shell |
 |
SHELL Model
 |
| shell |
|
SHELL Model
|
| 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}; } Physical Surface(181) = {6}; Physical Surface(182) = {10}; Physical Line(183) = {4}; Physical Line(184) = {7}; |
 |
Mesh with 2D-2order |
Mesh 2D set Order 2 |
 |
| Mesh save |
Save as gmsh.inp (Mesh -- Abaqus INP) |
|
| Mesh Convert to Calculix |
>python gi2ci2.py gmsh.inp calc.inp 2 S |
1) gmsh.inp ---- input file (gmsh's abaqus format ) 2) calc.inp ---- output file (calculix format , line elements are converted to node group ) 3) 2 ---- 2D 4) S --- PreWord 'S' will make Element Type 'S6' |
| Check and make BC with calculix |
>cgx -c calc.inp |
|
| prnt set comp SURFACE182 down plot e SURFACE181 plus e SURFACE182 b plus n CURVE183 plus f SURFACE182 send all abq names send SURFACE182 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 *SHELL SECTION , Elset=SURFACE181 , Material=STEEL 10 *SHELL SECTION , Elset=SURFACE182 , Material=PLA 10 *STEP *STATIC *BOUNDARY CURVE183,1,6,0 *DLOAD *include,input=SURFACE182.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 = 9.72[mm] (3D Result was 9.90[mm] ) |