feat: Add M1 mirror Zernike optimization with correct RMS calculation
Major improvements to telescope mirror optimization workflow: Assembly FEM Workflow (solve_simulation.py): - Fixed multi-part assembly FEM update sequence - Use ImportFromFile() for reliable expression updates - Add DuplicateNodesCheckBuilder with MergeOccurrenceNodes=True - Switch to Foreground solve mode for multi-subcase solutions - Add detailed logging and diagnostics for node merge operations Zernike RMS Calculation: - CRITICAL FIX: Use correct surface-based RMS formula - Global RMS = sqrt(mean(W^2)) from actual WFE values - Filtered RMS = sqrt(mean(W_residual^2)) after removing low-order fit - This matches zernike_Post_Script_NX.py (optical standard) - Previous WRONG formula was: sqrt(sum(coeffs^2)) - Add compute_rms_filter_j1to3() for optician workload metric Subcase Mapping: - Fix subcase mapping to match NX model: - Subcase 1 = 90 deg (polishing orientation) - Subcase 2 = 20 deg (reference) - Subcase 3 = 40 deg - Subcase 4 = 60 deg New Study: M1 Mirror Zernike Optimization - Full optimization config with 11 design variables - 3 objectives: rel_filtered_rms_40_vs_20, rel_filtered_rms_60_vs_20, mfg_90_optician_workload - Neural surrogate support for accelerated optimization Documentation: - Update ZERNIKE_INTEGRATION.md with correct RMS formula - Update ASSEMBLY_FEM_WORKFLOW.md with expression import and node merge details - Add reference scripts from original zernike_Post_Script_NX.py 🤖 Generated with [Claude Code](https://claude.com/claude-code) Co-Authored-By: Claude <noreply@anthropic.com>
This commit is contained in:
Antoine
188
docs/06_PROTOCOLS_DETAILED/ASSEMBLY_FEM_WORKFLOW.md
Normal file
188
docs/06_PROTOCOLS_DETAILED/ASSEMBLY_FEM_WORKFLOW.md
Normal file
@@ -0,0 +1,188 @@
|
||||
# Assembly FEM Optimization Workflow
|
||||
|
||||
This document describes the multi-part assembly FEM workflow used when optimizing complex assemblies with `.afm` (Assembly FEM) files.
|
||||
|
||||
## Overview
|
||||
|
||||
Assembly FEMs have a more complex dependency chain than single-part simulations:
|
||||
|
||||
```
|
||||
.prt (geometry) → _fem1.fem (component mesh) → .afm (assembly mesh) → .sim (solution)
|
||||
```
|
||||
|
||||
Each level must be updated in sequence when design parameters change.
|
||||
|
||||
## When This Workflow Applies
|
||||
|
||||
This workflow is automatically triggered when:
|
||||
- The working directory contains `.afm` files
|
||||
- Multiple `.fem` files exist (component meshes)
|
||||
- Multiple `.prt` files exist (component geometry)
|
||||
|
||||
Examples:
|
||||
- M1 Mirror assembly (M1_Blank + M1_Vertical_Support_Skeleton)
|
||||
- Multi-component mechanical assemblies
|
||||
- Any NX assembly where components have separate FEM files
|
||||
|
||||
## The 4-Step Workflow
|
||||
|
||||
### Step 1: Update Expressions in Geometry Part (.prt)
|
||||
|
||||
```
|
||||
Open M1_Blank.prt
|
||||
├── Find and update design expressions
|
||||
│ ├── whiffle_min = 42.5
|
||||
│ ├── whiffle_outer_to_vertical = 75.0
|
||||
│ └── inner_circular_rib_dia = 550.0
|
||||
├── Rebuild geometry (DoUpdate)
|
||||
└── Save part
|
||||
```
|
||||
|
||||
The `.prt` file contains the parametric CAD model with expressions that drive dimensions. These expressions are updated with new design parameter values, then the geometry is rebuilt.
|
||||
|
||||
### Step 2: Update Component FEM Files (.fem)
|
||||
|
||||
```
|
||||
For each component FEM:
|
||||
├── Open M1_Blank_fem1.fem
|
||||
│ ├── UpdateFemodel() - regenerates mesh from updated geometry
|
||||
│ └── Save FEM
|
||||
├── Open M1_Vertical_Support_Skeleton_fem1.fem
|
||||
│ ├── UpdateFemodel()
|
||||
│ └── Save FEM
|
||||
└── ... (repeat for all component FEMs)
|
||||
```
|
||||
|
||||
Each component FEM is linked to its source geometry. `UpdateFemodel()` regenerates the mesh based on the updated geometry.
|
||||
|
||||
### Step 3: Update Assembly FEM (.afm)
|
||||
|
||||
```
|
||||
Open ASSY_M1_assyfem1.afm
|
||||
├── UpdateFemodel() - updates assembly mesh
|
||||
├── Merge coincident nodes (at component interfaces)
|
||||
├── Resolve labeling conflicts (duplicate node/element IDs)
|
||||
└── Save AFM
|
||||
```
|
||||
|
||||
The assembly FEM combines component meshes. This step:
|
||||
- Reconnects meshes at shared interfaces
|
||||
- Resolves numbering conflicts between component meshes
|
||||
- Ensures mesh continuity for accurate analysis
|
||||
|
||||
### Step 4: Solve Simulation (.sim)
|
||||
|
||||
```
|
||||
Open ASSY_M1_assyfem1_sim1.sim
|
||||
├── Execute solve
|
||||
│ ├── Foreground mode for all solutions
|
||||
│ └── or Background mode for specific solution
|
||||
└── Save simulation
|
||||
```
|
||||
|
||||
The simulation file references the assembly FEM and contains solution setup (loads, constraints, subcases).
|
||||
|
||||
## File Dependencies
|
||||
|
||||
```
|
||||
M1 Mirror Example:
|
||||
|
||||
M1_Blank.prt ─────────────────────> M1_Blank_fem1.fem ─────────┐
|
||||
│ │ │
|
||||
│ (expressions) │ (component mesh) │
|
||||
↓ ↓ │
|
||||
M1_Vertical_Support_Skeleton.prt ──> M1_..._Skeleton_fem1.fem ─┤
|
||||
│
|
||||
↓
|
||||
ASSY_M1_assyfem1.afm ──> ASSY_M1_assyfem1_sim1.sim
|
||||
(assembly mesh) (solution)
|
||||
```
|
||||
|
||||
## API Functions Used
|
||||
|
||||
| Step | NX API Call | Purpose |
|
||||
|------|-------------|---------|
|
||||
| 1 | `OpenBase()` | Open .prt file |
|
||||
| 1 | `ImportFromFile()` | Import expressions from .exp file (preferred) |
|
||||
| 1 | `DoUpdate()` | Rebuild geometry |
|
||||
| 2-3 | `UpdateFemodel()` | Regenerate mesh from geometry |
|
||||
| 3 | `DuplicateNodesCheckBuilder` | Merge coincident nodes at interfaces |
|
||||
| 3 | `MergeOccurrenceNodes = True` | Critical: enables cross-component merge |
|
||||
| 4 | `SolveAllSolutions()` | Execute FEA (Foreground mode recommended)
|
||||
|
||||
### Expression Update Method
|
||||
|
||||
The recommended approach uses expression file import:
|
||||
|
||||
```python
|
||||
# Write expressions to .exp file
|
||||
with open(exp_path, 'w') as f:
|
||||
for name, value in expressions.items():
|
||||
unit = get_unit_for_expression(name)
|
||||
f.write(f"[{unit}]{name}={value}\n")
|
||||
|
||||
# Import into part
|
||||
modified, errors = workPart.Expressions.ImportFromFile(
|
||||
exp_path,
|
||||
NXOpen.ExpressionCollection.ImportMode.Replace
|
||||
)
|
||||
```
|
||||
|
||||
This is more reliable than `EditExpressionWithUnits()` for batch updates.
|
||||
|
||||
## Error Handling
|
||||
|
||||
Common issues and solutions:
|
||||
|
||||
### "Update undo happened"
|
||||
- Geometry update failed due to constraint violations
|
||||
- Check expression values are within valid ranges
|
||||
- May need to adjust parameter bounds
|
||||
|
||||
### "This operation can only be done on the work part"
|
||||
- Work part not properly set before operation
|
||||
- Use `SetWork()` to make target part the work part
|
||||
|
||||
### Node merge warnings
|
||||
- Manual intervention may be needed for complex interfaces
|
||||
- Check mesh connectivity in NX after solve
|
||||
|
||||
### "Billion nm" RMS values
|
||||
- Indicates node merging failed - coincident nodes not properly merged
|
||||
- Check `MergeOccurrenceNodes = True` is set
|
||||
- Verify tolerance (0.01 mm recommended)
|
||||
- Run node merge after every FEM update, not just once
|
||||
|
||||
## Configuration
|
||||
|
||||
The workflow auto-detects assembly FEMs, but you can configure behavior:
|
||||
|
||||
```json
|
||||
{
|
||||
"nx_settings": {
|
||||
"expression_part": "M1_Blank", // Override auto-detection
|
||||
"component_fems": [ // Explicit list of FEMs to update
|
||||
"M1_Blank_fem1.fem",
|
||||
"M1_Vertical_Support_Skeleton_fem1.fem"
|
||||
],
|
||||
"afm_file": "ASSY_M1_assyfem1.afm"
|
||||
}
|
||||
}
|
||||
```
|
||||
|
||||
## Implementation Reference
|
||||
|
||||
See `optimization_engine/solve_simulation.py` for the full implementation:
|
||||
|
||||
- `detect_assembly_fem()` - Detects if assembly workflow needed
|
||||
- `update_expressions_in_part()` - Step 1 implementation
|
||||
- `update_fem_part()` - Step 2 implementation
|
||||
- `update_assembly_fem()` - Step 3 implementation
|
||||
- `solve_simulation_file()` - Step 4 implementation
|
||||
|
||||
## Tips
|
||||
|
||||
1. **Start with baseline solve**: Before optimization, manually verify the full workflow completes in NX
|
||||
2. **Check mesh quality**: Poor mesh quality after updates can cause solve failures
|
||||
3. **Monitor memory**: Assembly FEMs with many components use significant memory
|
||||
4. **Use Foreground mode**: For multi-subcase solutions, Foreground mode ensures all subcases complete
|
||||
Reference in New Issue
Block a user