CAD/CAMCAD/CAM

You create the shape in CAD, create how to cut it (the tool's path) in CAM, and a post-processor turns it into an NC program the machine can read. This page explains the differences between CAD, CAM, and CAE and the flow from 3D model to machining, checked against public materials from software makers and public institutions.

The CAM workflow has
8 steps. Let's start with
the big picture!

Illustration: CAD/CAM — Illustration (not an exact drawing)

⌗Differences between CAD, CAM, and CAE

CAD (computer-aided design)

Computer-Aided Design

The work, and the software, of creating, editing, and examining the 2D and 3D shape of a part on a computer and turning it into drawings and other documents. It replaces the drafting board and hand drawing.One source / reference^[1]

CAM (computer-aided manufacturing)

Computer-Aided Manufacturing

In the narrow sense, creating the commands that run a CNC machine tool (G-code, etc.) with software. In the broad sense, it also covers machining planning, preparing the CAD model, NC programming, machine simulation, post-processing, and transfer to the shop floor (DNC, etc.).^[2][3]

CAE (computer-aided engineering)

Computer-Aided Engineering

The work of using software to simulate a product's performance (strength, heat, flow, etc.) and check whether the design is good. It proceeds in three stages: pre-processing (entering shape, materials, and loads), solving (solver), and post-processing (viewing results).One source / reference^[4]

Integrated CAD/CAM and standalone CAM

integrated CAD/CAM vs standalone CAM

Integrated systems where CAM runs inside CAD (Fusion, SOLIDWORKS CAM, Creo's machining functions, Onshape CAM Studio, etc.) make it easy for toolpaths to follow when you change the shape. Standalone CAM and CAM embedded in another vendor's CAD (hyperMILL's SOLIDWORKS and Inventor integration, SolidCAM, etc.) are strong in accepting data from any CAD.^{[5][6][7][8][9][10][11][12]}

→CAM workflow (from 3D model to machine)

The red “Common mistake” notes show mistakes likely to occur at that step (for the checklist of common mistakes, see theCoordinate systems, post, DNC page).

Prepare the 3D model
- Create it in your own CAD, or receive it from the customer as an intermediate file such as STEP. Check first that the received data has closed faces forming a solid (faces that do not close need repair).^[3][13][2]
Related:Data formats,Drafting
Define the stock and coordinate system (work origin)
- Enter the stock size and shape, and set the position and axis directions of the program origin (work coordinate system, WCS). The origin you set here is the point to match to the machine's work coordinate system, such as G54.^{[14][3][15][16]}
Related:G54–G59,G90
Choose tools and cutting conditions
- Choose the tool (diameter, flute length, holder) from the tool library and enter speed, feed, and depth of cut. If you store conditions in the tool library, you do not have to re-enter them every time.^{[3][7][9][16]}
Related:Tooling,Calculators
Create the toolpath (tool path)
- In the order roughing → semi-finishing → finishing → rest machining, choose a machining method suited to the shape (contour, pocket, waterline, raster, etc.) and have the toolpath calculated.^{[17][18][19][3][20]}
Check with simulation
- Check on screen how the stock is cut away, and collisions between tool, holder, fixture, and machine. Besides the simulation inside CAM, there is also verification software (VERICUT, NCVIEW, etc.) that reads the post-processed NC program itself.^{[21][22][23][24][3]}
Make the NC program with the post-processor
- Convert the path data in CAM (CL data) into an NC program in the format of the machine and NC control you use. Choose a post suited to each machine.^{[25][3][26][21]}
Related:G/M code dictionary
Send it to the machine (memory operation, DNC)
- Load the NC program into the NC control by USB, LAN, RS-232C, etc., and run it. For large programs that do not fit in the control's memory, use DNC operation, which machines while feeding the program from an external source.^[27][2]
Related:DNC operation and memory operation
Check on the machine before cutting
- Set the tool length and work coordinate system on the machine, and check the motion using the NC control's graphic display and safe-operation functions before starting the actual cut. The most common causes of a first-run collision are mistakes in tool offset or work coordinate settings, and the wrong tool in the spindle.^[16][28][15]
Related:G43,G54–G59

◇Types of CAM

2.5D

3-axis

3+2 (indexed 5-axis)

Simultaneous 5-axis

2.5D milling

2.5-axis milling

Cuts flat contours and pockets by stepping Z down to a set depth. You draw the contour in XY and only change the depth of cut in Z. Mainly for prismatic parts and drilling.^[3][29][9]
Main operations:Contour (outer profile), pocket, facing, drilling and tapping, chamfering, engraving^[3][30][9]

3D (3-axis) milling

3-axis surface milling

Moves the X, Y, and Z axes simultaneously to cut along curved surfaces. For dies and molds and freeform parts. Finishing passes at a fine pitch are stacked with a ball end mill.^{[29][9][20][3]}
Main operations:Waterline (Z-level), raster (parallel), surface-following (scallop, constant pitch), pencil, rest machining^[18][20]

Indexed 5-axis (3+2 axis, positional 5-axis)

3+2 axis / positional 5-axis

Tilts the tool orientation with the rotary axes and locks it, then does 3-axis machining in that attitude. Reduces setup changes and lets a short tool reach deep areas.^{[12][20][9][22]}

Related:5-axis machining

Simultaneous 5-axis

simultaneous 5-axis

Moves 3 linear axes and 2 rotary axes simultaneously, cutting while changing the tool orientation. For impellers, turbine blades, and shapes with undercuts. On the CAM side, how the tool axis is determined and collision avoidance matched to the machine structure are the keys.^{[20][9][12][31]}

Related:5-axis machining

Turning (lathe)

turning

Creates the path in which the tool moves in X and Z against a rotating stock. Outer diameter, inner diameter, end face, grooves, threads. Some CAM supports single-spindle and opposed twin-spindle machines.^[29][9][6]

Mill-turn (multitasking, Swiss-type)

mill-turn / Swiss-type

For machines that do turning and milling in one machine (multitasking machines, sliding-head automatic lathes, etc.). It requires programming that synchronizes the motion of multiple turrets and spindles, so the post for each machine and machine simulation are highly important.^{[32][9][30][5][11]}

Wire EDM

wire EDM

Creates the path the wire electrode follows, for 2-axis and 4-axis wire EDM machines.^{[33][9][34][32]}

CAD/CAM pages

≋

Toolpath types

Contour, pocket, hole, high-efficiency roughing, trochoidal; waterline, raster, surface-following, pencil, rest machining. Includes calculators for trochoidal slot milling and an initial depth-of-cut guide.

▤

CAD/CAM software list

25 products, unranked. Filter by CAM or CAD category, strengths in machining, delivery form, and free or trial versions. Published prices are dated.

⇄

Data formats

What STEP (AP203, AP214, AP242), IGES, Parasolid, ACIS, DXF, DWG, STL, and 3MF carry. Problems that occur in exchange.

⌖

Coordinate systems, post, DNC

Work coordinate system G54, stock and tool library, the 4 stages of simulation, post-processor, DNC operation, and a checklist of common mistakes.

⟲

5-axis machining

The difference between 3+2 and simultaneous 5-axis, machine configurations, NC functions such as tool center point control, calibration, common mistakes, and 5-axis calculations.

ACAD/CAM terms (35 terms)

Term	English	Category	Meaning
CADkyado	Computer-Aided Design	Basics	Creating the 2D or 3D shape of a part on a computer, editing it, and putting it into drawings and other documents.^[1]
CAMkyamu	Computer-Aided Manufacturing	Basics	Creating the commands that run a CNC machine tool (G-code, etc.) with software. In the broad sense, it also includes machining planning, simulation, and post-processing.^[2][3]
CAEshi-e-i	Computer-Aided Engineering	Basics	Using software to simulate a product's performance in order to check a design or solve problems.^[4]
Toolpath (tool path)tsūrupasu	toolpath / tool path	Basics	The route followed by the tool's cutting edge (or center). CAM calculates it from the model, the tool, and the conditions.^[3][21]
CL datashi-eru dēta	cutter location data / CL data	Basics	Machine-independent tool position data output by CAM. A post-processor converts it into an NC program for each machine.^[25]
Post-processor (post)posuto purosessa	post processor / post	Basics	Software that translates CAM path data into an NC program in the format of a specific machine and NC control.^[25][3][26]→ G/M code dictionary
NC program (G-code)enu-shi purogramu	NC program / G-code	Basics	Machining commands that the NC control reads. CAM outputs them through the post.^[2][3]→ G/M code dictionary
Setup (job)settoappu	setup / job	Basics	The group of operations done in one setup. It holds information on the stock, coordinate system, and the machine and tools used, and the machining operations are lined up inside it.^[3][21]
Work coordinate system (WCS)waku zahyokei	work coordinate system / WCS / workpiece coordinate system	Coordinates and setup	A coordinate system placed to fit the part. The CAM WCS is the coordinate reference for the post-processed NC program, and on the machine you match it by registering it as G54 or similar.^[14][15][16]→ G54–G59
Machine coordinate systemkikai zahyokei	machine coordinate system	Coordinates and setup	A coordinate system specific to the machine. The origin of the work coordinate system is registered as a position within the machine coordinate system.^[15]→ G53
Stocksozai	stock	Coordinates and setup	The shape and size of the material before cutting. Entering it in CAM reduces air cutting and is also used to track the remaining stock.^[3][30]
Tool librarykōgu raiburari	tool library	Coordinates and setup	A register of tool and holder shapes, dimensions, and so on.^[3][7][9]→ Tooling
2.5D machiningni-ten-go jigen kakō	2.5-axis machining / 2.5D	Machining type	Machining of a flat shape by stepping Z down to a set depth.^[3][29]
Indexed 5-axis (3+2 axis)warinashi go-jiku	3+2 axis / positional 5-axis	Machining type	Tilts the tool orientation with the rotary axes and locks it, then does 3-axis machining in that attitude.^[22][12][20]
Simultaneous 5-axis machiningdoji gojiku kako	simultaneous 5-axis machining	Machining type	Cutting while moving 3 linear axes and 2 rotary axes simultaneously.^[20][9]
Multitasking (mill-turn)fukugō kakō	mill-turn / multitasking	Machining type	Turning and milling done in one machine. Synchronization of multiple spindles and turrets is required.^[5][32][9]
Waterline machiningtōkōsen kakō	contour / Z-level / waterline	Toolpaths	A path that traces the contour of the shape at each constant height. Suited to steep slopes.^[18][20][3]
Raster machiningsōsasen kakō	parallel / raster	Toolpaths	A path that reciprocates along parallel lines in XY while Z follows the surface. Suited to gentle surfaces.^[18][20]
Surface-following machining (scallop)men-zoi kakō	scallop / constant stepover	Toolpaths	A path offset inward so that the spacing between passes stays constant on a curved surface.^[18][20]
Pencil machiningpenshiru kakō	pencil	Toolpaths	A path that follows small corner radii and valleys to cut areas the previous tool could not reach.^[18][20]
Rest machining (leftover machining)nokoshi-kezuri	rest machining	Toolpaths	A path that uses a smaller tool to cut only the areas the previous operation's tool left uncut.^[19][20]
High-efficiency roughing (adaptive)kōkōritsu arakakō	adaptive clearing / high-efficiency milling	Toolpaths	A roughing method that varies the pass spacing so that the tool engagement stays below a set limit. Uses the side of the tool at deep depth of cut.^[17][30]
Trochoidal millingtorokoido kakō	trochoidal milling	Toolpaths	A method that advances while drawing small circles and removes material bit by bit. Cuts slots and pockets with low cutting force.^[35]
Swarf machiningsuwāfu kakō	swarf milling	Toolpaths	Machining with simultaneous 5-axis in which the side of the tool is placed against an inclined wall.^[20][9]
Stepover (pitch)sutteppu ōbā	stepover / pick feed	Conditions	The spacing between adjacent passes. It affects the height of the cusps (ridges) on the finished surface.^[18][35][36]
Axial depth of cut ap, radial depth of cut aejiku-hōkō kirikomi	axial depth of cut (ap) / radial depth of cut (ae)	Conditions	ap is the amount the tool engages in the axial direction, and ae in the radial direction. High-efficiency roughing and trochoidal milling use a small ae and a large ap.^[35][17]
Machine simulationkikai shimyurēshon	machine simulation	Verification	Showing even the machine structure on screen to check collisions between tool, fixture, and machine, and stroke overruns.^[9][32][31]
Collision checkkanshō chekku	collision check / interference check	Verification	Checking before machining whether the tool and holder will hit the part, fixture, or machine.^[24][12][23]
NC verification softwareenu-shi kenshō sofuto	NC verification software	Verification	Software that reads the post-processed NC program itself and reproduces the machine's motion (VERICUT, NCVIEW, etc.).^[23][24]
DNC operationdi-enu-shi unten	DNC / drip feed / remote buffer operation	Transfer	Operation that machines while sending NC data from an external device. Used for large programs that do not fit in the NC control's memory.^[27]
Neutral format (intermediate file)chūritsu keishiki	neutral format	Data	A common format for exchanging shapes between different CAD and CAM systems. STEP and IGES.^[37][38][39]
B-rep (boundary representation)bi-reppu	boundary representation / B-rep	Data	A way of representing a solid by the connections of the faces, edges, and vertices that enclose it. Used by the kernels of many CAD systems.^[40][41]
Modeling kernelmoderingu kāneru	geometric modeling kernel	Data	The core software component that handles the shape calculations of CAD. Parasolid (Siemens) and ACIS (Spatial) are typical examples.^[40][41]
PMI (product and manufacturing information)pi-emu-ai	product and manufacturing information / PMI	Data	Information such as dimensions, tolerances, and datums attached to a 3D model. There is semantic PMI, whose meaning software can read, and graphic PMI, which is appearance only.^[42][43]→ Drafting
STL (triangle mesh)esu-ti-eru	STL / triangle mesh	Data	A format that represents a surface as a collection of triangles. It has no standard for units or color.^[44]

📚Sources

The CAD/CAM pages are based on software vendors' official pages and help, public pages of standards bodies and public institutions (Library of Congress, NIST, ISO), and university materials. Feature names and available operations differ by software and version, so check the help of the software you use.