From Drawing to Process Plan

Good programs start before the machine: they start on paper. Reading the drawing, choosing the datum, and sequencing operations determines whether the part works or scrapes. This page is the bridge between engineering drawing and G-code.

Concept

A process plan translates a drawing into ordered machine operations. Step 1: read the drawing and identify critical dimensions, datums, and surface finish requirements. Step 2: choose work zero relative to the drawing datums. Step 3: sequence operations — roughing first, finishing last, holes after profile. Step 4: select tools and cutting parameters. Only then write G-code.

Why It Matters

Writing code before planning produces a program that machines the wrong features in the wrong order. A part that needs a Ø10 H7 hole should be roughed to Ø9.8 then bored or reamed — not drilled to size directly. The process plan determines the tool list, cycle time, and whether the part holds tolerance. A missing plan can produce a correct-looking program for the wrong setup.

How It Works

The Process Plan Template

1. Material and stock — what are you starting from? Raw bar, plate, forging? Size and condition?
2. Datum — which feature does the drawing reference? Set work zero there. The datum should be a finished surface, not raw stock.
3. Operations in order — face, rough, finish, drill, tap, inspect. If facing is needed to establish the planned reference, schedule it before features that depend on that surface.
4. Tools — which tool for each operation? What H/D offset numbers? How many tools total?
5. Cutting parameters — RPM and feed from tooling data, not guesswork.
6. Inspection — which dimensions to check after each setup? What gauge?

Drawing Review Checklist

• Dimensions — identify all dimensions and their tolerances. Which are critical? Which are nominal?
• Datums — where do the dimensions reference from? That is where G54 should be.
• Surface finish — Ra requirements determine whether you need a finish pass.
• Holes — what size, tolerance, and depth? Drill directly vs drill-ream vs drill-bore?
• Threads — standard or custom? Internal or external? Tapping vs thread milling?
• Chamfers/fillets — what size? Which tool can produce them?

Example: Plate 100×80×12

A rectangular plate with a pocket and 4 holes. Process plan:

1. Face top surface with Ø63 face mill (establishes Z0)
2. Rough pocket with Ø10 end mill (leave 0.2 mm finish stock)
3. Finish pocket to size (light cut, good surface)
4. Spot drill 4×Ø6 holes (center drill)
5. Drill 4×Ø6 holes
6. Deburr edges

Work zero at lower-left corner on the top surface. Tool list: T01 face mill, T02 roughing end mill, T03 finishing end mill, T04 spot drill, T05 drill. Five tools, five operations, one setup.

Reading a Drawing Before You Touch the Machine

A drawing is a contract: it says what dimensions matter, what tolerances they carry, what surface finish is required, and what datum those dimensions reference. Before writing any G-code, read the drawing three times. First pass: what is the part, what material, what is the stock? Second pass: list every dimension that has a tolerance box, every GD&T symbol, every note about surface finish. Third pass: trace which datum each tolerance references — that datum is where G54 should live. A dimension that references datum B does not care where you clamped the part on the raw stock; it cares about B.

Choose the datum so that the critical dimensions are machined in one setup when possible. If the drawing locates holes from one side face and one end face, set G54 at the intersection of those two finished faces. If the drawing uses a bore as datum, machine that bore first, then flip the part to a soft jaw bored on that bore. Datum transfer — moving from raw stock to a finished face to a finished bore — is the art of process planning. Each transfer adds error; the fewer transfers, the better the tolerance stack-up.

Sequence operations in this order: face the raw stock (establishes Z0), rough the profile (removes bulk stock, leaves 0.4–0.8 mm), finish the profile (cuts to size), then drill holes, then bore/ream to tolerance, then tap if needed. Roughing before finishing protects the finished surfaces from the heat and deflection of the roughing cuts. Drilling before boring leaves a clean hole for the boring bar. Tapping last — a broken tap in a finished part scraps everything before it.

Tool selection follows the operation, not the other way around. For a Ø10 H7 bore on a specific bracket, the process uses a spot drill, a Ø9.8 twist drill, and a boring bar or reamer — not a Ø10 drill. The required nose radius depends on the specific contour and accessibility; choose the tool that reaches every corner without a blend. List the tools, speeds, and feeds on paper before opening CAM. The program is the last step, not the first.

Inspection planning is also part of the process. For each critical dimension, decide how you will measure it after the first part: calipers for ±0.1, micrometer for ±0.02, bore gauge for holes, height gauge for positions. If you cannot measure a tolerance on the tools you have, the tolerance is not achievable on your shop floor — and that decision belongs in the process plan, not after the first scrapped part.

Sample Process Plan: A Bracket

Take a simple 100×60×10 mm aluminum bracket with two Ø8 holes, one Ø10 H7 bore, and a 0.5×45° chamfer. The raw stock is a saw-cut plate. Process plan:

1. Face the top and one side (establishes Z0 and X datum). Mill to 100×60 finished size.
2. Mill the outer profile to finished dimensions in one setup (G54 at lower-left corner).
3. Spot-drill, drill Ø7.8 the two Ø8 holes, then ream to Ø8 H7 if required.
4. Spot-drill, drill Ø9.8 the Ø10 bore, then bore to Ø10 H7 with a boring bar.
5. Chamfer all edges 0.5×45° with a chamfer mill or manual deburr.
6. Inspect: hole positions, bore diameter, overall dimensions, surface finish.

Why this order? Facing first gives a clean Z0. Outer profile before holes so the holes are located from finished edges. Drilling before boring leaves a clean hole for the boring bar. Chamfering last so the chamfer tool does not knock the work loose. Each step protects the previous one.

If the Ø10 H7 bore is a datum for a later setup, machine it first and flip the part on a soft jaw bored to that bore. This is datum transfer: one extra setup, but every dimension referenced to the bore is now from the bore, not from the raw stock.

Roughing vs Finishing Allowances

Roughing removes bulk stock. It does not need to hold tolerance; it needs to remove material fast. Leave 0.4–0.8 mm on diameter (lathe) or 0.2–0.5 mm on wall (mill) for the finishing pass. Rough at high feed, moderate speed. Finishing cuts the final size: lower feed, higher speed, shallow depth. The finishing tool is often a different insert (sharper, polished) than the roughing tool.

On a lathe, G71 leaves U0.4 diameter and W0.1 axial as finish stock; G70 cuts it. On a mill, the CAM leaves a finish pass of 0.3 mm on walls and floor. If you rough to size, you have no room to correct tool wear; if you leave too much finish stock, the finish pass chatters. 0.4 mm on diameter is a standard classroom compromise.

Tolerance stack-up: if the drawing calls for Ø20 ±0.02, your process must hold better than that. Roughing ±0.1, finishing ±0.02, inspection at ±0.01. If your machine cannot hold ±0.02 on that diameter, the tolerance is not achievable — state that before the part starts, not after the first scrap.

Reading a Drawing Before You Program

Before writing a single G-code, read the drawing end to end: material, stock size, finished dimensions, tolerances, surface finish, datum symbols, notes, revision. Circle the datum references — every tolerance chains back to them. If the drawing says "datum A: Ø20 bore," your first setup must establish that bore. If the drawing says "all over tolerance ±0.05," your machine must hold that. If a tolerance is tighter than your machine can hold, stop and talk to the engineer before cutting.

Common drawing traps: a dimension that looks like it is a diameter but is actually a radius; a hole callout that says "through" but the material thickness is not stated; a surface finish symbol on a surface you planned to leave as milled. Read the notes block — it often contains the most important information (deburr, break sharp edges, material cert).

After reading, sketch the process on paper: raw stock, setups, tools, order. If the process does not fit in one setup, plan the second setup's datum transfer now. Do not start programming until the process plan is on paper. Programming without a process plan is how 500-line CAM programs get scrapped on the first part.

Workholding Strategy

The process plan must specify how the part is held. A vise for flat plate; a chuck for round bar; soft jaws for finished diameters; a tombstone for multiple parts. Workholding affects which faces are accessible: if the part is gripped by the Ø20 bore, the OD is accessible but the bore is not. Plan the operations so that each setup accesses the faces it needs.

Rule of thumb: the first setup should machine the datums. The second setup should reference those datums. If you flip the part without a machined datum to flip on, the second setup is random — every dimension from the first setup walks. Machine a clean pad or bore in setup 1, then flip on that pad in setup 2.

Clamping force: enough to hold the part, not so much that it distorts a thin wall. A thin-walled aluminum tube held too hard in a vise springs out of round when you release it. For thin walls, use expanding mandrels or soft jaws that support the wall from inside. Clamp on solid material, not on finished surfaces.

Tool Selection for the Process

The process plan lists every tool: tool number, type, diameter, corner radius, length. A roughing end mill, a finishing end mill, a drill, a chamfer mill. Each tool has a reason. If a tool is on the list but you cannot say what operation it does, remove it — extra tool changes cost 8 seconds each.

Tool overhang: use the shortest overhang that reaches the cut and clears the holder, not the longest tool you have. Long tools deflect. If a 50 mm projection reaches the pocket, do not use a 100 mm tool. Tool length also affects the H offset: longer tools have longer reach, but they deflect more under load. Match overhang to the job, and confirm holder clearance around the fixture.

ISO workpiece-material groups: P = steel, M = stainless, K = cast iron, N = non-ferrous (aluminum, copper, brass), S = superalloys/titanium, H = hardened steel. Use the right group for the material. A P-grade insert in aluminum builds up edge (BUE) and leaves a poor finish; an N-grade insert in steel wears fast. The insert manufacturer's catalog has the starting parameters for each group and material; the group is a starting point, not a fixed insert grade.

Common Mistakes

• Drilling before milling the flat surface — holes start on uneven stock and wander.
• Choosing work zero at a corner that is not the drawing datum — dimensions accumulate from the wrong origin.
• Skipping roughing and trying to finish in one cut — too much stock causes tool deflection and poor finish.
• Not planning inspection points — you must know what to measure before you measure it.
• Underestimating tool changes — each tool change takes time; consolidate operations where possible.

Practice

1. Why rough before finish?

2. What is the first operation on a raw plate?

3. Why spot drill before drilling?

4. What is a datum, and why does it matter?

Sources

• Haas mill programming: work and tool offsets