Modeling Interactions & Assemblies

Report
Joël Cugnoni, LMAF/EPFL, 2012

How can we model more complex cases ?
◦ It is possible to define interactions between
different regions of a model by the means of
additional equations that relate the degrees of
freedoms of multiple nodes.

Bilateral constraints to “glue” separate parts:

Unilateral constraints:
◦ Node to node interaction : Equation constraint
◦ Node to surface interaction : Kinematic coupling
◦ Surface to surface interation: Tie constraint
◦ Contact: no penetration between two faces, friction
& sliding => non linear behaviour, not in course
Available in Interaction->Constraints->Equation
 one linear equation between several DOFs
a1 Node1.DOF1 + a2 Node2.DOF2 + … = constant

Antisymmetry
1 * Node17.U1 + 1 * Node23.U1 = 0
17
y
Mechanism (Pulley)
1 * Node12.U2 - 1 * Node21.U1 = 0
23
21
14
x




Available in Interaction->Constraints->Coupling->Kinematic coupling
Multiple equations to keep relative position constant including rotations
Tranfers the displacements / rotation of the Master node to slave surface
Usually used with reference points to link parts or apply moments /
rotation to one face
Master Node : reference point with 6 DOFS
Kinematic coupling
y
Slave Nodes : 3 DOFS
x



Available in Interaction->Constraints->Tie
Multiple kinematic equations to keep relative position constant
between each point of the master surface and their
corresponding projection on the slave surface
Usually used to link two parts of an assembly to ensure
continuity of the displacements (approximation)
Slave surface
Small distance
(projection tolerance)
Projection lines
Master surface
y
x

Three methods:
◦ Continuous CAD model:
Merge all parts in CAD -> export STP model -> import
in Abaqus -> partition to differentiate the materials
◦ Merged geometry:
model as an assembly in CAD -> export as STP ->
import in Abaqus -> create assembly and position parts
-> Merge geometry + keep internal interfaces
◦ Tie / coupling constraints:
model as an assembly in CAD -> export as STP ->
import in Abaqus -> create assembly and position parts
-> Create Tie / coupling to model the interactions
between parts


See assembly1.cae
Procedure:
◦
◦
◦
◦
◦
◦
◦
◦
◦
◦
◦
◦
◦
◦
◦
◦
open assembly1-input.cae
create instance for piston and axe1
align axe1 with coaxial + face to face (-13mm offset)
merge and keep interfaces
add instance for biele1
align with coaxial +face2face +4mm offset
assign properties to all parts / regions and then create step
create 1st constraint: tie for axis to biele surfaces
create datum point in the middle of lower biele axis
create reference point
create constraint: kinematic coupling btw RP and lower axis of biele
boundary condition: pressure 0.1MPa on top of cylinder, all
displacement & rotation constrained on RP
mesh fused part with tets quad 2.8mm
mesh biele with hexa sweep or wedges (partition by extending faces)
run job
show results with several cutting plane to show
 1) mesh continuity between the merged parts
 2) displacement continuity but mesh discontinuity where tie is used

similar documents