# 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