GHCAD

GHCAD · CAM 7

UNTESTED CAM – BETA. NOT VERIFIED ON A MACHINE. USE AT YOUR OWN RISK. Check NC, controller cycles, tool offsets, datum, workholding and travel in the machine simulator before running. The path preview is not verified machine/fixture collision or stock-removal simulation.

1. Setup & orientation

Open CAM under Tools for the active part. Choose 3-axis milling, 2-axis turning or laser/plasma. Set the setup face, rotation and placement. Turning supports front/back flipping and an X/Y/Z axis for an imported rotationally symmetric model. Revolved sketches use their construction axis. Milling Z0 is stock top; turning Z0 is part front and X uses diameter programming. Choose G54–G59.

+ Setup adds Setup 2 while retaining Setup 1. Each setup has independent stock, placement, tools and operations. Calculate/export one setup at a time. Remaining material is not automatically transferred between setups; define the new blank.

2. Stock / blank

Milling accepts rectangular or round stock. Turning uses diameter, length, facing allowance and chuck clearance. Load a STEP blank reference for milling (at most 2 MB / 15,000 triangles). Calculation and stock volume use the STEP body's enclosing rectangular blank. The STEP body is shown as a reference; exact remaining material of its freeform shape is not simulated. Check stock/part placement in the view.

3. Tool library

Presets include end/face/ball/taper/taper-ball mills, HSS/carbide/spot drills, V-bits, taps, thread mills, CNMG/DCMT/VNMG inserts, boring bars, grooving/threading/parting inserts. Edit diameter, tip, nose radius, angle, flute length, shank, holder and flute count. Show tool geometry provides a simplified illustration, not a collision model.

Cutting presets are editable starting values, not manufacturer-verified recommendations. Calculate them from Vc and chip load/feed per revolution, or enter RPM, feed, plunge, depth and stepover. Selecting a tool applies its preset to the operation; operation data may then be edited independently. Match T/H/D offsets to the machine.

Export tool library saves a separate JSON file. Import tool library loads it next time. Import replaces an empty setup's library; an import missing tools used by operations is rejected. Edits also save the library locally; Load my saved library restores it. Save project includes setup tools in the single .ghcad file. Local storage is specific to the browser/domain; export makes the library portable.

4. Toolpaths

Automatic planning proposes operations in an empty setup. Review and edit the proposal. Add/copy/reorder/disable/delete operations in the tree. Select tool, geometry and cutting data per operation. Pocket floor faces can be selected in the view. Recalculate after edits; geometric selections must be reviewed after model changes.

ProcessOperations in this beta
3-axis millingFacing, 3D roughing, pockets, outside/inside profiles, 3D finishing, drilling, helical/circular boring, G84 tapping, internal thread milling, chamfering, engraving, V-carve.
2-axis turningFacing, OD rough/finish, drilling, ID boring profile, OD and manually defined ID grooves/reliefs, nominal 60° threading and parting. Rotational symmetry is required. AN hex bodies use a circumferential turning envelope and require separate milling. Reliefs are left for the grooving tool.
Laser / plasmaClosed 2D/DXF profiles and open centerline marking. Inside profiles first; kerf, power, pierce delay and cut/pierce height.

Kerf, start point and lead-in/out

Kerf modes: automatic (inside holes/outside perimeter), inside, outside or off/centerline. Compensation is calculated in the path: do not add machine G41/G42. Pick a start on the green profile or select its contour index and percentage along it. Lead-in and lead-out are separate straight waste-side moves. Set either to 0 mm to disable it and start/stop on the contour. Leads crossing finished geometry or leaving stock are rejected; reposition or shorten them. Marking follows the centerline.

V-carve

Closed XY outlines use V-bit angle and tip diameter to vary depth with available profile width, capped by maximum depth. This beta uses inward contour offsets with editable radial resolution (0.02–0.5 mm), not an exact medial-axis solver. Narrow centers may leave residual material up to the resolution. Review finish and cut a sample for critical work. Ordinary engraving uses constant depth.

Time, output and project save

Calculate displays paths/playback and estimated machine time at the bottom. Time includes commanded cutting, rapids, dwell and 10 seconds per tool load/change, including initial loading. An RPM-only change is not a tool change. No setup time is included. Acceleration and controller-specific delays are not modelled.

Export NC + setup sheet creates one ZIP for the active setup: generic Fanuc/ISO NC, printable HTML setup sheet and CAM JSON. The sheet includes time, blank volume/material, work offset, orientation, tool geometry and operation data. Print or save as PDF from the browser. Save project includes every part and its CAM setups in one file. Paths are recalculated after reopening.

Scope & licences

This is not support for every possible operation or controller. Undercuts inaccessible in a 3-axis setup require another setup. Holder/fixture collisions are not verified. Chamfer/engraving paths use XY sketches. Tapping requires correct pilot holes and machine cycles. Turning threads do not verify UNJ root form, thread class or sealing standards. STEP blanks use enclosing rectangular stock. Verify the post for your machine.

Licences, attribution and adapted CAM source are included. The existing CAD engine has separate LGPL terms. CAM is exclusive to GHCAD; GH Performance Design Studio remains without CAM.

Version 8 changes

Tool library opens in its own movable dialog. Choose an operation from the grouped cards. Turning defaults to horizontal 3D with Z+ to the right; the 2D view changes display only. No work-offset code omits G54–G59.

Surface selection is per operation: roughing/pockets use upward planar floor faces; 3D finishing uses the selected XY projections with the complete model retained for tool clearance. Turning rough/finish selections restrict axial spans around the full circumference. No selection means all applicable geometry. New operations start without selections or depth limits. Selected surfaces must be reviewed after geometry changes.

Bottom plane (milling) and Z stop plane (turning) belong to each operation, in the selected datum. An operation that crosses the limit is rejected rather than silently altered. This does not detect fixture, holder or chuck collisions. Nine-point stock datum selection and machine axis mapping affect exported NC; confirm the actual machine datum.

Automatic milling proposes individual detected sketch holes, planar pocket faces and finally outside contour; recognition is incomplete. Check hole depths and missing features. Global level roughing is manual and no longer appends a flat-surface pass. Automatic turning ends with parting off.

Tool material starting data covers aluminium, mild steel, stainless, brass and plastic. Use the explicit starting-data button to replace tool presets. Saved manual values are retained. Turning speed calculation uses stock diameter; tapping feed follows pitch. These are generic estimates, not manufacturer-approved settings.

Laser/plasma leads may be straight or tangent quarter arcs. Arc values specify radius; zero disables the lead. Manual starts are projected onto the compensated contour. Validate arc direction and I/J support for the controller.

V-carve accepts closed splines (adaptive Bezier flattening at 0.01 mm) and mixed line/spline boundaries. Rough offset levels are followed by adaptive raster finishing with varying Z based on local boundary clearance, V-angle, tip size and maximum depth. Broad regions become deeper than narrow tips; inner islands remain. A half-resolution radial margin is left. This is approximate, not an exact medial-axis solver or a rendered stock-removal simulation. Through cuts are separate operations. Increase radial resolution value for very dense designs. Arbitrary 3D relief is not supported by this V-carve method.

Dense mesh preview now draws every triangle. A real browser visual/performance acceptance test and physical cutting test are still required.

Version 10: setup orientation, graphics and machine profile

New milling setups try the largest planar face as XY, with Z out of the face. Existing saved setups are retained. Stock datum includes Pick XY plane on model; click a planar face and return to the nine-point datum dialog. Front, back, left, right, top and bottom follow this setup frame. Flip the plane normal if required. Manual stock sizes remain manual; review dimensions, hole positions, face selections and workholding after reorientation.

Laser/plasma automatically maps the original XY/XZ/YZ sketch plane flat. Solid preview, blank and cutting contours use the same transformation, including top/bottom and Z rotation. The auto-orient sketch plane button resets the sketch-plane mapping.

Preview uses a WebGL depth buffer where available, smooth shading within CAD faces, nearest visible face picking, screen-relative orbit and cursor-centred zoom. Paths no longer omit every nth segment. WCS has labelled coloured arrows. A canvas fallback is used if WebGL is unavailable. This is not a stock-removal or collision simulation. Real-browser visual/performance acceptance remains required.

Optional machine profile: emco pcturn 120, for turning only. Generic Fanuc/ISO remains default. The imported ERP configuration is included as assets/emco-pcturn-120-erp.json. Export uses ERP unit/start/tool/home conventions, numbered CRLF NC (.nc), optional M8/M9 and M00 for drilling. Explicit paths are retained; thread passes use G33 from the existing Emco/eCAM post. ERP canned G73/G72/G78 cycle conversion and constant-surface-speed output are not implemented here. Standard axis mapping is required, maximum spindle speed 4000 rpm. Selecting the profile clears work-offset code; check actual tool stations, offsets, datum and controller before running.

GHCAD defaults to English on all hosts, including local testing. A saved explicit Swedish/English choice is retained. The module title is CAM - Beta; untested-machine warnings remain.

Version 11

Inside roughing runs inside-out toward the inner wall; Outside roughing runs outside-in toward the final outer boundary. This ordering applies only to roughing, not finishing or other operations. Allowance remains. Select one or multiple floor faces, hole walls or closed edge loops; depth and operation bottom plane are independent. Through openings do not need a floor. Selected walls identify their closed section; disconnected/open edge chains are rejected. Curves and areas are approximated from the CAD mesh. Complex surfaces may require an explicit closed boundary.

The same geometry selection is available for pockets, face milling, inside/outside profiles and 3D finishing where applicable. No selection uses all applicable geometry. Outside roughing clears stock outside the part, not its holes. Surface selection and depth limits belong only to the selected operation. Geometry changes require review.

Entry methods: Linear ramp (default), Helical and Plunge. Set maximum ramp angle and helical radius. Linear entry follows the existing toolpath, back and forth for open paths. Helical entry is checked conservatively against model/stock and selected area. Some short, isolated V-carve strokes and open 3D-finishing paths cannot accept the requested ramp; calculation then stops and asks for another entry method. It never silently changes to plunge. Drilling, tapping, threading and countersinking retain their own axial/process feed. Collision checks do not certify holder/chuck/fixture clearance or residual stock.

Circular boring supports a larger top diameter and smaller bottom diameter, including a tapered helical finish pass. Pick an internal cylindrical/conical face or enter dimensions. Undercuts are rejected. Countersinking is a separate operation with countersink tools (82/90-degree presets); target diameter, tool angle and tip diameter determine tool-tip depth. Verify pilot-hole depth. A selected cone must match the countersink angle.

Library geometry fields depend on tool type. An end mill does not show insert width or insert access angles. Stepover is entered as percent of diameter (35 means 35%). User tool names remain saved. English library text and setup sheet notes are updated; setup sheet follows the chosen English/Swedish export language.

Arc lead-in/out now have independent 30–180-degree sweep angles, default 135 degrees. Radius and zero-disable remain. NC exports always use .nc, including Emco. Turning finish reliefs use one radial X plunge and an axial finish pass when the insert fits, assuming the relief is already roughed. Rough reliefs retain stepped plunges.