from __future__ import annotations import asyncio from pathlib import Path from typing import Any from solidworks_mcp.adapters import create_adapter from solidworks_mcp.adapters.base import ExtrusionParameters from solidworks_mcp.config import load_config ROOT = Path(__file__).resolve().parents[3] ARTIFACT_DIR = ROOT / "docs" / "getting-started" / "tutorial-parts" OUTPUT_PART = ARTIFACT_DIR / "yoke_female_from_prompt.SLDPRT" OUTPUT_IMAGE = ARTIFACT_DIR / "yoke_female_from_prompt_isometric.png" ANSWER_KEY = Path( r"C:\Users\Public\Documents\SOLIDWORKS\SOLIDWORKS 2026\samples\learn\U-Joint\Yoke_female.sldprt" ) ANSWER_KEY_IMAGE = ARTIFACT_DIR / "answer_key_yoke_female_isometric.png" # Dimensions from read_yoke_female_geometry.py reverse-engineering of the SW 2026 sample: # Base cylinder: dia=38.10mm (r=19.050), height=47.625mm, Top(XZ) plane at Y=0 # U-slot profile: Front(XY) plane — same 3 arcs + 4 walls as yoke_male, but outer # walls end at Y=0 (not Y=-1.366); bottom edge closes at Y=0 # Arm gap (slot): Right(YZ) plane, Z:+-10.160mm, Y:0..29.145mm (starts at Y=0, # not Y=-7.455mm like yoke_male) # Pin bore: Front(XY) plane, dia=9.525mm (r=4.7625), center (0,9.525), # through-all in Z (same as yoke_male) # Bolt holes: 4x dia=6.35mm (r=3.175) circles on top face at Y=47.625mm, # bolt circle r=12.700mm, at 0/90/180/270 deg (world X/Z axes), # cut ThroughAll into cylinder def require(result: Any, label: str) -> Any: if not result.is_success: raise RuntimeError(f"{label} failed: {result.error}") return result def unwrap_for_method(adapter: Any, method_name: str) -> Any | None: current: Any | None = adapter visited: set[int] = set() while current is not None and id(current) not in visited: visited.add(id(current)) if hasattr(current, method_name): return current current = getattr(current, "adapter", None) return None def create_sketch_on_offset_plane(adapter: Any, offset_mm: float) -> str: """Create a reference plane at offset_mm above the Top plane, open a sketch on it. Uses InsertRefPlane (swRefPlaneReferenceConstraints_Distance=8) which is more reliable than coordinate-based face selection after parametric cuts have been applied. Returns the offset plane feature name so it can be hidden later. """ raw = unwrap_for_method(adapter, "_handle_com_operation") if raw is None or raw.currentModel is None: raise RuntimeError("No active model for offset-plane sketch") def _op() -> str: from solidworks_mcp.adapters import sw_type_info model = raw.currentModel sw_type_info.flag_doc(model, 1) # Find the Top Plane feature by name (try both English and Spanish/localised) top_plane = None for name in ("Top Plane", "Top", "Planta", "Plano Superior"): try: top_plane = model.FeatureByName(name) if top_plane is not None: break except Exception: pass if top_plane is None: raise RuntimeError("Top plane feature not found") model.ClearSelection2(True) sw_type_info.flag_methods(top_plane, "IFeature") if not top_plane.Select2(False, 0): raise RuntimeError("Failed to select Top Plane for offset reference") # swRefPlaneReferenceConstraints_Distance = 8 offset_m = offset_mm / 1000.0 plane_feat = model.FeatureManager.InsertRefPlane(8, offset_m, 0, 0.0, 0, 0.0) if not plane_feat: raise RuntimeError(f"InsertRefPlane at {offset_mm}mm returned None") sw_type_info.flag_methods(plane_feat, "IFeature") plane_name = str(plane_feat.Name) model.ClearSelection2(True) if not plane_feat.Select2(False, 0): raise RuntimeError(f"Failed to select offset plane '{plane_name}'") raw.currentSketchManager = model.SketchManager raw._reset_sketch_entity_registry() try: sketch = raw.currentSketchManager.InsertSketch(True) except Exception: sketch = raw.currentSketchManager.InsertSketch() raw.currentSketch = sketch raw._sketch_count += 1 name = str(getattr(sketch, "Name", None) or f"Sketch_{raw._sketch_count}") raw._last_sketch_name = name return name result = raw._handle_com_operation(f"create_sketch_on_offset_{offset_mm}", _op) if not result.is_success: raise RuntimeError(f"create_sketch_on_offset_plane({offset_mm}) failed: {result.error}") return str(result.data) async def ensure_saved_part_active(adapter: Any, model_path: Path, label: str) -> None: require(await adapter.open_model(str(model_path)), label) async def build_part() -> None: config = load_config() adapter = await create_adapter(config) await adapter.connect() try: require(await adapter.create_part(name="yoke_female_from_prompt"), "create_part") # ── Sketch1: Base cylinder dia=38.10mm on Top plane (XZ at Y=0) ───────── # Identical to yoke_male. Extruded 47.625mm upward (+Y). require(await adapter.create_sketch("Top"), "create_sketch BaseCircle") require(await adapter.add_circle(0, 0, 19.050), "base circle r=19.050") require(await adapter.exit_sketch(), "exit_sketch BaseCircle") require( await adapter.create_extrusion(ExtrusionParameters(depth=47.625)), "BaseExtrude 47.625mm", ) # ── Sketch2: U-slot cut on Front plane (XY at Z=0) ────────────────────── # Same 3 arcs + 4 walls as yoke_male, but: # - Outer walls end at Y=0 (not Y=-1.366) # - Bottom closing edge at Y=0 (not Y=-1.366) # Read from SW sample: outer walls span Y=0..29.210mm. require(await adapter.create_sketch("Front"), "create_sketch USlot") # bottom_edge at Y=-0.5 (below the solid base): arc2 dips to Y=0 at (0,0); # if bottom_edge were at Y=0 the arc would create a sketch self-intersection # at (0,0) making the profile invalid. The cut result is identical since the # cylinder base is at Y=0 — anything below is already outside the solid. bottom_edge = require( await adapter.add_line(-19.050, -0.5, 19.050, -0.5), "bottom edge Y=-0.5" ) right_outer = require( await adapter.add_line(19.050, -0.5, 19.050, 29.210), "right outer" ) arc1 = require( await adapter.add_arc(19.050, 19.685, 19.050, 29.210, 9.525, 19.685), "right arm tip arc R9.525", ) right_inner = require( await adapter.add_line(9.525, 19.685, 9.525, 9.525), "right inner wall" ) arc2 = require( await adapter.add_arc(0, 9.525, -9.525, 9.525, 9.525, 9.525), "U-slot bottom arc R9.525", ) left_inner = require( await adapter.add_line(-9.525, 9.525, -9.525, 19.685), "left inner wall" ) arc3 = require( await adapter.add_arc(-19.050, 19.685, -9.525, 19.685, -19.050, 29.210), "left arm tip arc R9.525", ) left_outer = require( await adapter.add_line(-19.050, 29.210, -19.050, -0.5), "left outer" ) xaxis = require( await adapter.add_centerline(-19.050, 0, 19.050, 0), "X-axis centerline" ) require( await adapter.add_sketch_dimension(arc1.data, None, "radial", 9.525), "dim R9.525 right arm", ) require( await adapter.add_sketch_dimension(arc2.data, None, "radial", 9.525), "dim R9.525 U-bottom", ) require( await adapter.add_sketch_dimension(arc3.data, None, "radial", 9.525), "dim R9.525 left arm", ) require( await adapter.add_sketch_constraint(right_outer.data, None, "fix"), "fix right outer", ) require( await adapter.add_sketch_constraint(left_outer.data, None, "fix"), "fix left outer", ) require( await adapter.add_sketch_constraint(arc2.data, xaxis.data, "tangent"), "arc2 tangent to X-axis", ) require( await adapter.add_sketch_dimension(bottom_edge.data, None, "linear", 38.100), "dim bottom edge width 38.100mm", ) require( await adapter.add_sketch_dimension(right_inner.data, None, "linear", 10.160), "dim right inner 10.160mm", ) require( await adapter.add_sketch_dimension(left_inner.data, None, "linear", 10.160), "dim left inner 10.160mm", ) require(await adapter.exit_sketch(), "exit_sketch USlot") require( await adapter.create_cut_extrude( ExtrusionParameters(depth=0.0, end_condition="ThroughAll", both_directions=True) ), "USlot cut through-all-both", ) # ── Sketch8: Arm gap on Right plane (YZ at X=0) ────────────────────────── # Right-plane coords: sketch_x=world_Z, sketch_y=world_Y. # Female arm gap: Z:+-10.160mm, Y:0..29.145mm (starts at Y=0, not -7.455mm). require(await adapter.create_sketch("Right"), "create_sketch ArmGap") require(await adapter.add_line(-10.160, 0, 10.160, 0), "gap bottom Y=0") require(await adapter.add_line(10.160, 0, 10.160, 29.145), "gap right") require(await adapter.add_line(10.160, 29.145, -10.160, 29.145), "gap top") require(await adapter.add_line(-10.160, 29.145, -10.160, 0), "gap left") require(await adapter.exit_sketch(), "exit_sketch ArmGap") require( await adapter.create_cut_extrude( ExtrusionParameters(depth=0.0, end_condition="ThroughAll", both_directions=True) ), "ArmGap cut through-all-both", ) # ── Sketch11: Pin bore dia=9.525mm on Front plane (XY at Z=0) ─────────── # Front-plane coords: sketch_x=world_X, sketch_y=world_Y. # Circle at (0, 9.525): cross-pin hole at Y=9.525mm. Identical to yoke_male. require(await adapter.create_sketch("Front"), "create_sketch PinBore") require(await adapter.add_circle(0, 9.525, 4.7625), "pin bore r=4.7625mm") require(await adapter.exit_sketch(), "exit_sketch PinBore") require( await adapter.create_cut_extrude( ExtrusionParameters(depth=0.0, end_condition="ThroughAll", both_directions=True) ), "PinBore cut through-all-both", ) # ── Sketch12: Bolt holes on top face (Y=47.625mm) ───────────────────────── # 4x dia=6.35mm (r=3.175mm) bolt holes on a r=12.700mm bolt circle. # Arranged at 0/90/180/270 deg (world X and Z axes) on the top face. # Use a reference plane offset from Top by 47.625mm to avoid unreliable # coordinate-based face selection after parametric cuts. # Sketch plane coords (offset plane parallel to Top): sketch_x=world_X, sketch_y=world_Z. # Cut ThroughAll downward (-Y) into the cylinder body. create_sketch_on_offset_plane(adapter, 47.625) BOLT_R = 12.700 # bolt circle radius HOLE_R = 3.175 # hole radius (dia=6.35mm) require(await adapter.add_circle(BOLT_R, 0, HOLE_R), "bolt hole +X") require(await adapter.add_circle(0, BOLT_R, HOLE_R), "bolt hole +Z") require(await adapter.add_circle(-BOLT_R, 0, HOLE_R), "bolt hole -X") require(await adapter.add_circle(0, -BOLT_R, HOLE_R), "bolt hole -Z") require(await adapter.exit_sketch(), "exit_sketch BoltHoles") require( await adapter.create_cut_extrude( ExtrusionParameters( depth=0.0, end_condition="ThroughAll", both_directions=False, reverse_direction=True, ) ), "BoltHoles cut ThroughAll into cylinder", ) # ── Save and export ─────────────────────────────────────────────────────── require(await adapter.save_file(str(OUTPUT_PART)), "save_file") await ensure_saved_part_active(adapter, OUTPUT_PART, "reopen for screenshot") require( await adapter.export_image( { "file_path": str(OUTPUT_IMAGE), "format_type": "png", "width": 1600, "height": 1000, "view_orientation": "isometric", } ), "export_image", ) if ANSWER_KEY.exists(): require(await adapter.open_model(str(ANSWER_KEY)), "open answer key") require( await adapter.export_image( { "file_path": str(ANSWER_KEY_IMAGE), "format_type": "png", "width": 1600, "height": 1000, "view_orientation": "isometric", } ), "export_image answer key", ) await ensure_saved_part_active(adapter, OUTPUT_PART, "restore tutorial part") finally: await adapter.disconnect() if __name__ == "__main__": ARTIFACT_DIR.mkdir(parents=True, exist_ok=True) asyncio.run(build_part()) print(OUTPUT_PART) print(OUTPUT_IMAGE) print(ANSWER_KEY_IMAGE)