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] |