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Pitfalls

This document is the most valuable part of the project — every item was actually hit, and most were only understood after independent readback.

1. errStatus == 0 does not always mean success

The last out-parameter of IAssemblyDoc.AddMate5 is swAddMateError_e:

swAddMateError_ErrorUknown         = 0
swAddMateError_NoError             = 1     ← success is 1, not 0
swAddMateError_IncorrectSelections = 4

Lesson: don’t assume “0 means success”. Look up the enum, don’t guess.

2. IBody2.Operations2 only accepts API temporary bodies

Boolean-intersecting two document bodies directly:

Operations2(SWBODYINTERSECT=15901, toolBody, out err)
→ returns (None, 1)

In swBodyOperationError_e, 1 is swBodyOperationNonApiBody.

Fix:

ta = body_a.Copy2(False)      # IsTemporaryBody() → True
tb = body_b.Copy2(False)
res = ta.Operations2(15901, tb, 0)   # pass a plain int for the out-param
arr, code = res                       # returns (result, errorcode)

Another trap: passing VARIANT(VT_BYREF|VT_I4) for the out-param raises TypeError: int() argument must be ... not 'VARIANT'. Pass a plain int.

3. Late binding cannot reach some face / edge / vertex methods

Call pywin32 late binding C# early binding
IFace2.GetSurface() ❌ member not found ✅
IEntity.Select4() ❌ type mismatch ✅
IVertex.GetPoint() ❌ TypeError ✅
IComponent2.GetBodies2(0) ⚠️ wrong parameter count ✅

Conclusion: anything touching faces, edges, vertices or components must go through generated C#.

Note: IFace2 does not inherit IEntity in the interop, but the underlying Face2 COM object supports the IEntity QI, so in C# you write (IEntity)(object)face.

4. SolidWorks does not register in the ROT

Marshal.GetActiveObject("SldWorks.Application") only succeeds when SolidWorks was started interactively. When it is launched in the background through COM Dispatch:

COMException 0x800401E3 (MK_E_UNAVAILABLE)

Fix: two-level fallback

try { sw = (ISldWorks)Marshal.GetActiveObject("SldWorks.Application"); }
catch { sw = (ISldWorks)Activator.CreateInstance(Type.GetTypeFromProgID("SldWorks.Application")); }

And do a real round-trip probe (RevisionNumber() + GetDocumentCount()), because Activator.CreateInstance sometimes returns an empty shell proxy — checking only for non-null gives a false positive.

5. The material library must live in a directory SolidWorks scans

The same .sldmat file:

Location Result
E:\...\lang\chinese-simplified\sldmaterials\ ✅ works
%LOCALAPPDATA%\swforge\ ❌ fails silently, density falls back to 1000
C:\ProgramData\SOLIDWORKS\SOLIDWORKS <year>\自定义材料\ ✅ works

Also, SolidWorks’ bundled Chinese library has no GB grades (no Q235 / 45 / 40Cr), so you have to generate them. Generate by cloning material nodes from the native library and changing only the name and DENS/EX/NUXY — hand-written XML is rejected as an invalid library.

6. Convert units once, at the boundary

IAssemblyDoc.AddComponent5(path, ..., X, Y, Z) expects metres, while this project’s convention is millimetres. Without conversion, a part lands 60 metres away — and that also silently invalidated the “5 mm overlap” interference test, which could never detect an overlap.

Convention: millimetres everywhere outside COM; divide by 1000 going in, multiply coming out.

7. _value() calling a method that requires arguments

The generic wrapper _value(obj, name) calls value() with no arguments. For COM methods that need arguments (like GetUserPreferenceInteger(47, 0)) this raises “the parameter is not optional”.

Fix: call parameterized methods explicitly, don’t route them through the generic wrapper.

8. except: continue disguises “could not read” as “does not exist”

An early _view_list() used md.GetViews, which returns a native PyIDispatch; attribute access threw, and except: continue swallowed it — so the counting function always returned 0 views while callers saw nothing wrong.

Fix: switch to the GetFirstView() linked list; and anywhere you catch and continue, leave a visible failure signal.

9. The drawing template decides units and frame

E:\...\data\templates\GB.drwdot is an English template: inches, no GB sheet format. C:\ProgramData\...\templates\gb_a3.drwdot is the Chinese one: millimetres, a3 - gb.slddrt.

Using the wrong template shows up as 100 mm rendered as 3.94 (inches) and a sheet with no border or title block.

10. InsertModelAnnotations4 does not give overall dimensions

It inserts model driving dimensions. A part made of “one base plate + four plates welded into a tube” only has a dozen of them, and SolidWorks deduplicates them across views (which is why a top view often legitimately shows 0 dimensions). Measured cap:

  1. And they are frequently vertical-only.

Overall dimensions must be added explicitly: take IView.GetVisibleEntities2(null, swViewEntityType_Vertex=2), find the extreme vertices by model coordinate, select them, then call AddHorizontalDimension2 / AddVerticalDimension2.