Gmsh Assembly -> Calculix   (via unv)

Tweet

�@

�@

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 Media:unv2xUpd2.zip   from
  http://www.caelinux.org/wiki/index.php/Proj:UNVConvert
• extract zip file and 
  copy unv2abaqus.py to unv2calculix.py 
  copy unv2x.py to unv2xc.py
  
• open unv2calculix.py with TextEditor  
    change line 1
          from unv2x import *
   to 
          from unv2xc import *
   
    change line 112
          fil.write('%8d' % (lst.pop(0)))
  to
        fil.write(('%8d'+ls) % (lst.pop(0)))
• save and close TextEditor

• open unv2xc.py with TextEditor 
  change line 179-180

            self.datasetsIds=[2411,2412,2467]
            self.datasetsHandlers=[UNV2411Reader,UNV2412Reader,UNV2467Reader]

       to
            self.datasetsIds=[2411,2412,2467,2477]
            self.datasetsHandlers=[UNV2411Reader,UNV2412Reader,UNV2467Reader,UNV2467Reader]

• save and close TextEditor

Make Assy with Gmsh

// 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(56) = {20};
Physical Surface(57) = {46};
Physical Volume(58) = {1};
Physical Volume(59) = {2};

• Mesh 3D  and set order 2
  
• Save as gmsh.unv  (check Save Group of nodes)
  
•  
• Run convert script

 gmsh.unv   is input file name ,   gmsh  is output inp file name ( it will make gmsh.inp )

• Run calculix
   

  �@cgx   -c   gmsh.inp

• 
• display mesh

plot elem all view elem on view edge off frame

�@

•  
• check set
  

�@prnt set 1     all stat:o n:1562 e:813 f:436 p:0 l:0 s:0 b:0 L:0 S:0 se:0 sh:0 2     NALL stat:c n:1562 e:0 f:0 p:0 l:0 s:0 b:0 L:0 S:0 se:0 sh:0 3     C3D10 stat:c n:0 e:813 f:0 p:0 l:0 s:0 b:0 L:0 S:0 se:0 sh:0 4     +C3D10 stat:c n:0 e:813 f:0 p:0 l:0 s:0 b:0 L:0 S:0 se:0 sh:0 5     PERMANENTGROUP1 stat:c n:31 e:0 f:0 p:0 l:0 s:0 b:0 L:0 S:0 se:0 sh:0 6     PERMANENTGROUP2 stat:c n:161 e:0 f:0 p:0 l:0 s:0 b:0 L:0 S:0 se:0 sh:0 7     PERMANENTGROUP3 stat:c n:819 e:0 f:0 p:0 l:0 s:0 b:0 L:0 S:0 se:0 sh:0 8     PERMANENTGROUP4 stat:c n:774 e:0 f:0 p:0 l:0 s:0 b:0 L:0 S:0 se:0 sh:0

• So set names are too long , copy sets  for convenience.

seta P1 set PERMANENTGROUP1 seta P2 set PERMANENTGROUP2 seta P3 set PERMANENTGROUP3 seta P4 set PERMANENTGROUP4

display and check each sets

plot n P1 �@ (fix nodes)	�@
plot n P2 (load nodes)	�@
plot n P3 (Material1)	�@
plot n P4 (Material4)	�@

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

seta FIX set P1 plot n FIX ( FIX is fix node sets )	�@
comp P2 down seta LOAD set P2 plot f LOAD ( LOAD is face sets )	�@
seta M1 set P3 setr M1 set P4 comp M1 up plot e M1 plus n P3 (M1 is material 1 sets ) (because there are common nodes between P3 and P4 , 'setr M1 set P4'  is needed )	�@
�@(If not using  'setr M1 set P4'     elements sets is not correct ) plot e M1 plus n P3	�@
seta M2 set P4 setr M2 set P3 comp M2 up plot e M2 plus n P4	�@
plot e M1 plus e M2 plus n FIX plus f LOAD  (confirm each sets )	�@
send all abq send M1 abq names send M2 abq names send LOAD abq pres 1 send FIX abq names	�@

• sol.inp    is  like this

*INCLUDE, INPUT=all.msh *INCLUDE, INPUT=FIX.nam *INCLUDE, INPUT=M1.nam *INCLUDE, INPUT=M2.nam *MATERIAL, NAME=STEEL *ELASTIC  200000  ,  0.3 *MATERIAL, NAME=PLA *ELASTIC  1000  ,  0.35 *SOLID SECTION , Elset=EM1 , Material=STEEL *SOLID SECTION , Elset=EM2 , Material=PLA *STEP *STATIC *BOUNDARY NFIX,1,3,0 *DLOAD *include,input=LOAD.dlo *NODE PRINT,NSET=Nall U *EL PRINT,ELSET=Eall S *NODE FILE U *EL FILE S *END STEP

�@

now:

///