Import and modify an assembly model from CAD
3D to 2D
adjust scale, if needed
Is symmetry appropriate ?
2D, planar element types
Need for "Real Constants"
Materials which may yield (plasticity)
Multiple bodies with
different materials
different thickness (element behavior) and "Real Constants"
assignment of mesh "Attributes" on geometry (areas)
Contact between parts can change
Load steps (clamp, and then pressurize pipe)
NON-Linear Solution:
small or large deformations ?
automatic time stepping / gradual load application (substeps)
iterative solution, (equilibrium) convergence
results controls
Postprocessing: Different Bodies (Selecting/Scoping)
A 3D solid model in Parasolid format (meter dimensions), pipe_and_clamp.x_t, is available to download or from the Angel HW folder.
An aluminum bracket clamps a very long PVC plastic pipe. The material properties are given:
| Elastic Modulus (psi) | Poisson's Ratio | |
| Aluminum | 10,000,000 | 0.33 |
| PVC plastic | 827,000 | 0.40 |
The aluminum part is 0.5" thick
The coefficient of friction between the aluminum and PVC plastic is 0.05
The PVC plastic may yield and the stress strain curve is given as:
| Strain (in/in) | Stress (psi) |
 |
| 0.002 | 1654 | |
| 0.015 | 11610 | |
| 0.027 | 15290 | |
| 0.068 | 20970 | |
| 0.122 | 24240 | |
|
Note: Use a Multi-linear, kinematic hardening material model
|
||
Loading: The left (flat edge) is fixed to a rigid wall (ALL DOF, zero)
A bolt (not modeled) applies a 250 lbf clamping force on the bracket 0.1" from the end (which places it at the end of the round corner feature).
After the pipe is clamped in the bracket, it is pressurized. The internal pressure is 500 psi. The clamping force is NOT removed - it is held at 250 lbf when the pressure load is added.
Check the scale of your model (and adjust, if needed):
The clamp bracket overall dimensions are 2.0" wide x 1.5" height
The pipe is 1.125" O.D. and 1.0" I.D.
Use the MeshTool to assign Area Attributes to each part (material ID, element type ID, and real constant number)
Use SMRTSIZE for meshing. It creates a fine mesh where the two bodies will have contact.
Use the Contact Manager and Contact Wizard to define edges for target and contact pairs.
1. A plot showing different materials assigned to the parts
2. A plot showing the mesh (document the number of nodes and elements used)
3. A plot showing the stress-strain curve for the PVC material
4. A plot showing ALL loads and constraints on the model (clamping and pressure loads)
AT THE END OF LOAD STEP 1 (clamping load, only)
5. A plot of SX stress on only the clamp body (which might be used for an estimate and comparison of bending stress in the outermost fiber)
AT THE END OF EACH LOAD STEP:
6. A plot showing total deformation (both parts included)
7. A plot showing the vonMises stress in EACH part
8. A plot showing the equivalent (vonMises) plastic strain in the PVC part (to show where yielding occurred).
9. A plot of contact pressure on EVERY contact pair in your model