ,  0.3 *MATERIAL, NAME=PLA *ELASTIC  1000  ,  0.35 *SOLID SECTION , Elset=E301 , Material=STEEL *SOLID SECTION , Elset=E302 , Material=PLA *STEP *STATIC *BOUNDARY N101,1,3,0 *DLOAD *include,input=N201.dlo *NODE PRINT,NSET=Nall U *EL PRINT,ELSET=Eall S *NODE FILE U *EL FILE S *END STEP

return

///