CAD/CAM and Post-Processing

Introduction

Computer-aided design (CAD) and computer-aided manufacturing (CAM) connect product definition with machine execution. CAD describes the geometry, dimensions, tolerances, materials, and design intent of a component. CAM converts that information into machining operations, toolpaths, verification data, and machine-ready numerical control (NC) code. Post-processing adapts the generic toolpath to a particular machine-tool and controller.

This connection is not a simple file conversion. It is an engineering decision process involving coordinate systems, stock, cutting tools, machining strategies, tolerances, collision avoidance, simulation, data exchange, and verification. A visually correct CAD model can still produce an unsafe or inaccurate program if its units, work offset, tool definition, machine limits, or post-processor configuration is wrong.

A useful process chain is:

CAD model → design interpretation → CAM setup → operation planning → toolpath calculation → verification → post-processing → machine simulation and prove-out → machined component

The chain is only as reliable as its weakest link. Therefore, competent CNC programmers must understand both digital models and physical machining.

Learning Objectives

By the end of this chapter, the learner should be able to:

1. Explain how CAD data is prepared for CAM use.
2. Select appropriate machining strategies for common features and materials.
3. Define tools, holders, workholding, stock, coordinate systems, and machining boundaries.
4. Distinguish geometric accuracy, tolerance, surface finish, and manufacturing capability.
5. Simulate material removal and identify gouges, collisions, overcuts, and uncut stock.
6. Explain the function and risks of post-processors.
7. Evaluate model interoperability and diagnose common data-transfer errors.
8. Apply a structured workflow to create and verify a production-ready NC program.

1. CAD Data as Manufacturing Information

A CAD model may be represented as a solid, surface model, wireframe, mesh, or drawing. A solid model is generally preferred for prismatic and rotational machining because it represents enclosed volume and supports reliable mass properties, sectioning, and interference checks. Surface models can accurately describe complex shapes but may contain gaps, overlaps, or incorrect surface normals. Meshes are useful for scanning, additive manufacturing, and visual reference, but they are often unsuitable for precise subtractive programming unless repaired or converted.

CAD geometry contains two different kinds of information:

• Geometric information: faces, edges, curves, coordinates, and topology.
• Design-intent information: dimensions, datums, fits, tolerances, material, surface-finish requirements, and feature relationships.

A neutral file format may preserve geometry while losing design history, feature names, associativity, or tolerances. Common exchange formats include STEP, IGES, Parasolid, DXF, and STL. Their suitability depends on the application.

Model preparation

Before programming, the model should be inspected for:

• missing or duplicated faces;
• open shells where a closed solid is expected;
• extremely small sliver faces;
• incorrect units or scale;
• unwanted construction geometry;
• ambiguous fillets, chamfers, or threads;
• suppressed features that affect machining;
• incorrect surface normals;
• missing datum or coordinate-system information.

A model should not be modified casually merely to make programming easier. If a change affects function, fit, or inspection, it requires engineering authorization. CAM-derived simplifications should be clearly identified as manufacturing representations rather than design revisions.

2. Interoperability and the Digital Thread

Interoperability is the ability of different software and equipment to exchange usable information. It includes syntactic interoperability—whether a file can be opened—and semantic interoperability—whether its meaning remains correct. A model that opens successfully but changes from millimetres to inches is syntactically successful but semantically unsafe.

The model-based definition approach attempts to place manufacturing information directly in the 3D model. Product manufacturing information may include geometric dimensioning and tolerancing (GD&T), surface texture, material, datum references, and process notes. Standards such as STEP AP242 support richer product and manufacturing information exchange than older geometry-only workflows, although practical implementation varies by software.

A robust data-control procedure includes:

1. Confirm part number, revision, units, material, and approval status.
2. Compare the received model with the released drawing or product-manufacturing definition.
3. Heal and validate geometry without changing functional intent.
4. Record the exchange format and software versions.
5. Establish a traceable link between the model revision, CAM file, post-processor, and NC file.
6. Revalidate the program whenever the model, tool library, machine, controller, or post changes.

Associativity is particularly important. In an associative workflow, a design change can update selected CAM features and toolpaths. However, automatic regeneration is not equivalent to engineering approval. A changed hole location may update a drilling operation while leaving workholding, tool access, inspection plans, or collision conditions invalid.

3. CAM Setup: Stock, Fixtures, and Coordinate Systems

A CAM setup is the digital description of how the part will be held and machined. It normally includes the model, stock, fixture or machine components, work coordinate system (WCS), tools, and operation sequence.

Stock definition

Stock may be defined as:

• a rectangular or cylindrical primitive;
• a bounding box with controlled offsets;
• an extruded profile;
• a casting or forging envelope;
• a previous-operation model;
• scanned or measured material.

Stock must represent the material actually present. Excess stock can cause unnecessary cutting; insufficient stock can cause the simulation to remove material that exists physically, creating a false sense of completion.

For a rectangular blank with model dimensions L, W, and H, and uniform allowances a_L, a_W, and a_H, the stock dimensions are:

Here L_s, W_s, and H_s are stock dimensions. The one-sided allowance in height assumes the lower face is already located against a datum or is intentionally left unchanged. If allowances apply to both faces, the corresponding dimension receives 2a. The equation is a planning relationship, not a universal rule; castings, forgings, and near-net blanks require their actual envelope to be measured or specified.

Work coordinate systems

The WCS establishes the origin and positive axes used by CAM and the machine. Typical origins are:

• top of stock for simple prismatic work;
• finished part datum for inspection alignment;
• centre of a rotary part;
• a fixture datum or vise corner;
• a probe-established reference point.

The programmer must distinguish the CAD coordinate system, CAM WCS, machine coordinate system, and controller work offset such as G54. A toolpath can be geometrically correct in CAM but cut incorrectly if the physical setup uses a different origin or orientation.

Best practice is to define the WCS from functional datums whenever possible. Datum selection should support accurate workholding, measurement, and repeatability rather than merely simplify screen selection.

Fixtures and accessibility

Fixtures must be represented where they can interfere with tools, holders, probes, or rotary axes. A simplified fixture is acceptable only if its envelope remains conservative. Ignoring a clamp because it is “not part of the model” is a common cause of collisions.

4. Selecting Machining Strategies

A machining strategy specifies how a tool moves through material. It should be selected from feature geometry, material, rigidity, tool capability, tolerance, surface finish, and production volume.

Roughing

Roughing removes large volumes efficiently while leaving a controlled allowance for finishing. Adaptive or constant-engagement strategies maintain a more uniform cutter load by varying feed direction and step-over. Conventional pocketing may be effective for simple open regions, but sharp internal corners and changing engagement can increase load.

A roughing allowance should be large enough to avoid accidental finishing during an unstable operation, but small enough to prevent excessive finishing stock. It may be unequal: a wall allowance can differ from a floor allowance when distortion, tool deflection, or subsequent datum creation is considered.

Rest machining

Rest machining targets material left by a larger tool in corners, narrow regions, or around features. It uses the previous toolpath or in-process stock as a reference. Rest operations should be based on verified remaining stock, not merely on the nominal model, because tool deflection and holder clearance can affect the real result.

Finishing

Finishing strategies include contouring, planar passes, parallel passes, scallop machining, projection, pencil tracing, and flowline machining. A strategy should follow the geometry in a way that controls cusp height, cutting direction, tool engagement, and surface quality.

For a ball-nose tool on a surface, cusp height depends on tool radius, step-over, and local curvature. A simplified flat-surface approximation is:

where h is approximate cusp height, s is lateral step-over, and R is the ball-nose radius. This approximation assumes small step-over relative to tool radius and a locally planar surface. It is not sufficient by itself for steep or highly curved surfaces, where scallop geometry and surface normal direction must be evaluated by the CAM system. Units must be consistent; if s and R are in millimetres, h is in millimetres.

Holemaking

Hole operations may include spot drilling, drilling, peck drilling, boring, reaming, tapping, thread milling, and interpolation. The selected method depends on hole diameter, depth, material, tolerance, chip evacuation, machine capability, and required surface condition. A deep hole in aluminium may need a different cycle and coolant approach from a shallow hole in hardened steel.

Five-axis and multiaxis machining

Five-axis machining can orient the tool to improve access, reduce tool length, maintain favourable cutting conditions, and machine undercuts. It also introduces risks involving rotary-axis limits, singularities, excessive angular motion, gouging, and post-processor kinematics. A mathematically valid tool orientation is not automatically machine-feasible.

5. Tools, Cutting Data, and Process Planning

A digital tool definition must include diameter, corner radius or tip geometry, flute length, overall length, holder, gauge length, number of teeth, and orientation. The tool assembly—not only the cutter—determines accessibility and collision risk.

Two fundamental cutting relationships are commonly used. For a rotating tool:

where v_c is cutting speed in metres per minute, D is tool diameter in millimetres, and N is spindle speed in revolutions per minute. Rearranging gives:

For a milling cutter with z teeth and feed per tooth f_z in millimetres per tooth, feed rate is:

where v_f is feed rate in millimetres per minute. These relationships assume the programmed cutting diameter and feed per tooth are appropriate for the operation. Manufacturer recommendations may require adjustment for radial engagement, axial depth, material, coolant, machine rigidity, and tool overhang.

Worked example. A four-flute, 10 mm cutter is recommended to operate at a cutting speed of 150 m/min and feed per tooth of 0.04 mm/tooth. The spindle speed is:

N = (1000 × 150)/(π × 10) ≈ 4775 rpm

The feed rate is:

v_f = 0.04 × 4 × 4775 ≈ 764 mm/min

The controller may require a permissible rounded value, such as 4,800 rpm and 765 mm/min, provided that machine and tool limits are respected. The calculation does not determine depth of cut, coolant, or tool life; those require process knowledge and supplier data.

Tool selection should consider:

• workpiece material and hardness;
• tool material and coating;
• feature accessibility;
• required corner radius;
• holder clearance;
• rigidity and overhang;
• chip evacuation;
• tolerance and finish;
• tool-change and inspection requirements.

6. Tolerances, Accuracy, and Surface Finish

CAD geometry is idealized; machining produces a physical surface affected by machine accuracy, thermal growth, fixturing, tool deflection, runout, wear, vibration, and measurement uncertainty. CAM tolerance is therefore not the same as part tolerance.

A CAM tolerance controls how closely a calculated toolpath approximates the CAD surface. A tight tolerance can improve geometric approximation but may create a very large NC file, increase calculation time, and exceed the machine’s practical capability. A loose tolerance can produce visible faceting or dimensional error. The selected value should reflect the drawing tolerance, tool diameter, surface curvature, machine capability, and inspection method.

Tolerance budgeting can be expressed conceptually as a combination of contributors. If independent deviations are approximately random, a root-sum-square estimate is sometimes used:

where T_i are standard-deviation-like contributions. This is not a universal tolerance stack-up formula. It assumes contributors are appropriately represented, statistically independent, and roughly centred. Worst-case design uses arithmetic addition of absolute limits instead and is more conservative.

Surface finish is influenced by cusp height, tool geometry, feed marks, vibration, material, coolant, and tool condition. CAM can reduce programmed scallop height, but it cannot compensate for a weak fixture or a worn tool. Inspection must therefore measure the finished part using an appropriate datum scheme and instrument.

7. Toolpath Verification and Simulation

Verification is performed at several levels:

1. Geometric verification: Does the toolpath follow the intended model?
2. Material-removal simulation: Is stock removed in the correct sequence?
3. Collision verification: Does the cutter, holder, spindle, or fixture collide?
4. Machine simulation: Are axes, limits, rotary kinematics, and travel realistic?
5. Code verification: Does the posted NC file produce the same motion assumed in CAM?

Material-removal simulation compares the initial stock with the remaining in-process stock. It can reveal uncut regions, overcut surfaces, incorrect approach moves, and errors in operation ordering. A simulation based only on the cutter tip may miss holder or spindle collisions. A simulation based only on the generic CAM machine may miss controller-specific transformations.

Important verification concepts include:

• Gouge: unintended removal of material by the cutter, holder, or another component.
• Collision: physical interference between machine components, tools, fixtures, stock, or part.
• Excess stock: material that should have been removed but remains.
• Overtravel: commanded motion beyond an axis or machine limit.
• Singularity: a kinematic condition in which small tool-orientation changes require extreme rotary-axis motion.
• Rapid-through-stock: an unsafe rapid movement crossing material or fixture space.

Simulation is not proof of safety. It depends on accurate machine models, tool assemblies, fixture geometry, controller behavior, and post-processing. The first physical run should still use a controlled prove-out: correct work offset, tool-length verification, single-block or reduced rapid mode where appropriate, feed override, and operator observation.

8. Post-Processing

CAM systems commonly calculate a machine-independent toolpath. The post-processor translates it into the syntax and kinematics required by a particular machine and controller. It may control:

• G- and M-code format;
• units and decimal precision;
• absolute or incremental output;
• plane selection;
• tool-change and spindle commands;
• coolant commands;
• work offsets;
• canned cycles;
• cutter compensation;
• rotary-axis conventions;
• inverse-time feed for multiaxis motion;
• machine limits and retract behavior;
• program headers, comments, and end codes.

A post-processor is not merely a formatting template. For multiaxis machines it may transform tool-center-point data into coordinated linear and rotary-axis positions. Incorrect axis signs, rotary limits, pivot lengths, or TCP assumptions can cause serious damage even when the generic toolpath is correct.

Evaluating a post-processor

A post should be evaluated against a controlled test suite, including:

1. Basic three-axis motion.
2. Tool change and length compensation.
3. Work-offset activation.
4. Circular interpolation in each relevant plane.
5. Drilling and tapping cycles.
6. Retracts near fixtures.
7. Rotary-axis motion and limit handling.
8. Unit changes and decimal precision.
9. Program restart behaviour.
10. Safe program termination.

The output should be reviewed by an experienced programmer and, where available, run through a controller-specific verifier. Changes to a post require version control and regression testing. A post that works for one machine should never be copied to another solely because the controllers have similar names.

9. A Structured CAD/CAM Workflow

A disciplined workflow reduces omissions:

Stage 1: Interpret the product definition

Identify datums, critical features, tolerances, surface requirements, material, heat treatment, and inspection requirements.

Stage 2: Plan the process

Decide workholding, setups, datum sequence, roughing and finishing operations, tool access, and likely inspection points.

Stage 3: Build the CAM setup

Load the approved model, define stock and fixtures, establish WCS, and confirm units and orientation.

Stage 4: Create operations

Select tools and cutting data; define containment, heights, entry and exit moves, step-over, depth of cut, allowances, and coolant.

Stage 5: Regenerate and inspect

Check operation dependencies, tool axes, linking moves, tool lengths, and areas not reached by the tool.

Stage 6: Simulate

Perform material-removal, collision, and machine-kinematic verification. Inspect the remaining stock against the model.

Stage 7: Post-process

Use the approved machine-specific post. Record post version, machine, controller, units, and program revision.

Stage 8: Review the NC code

Check headers, offsets, tool numbers, spindle and feed commands, compensation, safe retracts, canned cycles, and end-of-program commands.

Stage 9: Prove out and document

Verify setup, tools, offsets, and workholding. Run under controlled conditions, measure the first component, record results, and update process documentation.

10. Illustrative Case: A Two-Setup Aluminium Housing

Background

A small aluminium housing has a milled pocket, four mounting holes, a contoured upper surface, and two precision datum faces. The component is manufactured from a rectangular billet on a three-axis machining centre. The drawing specifies a 0.05 mm positional tolerance for the mounting-hole pattern and a 0.02 mm flatness requirement on one datum face.

Problem

An initial CAM program produced an acceptable visual simulation, but the first physical component had a hole-pattern error and a collision between the holder and a vise jaw during a finishing operation.

Analysis

The programmer had selected the top of stock as the WCS, while the inspection plan referenced the finished datum face. The setup also used a simplified fixture model that did not include the raised vise jaw. The post-processor output was syntactically valid, but the machine simulation used an incorrect holder length.

Approach and solution

The process was redesigned as follows:

• Setup 1 faced the billet and created the primary datum.
• Setup 2 located the part from the machined datum faces.
• The WCS was aligned with the inspection datums rather than the raw stock.
• The complete vise and jaw geometry was added to the CAM model.
• A shorter finishing tool with a verified holder assembly was selected.
• Hole locations were generated from the released model and checked against the drawing.
• Roughing, rest machining, and finishing were simulated using accurate in-process stock.
• The post-processed file was verified in a controller-specific machine simulation.
• The first part was run with reduced rapid override and measured using a coordinate-measuring machine.

Outcome

The second trial eliminated the holder collision and reduced the hole-pattern error to within the specified tolerance. The datum face also met flatness requirements after the facing strategy was changed to use balanced passes and a more rigid tool assembly.

Learning points

The case demonstrates that model accuracy alone does not guarantee manufacturing accuracy. Datum selection, fixture representation, tool assembly, inspection alignment, and post-processor validation must agree. It also shows why “simulation complete” is not an adequate release criterion unless the simulation reflects the actual machine and setup.

11. Challenges, Limitations, and Professional Responsibilities

CAM automation can conceal errors. Automatic feature recognition may misidentify a counterbore as a blind hole; automatic tool selection may choose a tool that fits geometrically but lacks sufficient rigidity; automatic rest machining may rely on an unverified previous operation. Human review remains essential.

Major limitations include:

• incomplete or corrupt CAD data;
• inaccurate machine and fixture models;
• unverified tool assemblies;
• controller-specific differences;
• excessive NC file size;
• numerical rounding and chordal approximation;
• thermal and elastic effects not represented in simulation;
• inadequate measurement or datum interpretation.

Professionally, NC programmers are responsible for traceability and safe release. Programs should identify revision, machine, units, work offsets, tools, and post version. Obsolete files should be controlled to prevent accidental use. Safety interlocks, guarding, lockout procedures, and local regulations remain mandatory; software verification does not replace machine safety practice.

Intellectual property and cybersecurity are also relevant. CAD models, tool libraries, and NC programs may be proprietary. Access control, secure transfer, malware protection, and authenticated revision control are necessary in connected manufacturing environments.

12. Contemporary Developments

Modern CAM systems increasingly use digital twins, cloud collaboration, model-based definition, automated feature recognition, and machine-learning assistance. AI may suggest tools, identify inefficient toolpaths, classify features, or detect anomalous cutting behaviour. These systems can improve productivity, but recommendations must be explainable and validated against material, machine, tooling, and quality requirements.

Digital twins are useful only when the virtual machine reflects actual kinematics, controller logic, tooling, and maintenance state. Data-driven optimization can also amplify poor historical practice if training data contain unsafe or nonconforming programs. Human approval, controlled data, and measurable acceptance criteria remain necessary.

Best Practices

• Use released models and confirm revision, units, and material.
• Preserve functional design intent when repairing geometry.
• Define stock and fixtures conservatively and realistically.
• Use functional datums for WCS selection.
• Represent the complete tool assembly, not just the cutter.
• Match CAM tolerance to part tolerance and machine capability.
• Simulate material removal, collisions, and actual machine kinematics.
• Validate post-processors with a documented test suite.
• Review posted code independently of the graphical toolpath.
• Prove out programs under controlled conditions and measure the first part.
• Maintain revision control for models, CAM files, posts, and NC programs.
• Treat automation and AI as decision support, not as a substitute for engineering judgment.

Chapter Summary

CAD/CAM transforms a digital product definition into a verified manufacturing process. Effective programming requires more than selecting a toolpath: the programmer must validate geometry, preserve design intent, define realistic stock and fixtures, establish functional coordinate systems, select suitable strategies and tools, and control tolerances. Material-removal and machine simulation reveal many errors, but their reliability depends on accurate digital representations. Post-processors translate generic toolpaths into controller-specific code and must be tested, version-controlled, and evaluated with the real machine in mind. Interoperability, traceability, safe prove-out, inspection, and professional responsibility complete the digital manufacturing workflow.

Key Terms

CAD: Computer-aided design used to create and document product geometry.

CAM: Computer-aided manufacturing used to plan machining and generate toolpaths.

Post-processor: Software that converts a generic CAM toolpath into machine- and controller-specific NC code.

WCS: Work coordinate system defining the programmed origin and axes.

Stock: Raw material available before a machining operation.

In-process stock: Digital representation of material remaining after simulated operations.

Tool assembly: Cutter, holder, arbor, gauge length, and associated geometry.

Associativity: A maintained relationship allowing downstream data to respond to approved model changes.

Interoperability: Ability of systems to exchange information while preserving its meaning.

Rest machining: Removal of material left by a preceding larger or less accessible tool.

Gouge: Unintended removal of material from the part.

Collision: Physical interference between machine, tool, fixture, stock, or part.

Chordal tolerance: Maximum deviation between a calculated toolpath segment and the intended surface.

Datum: Reference feature or system used to locate, orient, or inspect a part.

Cusp height: Ridge height left between adjacent finishing passes.

Cutting speed: Relative speed between the cutting edge and workpiece surface.

Feed per tooth: Distance advanced per cutter tooth during milling.

Digital twin: A digital representation that models relevant behaviour of a physical manufacturing system.

Model-based definition: Product definition in which 3D geometry carries manufacturing information.

Prove-out: Controlled first execution used to confirm program and setup safety and correctness.

Review Questions

Short Answer Questions

1. Why can a CAD model that opens correctly still be unsafe for CAM programming?
2. What is the purpose of defining fixtures in a CAM setup?
3. Distinguish CAM tolerance from the tolerance specified on a component drawing.
4. What information does a post-processor add or transform?
5. Why should the tool holder be included in collision simulation?

Long Answer Questions

1. Explain a complete CAD-to-NC workflow, identifying major verification activities at each stage.
2. Compare roughing, rest machining, and finishing strategies and state when each is appropriate.
3. Discuss the effects of WCS and datum selection on machining accuracy and inspection.
4. Explain how interoperability problems arise during CAD data exchange and propose controls to reduce them.
5. Describe a documented method for evaluating and releasing a machine-specific post-processor.

Analytical / Application Questions

1. A 12 mm, three-flute cutter is recommended at 120 m/min and 0.05 mm/tooth. Calculate spindle speed and feed rate, showing units and suitable rounding.
2. A simulated toolpath is gouge-free, but the physical machine has a longer holder than the CAM model. Analyse the likely risks and specify corrective actions.
3. Design a two-setup CAM plan for a component with two precision datums, a deep pocket, and side holes. Justify the WCS locations, fixture representation, tool sequence, verification steps, and inspection strategy.

Multiple Choice Questions with Answers

Question 1

Which representation generally provides the most reliable basis for solid-model CAM programming?

A. A closed solid model

B. A raster image

C. A hand-drawn sketch

D. A colour-rendered mesh only

Correct Answer: A. A closed solid model

Question 2

What is the primary function of a post-processor?

A. To design the original component

B. To translate a generic toolpath into machine-specific NC code

C. To measure surface roughness

D. To replace the machine controller

Correct Answer: B. To translate a generic toolpath into machine-specific NC code

Question 3

A 10 mm cutter operates at 150 m/min. Using N = 1000v_c/(πD), the approximate spindle speed is:

A. 477 rpm

B. 1,500 rpm

C. 4,775 rpm

D. 47,750 rpm

Correct Answer: C. 4,775 rpm

Question 4

Which item is most important when defining a CAM setup for collision verification?

A. The screen colour theme

B. The complete fixture envelope

C. The drawing file name only

D. The operator’s preferred feed override

Correct Answer: B. The complete fixture envelope

Question 5

Rest machining is primarily used to:

A. Remove material left by a previous tool

B. Create a new CAD assembly

C. Change inch units to metric units

D. Measure spindle power

Correct Answer: A. Remove material left by a previous tool

Question 6

What does a CAM chordal tolerance control?

A. The hardness of the workpiece

B. The approximation of the calculated path to the intended surface

C. The number of fixture clamps

D. The controller memory size

Correct Answer: B. The approximation of the calculated path to the intended surface

Question 7

For a four-flute cutter at 4,775 rpm and 0.04 mm/tooth, the approximate feed rate is:

A. 47.75 mm/min

B. 191 mm/min

C. 764 mm/min

D. 19,100 mm/min

Correct Answer: C. 764 mm/min

Question 8

Why is a controller-specific simulation valuable after generic CAM simulation?

A. It verifies controller syntax and machine kinematics more realistically

B. It eliminates the need for work offsets

C. It automatically repairs damaged fixtures

D. It guarantees tool life

Correct Answer: A. It verifies controller syntax and machine kinematics more realistically

Question 9

Which statement about a post-processor is correct?

A. A post is interchangeable among all machines using the same cutter

B. A post may control rotary-axis transformations and machine limits

C. A post changes the material properties of the part

D. A post replaces inspection

Correct Answer: B. A post may control rotary-axis transformations and machine limits

Question 10

Which practice best supports traceability in CNC programming?

A. Deleting previous revisions immediately

B. Using any post that produces readable code

C. Recording model, CAM, post, machine, and NC revisions

D. Relying only on the operator’s memory

Correct Answer: C. Recording model, CAM, post, machine, and NC revisions