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_male_from_prompt.SLDPRT" OUTPUT_IMAGE = ARTIFACT_DIR / "yoke_male_from_prompt_isometric.png" ANSWER_KEY = Path( r"C:\Users\Public\Documents\SOLIDWORKS\SOLIDWORKS 2026\samples\learn\U-Joint\Yoke_male.sldprt" ) ANSWER_KEY_IMAGE = ARTIFACT_DIR / "answer_key_yoke_male_isometric.png" # Dimensions from read_yoke_geometry.py reverse-engineering of the SW 2026 sample: # Base cylinder: dia=38.10mm (r=19.050), height=47.625mm (1-7/8"), Top(XZ) plane at Y=0 # Arm gap (slot): Right(YZ) plane, slot Z:±10.160mm, Y:-7.455 to 29.145mm, through-all in X # U-slot profile: Front(XY) plane, complex arcs+lines (see Sketch2 in reader output) # Pin bore: Front(XY) plane, dia=9.525mm (r=4.7625), center (0,9.525), through-all in Z # Stub shaft: Top(XZ) at Y=47.625mm, dia=12.70mm (r=6.350), extrude to Y=66.675mm (19.05mm) # Stub bore: Face1 (top of stub after chamfer), D-profile r=6.350 + chord at X=4.763 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_face_y(adapter: Any, y_mm: float) -> str: """Select the face at world Y=y_mm (on the Z=0 axis) and open a sketch on it. SelectByID2 requires a Callout parameter typed as ICallout*. Passing Python None marshals as VT_NULL which SolidWorks rejects; instead we pass a VT_DISPATCH null VARIANT (win32com.client.VARIANT(VT_DISPATCH, None)) which matches the expected COM null-pointer type. Runs through _handle_com_operation to respect the COM STA thread invariant. Returns the sketch name. """ raw = unwrap_for_method(adapter, "_handle_com_operation") if raw is None or raw.currentModel is None: raise RuntimeError("No active model for face sketch") def _op() -> str: import pythoncom import win32com.client as _win32 model = raw.currentModel y_m = y_mm / 1000.0 null_callout = _win32.VARIANT(pythoncom.VT_DISPATCH, None) # Clear any lingering sketch/feature selection from the previous operation, # then rebuild so new faces from recent features are fully tessellated and # selectable. Without this, SelectByID2("", "FACE", ...) may return False # even when the face geometrically exists. try: model.ClearSelection2(True) except Exception: pass try: model.ForceRebuild3(True) except Exception: pass # Try a set of candidate (x, z) offsets in case the exact center misses. # The face of interest (top cap) has radius r ≈ 19mm; any interior point works. # Also try both Extension.SelectByID2 and the model-level SelectByID2. candidate_xz = [ (0.0, 0.0), (0.005, 0.0), (-0.005, 0.0), (0.0, 0.005), (0.0, -0.005), (0.008, 0.008), (0.010, 0.0), (0.0, 0.010), (0.015, 0.015), ] selected = False for cx, cz in candidate_xz: for sel_fn in ( lambda cx=cx, cz=cz: model.Extension.SelectByID2( "", "FACE", cx, y_m, cz, False, 0, null_callout, 0 ), lambda cx=cx, cz=cz: model.SelectByID2( "", "FACE", cx, y_m, cz, False, 0, null_callout, 0 ), ): try: selected = bool(sel_fn()) except Exception: selected = False if selected: break if selected: break if not selected: raise RuntimeError(f"SelectByID2 FACE at Y={y_mm}mm returned False for all candidate points") 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_face_y{y_mm}", _op) if not result.is_success: raise RuntimeError(f"create_sketch_on_face_y({y_mm}) failed: {result.error}") return str(result.data) def chamfer_edge_at(adapter: Any, wx_mm: float, wy_mm: float, wz_mm: float, distance_mm: float) -> None: """Chamfer the edge nearest to world coordinates. Non-fatal on failure.""" raw = unwrap_for_method(adapter, "_handle_com_operation") if raw is None or raw.currentModel is None: return def _op() -> str: model = raw.currentModel selected = model.Extension.SelectByID2( "", "EDGE", wx_mm / 1000.0, wy_mm / 1000.0, wz_mm / 1000.0, False, 0, None, 0, ) if not selected: raise RuntimeError(f"Failed to select edge at ({wx_mm}, {wy_mm}, {wz_mm})mm") fm = model.FeatureManager feature = fm.FeatureChamfer( 1, distance_mm / 1000.0, distance_mm / 1000.0, 0, 0, False, False, False, False, ) if not feature: raise RuntimeError("FeatureChamfer returned None") return str(feature.Name) result = raw._handle_com_operation("chamfer_edge", _op) if not result.is_success: print(f"[warn] Chamfer skipped: {result.error}") 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_male_from_prompt"), "create_part") # ── Sketch1: Base cylinder ∅38.10mm on Top plane (XZ at Y=0) ───────────── # Extruded 47.625mm upward (+Y). The cylinder forms the yoke body and arm zone. # Arm zone: Y=0..29.145mm (the U-fork). Shaft zone: Y=29.145..47.625mm. require(await adapter.create_sketch("Top"), "create_sketch BaseCircle") require(await adapter.add_circle(0, 0, 19.050), "base circle dia=38.10mm") 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) ────────────────────── # Closed loop of 5 lines + 3 arcs. Removes the arm-strip regions (X>9.525 # and X<-9.525) from the cylinder below Y=29.210, leaving the centre # X=±9.525 as the arm material with rounded arm tips. # Radial dimensions required to fully define the sketch for FeatureCut. # Arc CCW direction (Dir=1): confirmed by angle traversal: # right arm: 90°→180° (top→left, short arc) # U-bottom: 180°→270°→0° (left→bottom(0,0)→right, 180° arc) # left arm: 0°→90° (right→top, short arc) require(await adapter.create_sketch("Front"), "create_sketch USlot") bottom_edge = require( await adapter.add_line(-19.050, -1.366, 19.050, -1.366), "bottom edge" ) right_outer = require(await adapter.add_line(19.050, -1.366, 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, -1.366), "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 wall", ) require( await adapter.add_sketch_constraint(left_outer.data, None, "fix"), "fix left outer wall", ) require( await adapter.add_sketch_constraint(arc2.data, xaxis.data, "tangent"), "arc2 tangent to X-axis (bottom at origin)", ) 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 wall height 10.160mm", ) require( await adapter.add_sketch_dimension(left_inner.data, None, "linear", 10.160), "dim left inner wall height 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 rectangular slot on Right plane (YZ at X=0) ───────── # Right-plane coords: sketch_x=world_Z, sketch_y=world_Y. # Removes material at Z:±10.160mm, Y:-7.455..29.145mm through-all in X. # This creates the two yoke arms (front arm Z>10.160, back arm Z<-10.160). require(await adapter.create_sketch("Right"), "create_sketch ArmGap") require(await adapter.add_line(-10.160, -7.455, 10.160, -7.455), "gap bottom") require(await adapter.add_line(10.160, -7.455, 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, -7.455), "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 ∅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): the cross-pin hole at Y=9.525mm (arm height). # Through-all in Z passes through both front and back arms. require(await adapter.create_sketch("Front"), "create_sketch PinBore") require(await adapter.add_circle(0, 9.525, 4.7625), "pin bore dia=9.525mm") 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: Stub shaft ∅12.70mm on Top plane ──────────────────────────── # The target model starts Boss-Extrude2 from Face<1> (top of base cylinder # at Y=47.625mm) and extrudes 19.05mm. We achieve identical geometry by # sketching on the Top plane and extruding 66.675mm: the first 47.625mm of # the r=6.350mm column merges invisibly into the base cylinder (r=19.050mm); # only the top 19.05mm (Y=47.625..66.675mm) protrudes as the stub shaft. # This avoids face-selection issues with the parametric base-cylinder face. require(await adapter.create_sketch("Top"), "create_sketch StubShaft") require(await adapter.add_circle(0, 0, 6.350), "stub shaft dia=12.70mm") require(await adapter.exit_sketch(), "exit_sketch StubShaft") require( await adapter.create_extrusion( ExtrusionParameters(depth=66.675) ), "StubExtrude 66.675mm from Top (net protrusion 19.05mm above base)", ) # ── Sketch13: Stub bore D-profile on Face<1> (top of stub shaft) ─────────── # Sketch on the top face of the stub shaft at Y=66.675mm. ThroughAll Direction 1 # cuts downward (-Y) through the 19.05mm stub. No both_directions needed. # D-profile = long CCW arc (≈277°, around left side) + chord line closing it. # Arc: center=(0,0) r=6.350, CCW from (4.763,4.200) to (4.763,-4.200). # Chord: closes from arc-end back to arc-start at X=4.763. # No radial dimension — coordinates already approximate r=6.350; adding a # driven dimension shifts endpoints and opens the closed profile. create_sketch_on_face_y(adapter, 66.675) require( await adapter.add_arc(0, 0, 4.763, 4.200, 4.763, -4.200), "D-bore arc CCW long", ) require(await adapter.add_line(4.763, -4.200, 4.763, 4.200), "keyway chord") require(await adapter.exit_sketch(), "exit_sketch StubBore") require( await adapter.create_cut_extrude( ExtrusionParameters(depth=0.0, end_condition="ThroughAll", both_directions=False) ), "StubBore cut ThroughAll into stub", ) # ── 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)