Coolant, Workholding, and Setup for Your First CNC Job

Part 8 of the CNC Machining Mini-Course — the finale. Start with Part 1 if you're just joining.

---

There's a saying in machining: good setups make good parts. You can have the best CAD model, the most efficient CAM toolpaths, and the highest-quality machine on the floor — and still produce scrap if the workholding is wrong or the coolant isn't appropriate for the job.

This post covers the physical reality of setting up and running a CNC job: how to hold your work so it doesn't move, how to manage heat and chip evacuation, and the step-by-step process of going from a blank piece of material to a first good part.

---

Workholding: The Part Must Not Move

The first rule of machining is that the workpiece cannot move during the cut. Cutting forces are real — a half-inch endmill in steel at reasonable feed rates generates tens to hundreds of pounds of force. If your part shifts even a few thousandths, you'll cut in the wrong place. If it shifts more, you'll hear it — loudly — before something breaks.

Machine Vises

The machine vise (also called a milling vise or Kurt-style vise) is the most common workholding solution for prismatic parts on a mill. It's a precision jaw vice bolted to the table. You put the part between the jaws, tighten the screw, and the part is clamped.

A few vise-specific tips:

Parallels: When clamping a flat part, you don't want it sitting directly on the rough cast iron of the vise jaw bed. Use precision parallels — matched pairs of hardened steel bars in consistent heights. Place the part on top of the parallels so it sits at a known, flat height. Tap the part down with a dead blow mallet after initial clamping to seat it fully on the parallels. If a parallel can be pulled out after clamping, the part isn't fully seated.

Kurt vises: The Kurt D688 and variants are the industry standard machine vise. They're expensive for a reason — they hold tight tolerances, the jaws close parallel and square, and they're built to last decades. When I was running Haas machines in my shop, Kurt vises lived on the table.

Soft jaws: A set of jaws machined from aluminum (or steel, for permanent fixtures) to match the profile of a specific part. Instead of two flat jaws gripping a square part, you machine pockets that exactly match the part's shape. This allows clamping of odd geometries, minimizes distortion on thin parts, and is standard practice for production runs.

Clamps and T-Slot Fixturing

For larger parts that won't fit in a vise, you clamp directly to the T-slot table. Step clamps (also called bridge clamps), toe clamps, and strap clamps bolt into the T-slots and clamp across the top of the part.

Rules for direct clamping:

• Alternate clamps around the part — don't put them all on one side

• Support the part underneath — don't clamp it spanning a void

• Keep clamps as close to the work as possible; the farther out, the more they flex

• Use a clamp on both sides of each cut line when possible

Collets and Chucks (Lathe)

On a lathe, workholding is the chuck — a device at the spindle that grips the part and spins it.

3-jaw chucks: Self-centering, fast to use, grip round or hex stock automatically. Not perfectly accurate — a 3-jaw chuck typically holds ±0.005" concentricity at best, which is fine for many jobs but not precision work.

4-jaw chucks: Each jaw adjusts independently. More accurate (you can indicate to better than 0.001" with care) but requires more setup time. Used when concentricity to a previously turned feature matters.

Collet chucks: For bar stock work, a collet chuck grips the bar with very high accuracy. The standard for production turning of small to medium parts.

Between centers: For long shafts where concentricity and straightness matter, turn between a drive center (at the headstock) and a live center (in the tailstock). This is how precision shafts are finished.

---

Coolant and Cutting Fluid

Coolant does two things: removes heat and evacuates chips. Both matter, and neglecting either leads to shorter tool life, worse surface finish, and at the extreme, burned workpiece material or broken tooling.

Types of Coolant

Flood coolant: A stream of water-soluble coolant (usually a synthetic or semi-synthetic mixed to 5–10% concentration in water) pumped continuously over the cut zone. This is the standard for production machining of steel, stainless, aluminum, and most other metals. Flood coolant is what most Haas and Tormach machines use.

Mist coolant: A fine mist of coolant mixed with air. Provides some cooling and chip clearing with much less fluid use. Less effective than flood for heavy cuts but useful for cast iron (where flood can cause thermal shocking) and light finishing operations.

Air blast: Compressed air directed at the cut. No lubricating or cooling benefit from the fluid — it's purely chip evacuation. Excellent for cast iron (flood damages it). Also used in clean-room environments where coolant residue is unacceptable.

Through-spindle coolant (TSC): Coolant pumped through the spindle itself and out through holes in the cutting tool. Extremely effective — the coolant arrives right at the cutting edge, deep inside a pocket or hole where external flood can't reach. Standard on high-production machines. Haas offers TSC as an option. Especially important for deep hole drilling.

Dry machining: No coolant at all. Used for specific materials (some cast irons, certain composites, ceramics) and with specific tool geometries. Not appropriate for general steel or aluminum work.

Choosing Coolant for Material

| Material | Recommended Approach |

|---|---|

| Aluminum | Flood or mist with light cutting oil; some operations work dry with air blast |

| Mild steel | Flood with water-soluble coolant |

| Stainless steel | Flood — generous flow, chip evacuation is critical |

| Titanium | Heavy flood — titanium is a champion at retaining heat |

| Cast iron | Air blast only — flood causes thermal cracking |

| Plastics | Air blast or light mist; coolant can swell some plastics |

| Composites / graphite | Air blast; coolant contaminates many composite materials |

Coolant Concentration and Maintenance

Water-soluble coolants are mixed at specific ratios — typically 5–10 parts water to 1 part concentrate. Too lean (too much water) and you lose lubrication and get corrosion. Too rich (too much concentrate) and you waste money and may get foaming or biological growth.

Test coolant concentration with a refractometer — a handheld optical instrument that reads the refractive index and converts it to concentration. Check concentration weekly. In my shop, we kept a coolant log.

Coolant goes bad. Water-soluble coolant in a sump grows bacteria, develops smell, and loses effectiveness. Change your sump every 6–12 months, clean the tank, and start fresh. "Rancid" coolant is genuinely unpleasant to work around and corrodes your machine's ways over time.

---

The Setup Sequence: First Part to Production

Here's the step-by-step sequence I followed in my shop for a new job:

1. Read and Understand the Drawing

Before touching a machine, read the print (engineering drawing). Understand:

• What's the finished part geometry?

• What are the critical tolerances? (Anything tighter than ±0.005" needs special attention)

• What material?

• What surface finish is required? (Ra 125 microinch vs Ra 32 are very different)

• Are there any inspection requirements or certificates needed?

2. Plan Your Setups

A "setup" is one orientation of the part in the machine. Most parts require multiple setups — for example, mill one side, flip the part, mill the other side.

Plan the sequence of setups before programming. The most common mistake beginners make is starting to program without thinking about what features are accessible from which orientation, and how each setup will hold the part for the next one.

3. Prepare the Stock

Get your stock — a block of metal, a piece of bar stock — to a workable starting size. Most stock comes slightly oversized. For a milled part, you typically want a few thousandths (0.010"–0.030") of cleanup stock on the surfaces you'll be machining.

If you need precise stock dimensions, face mill the stock first to get known flat, square starting surfaces.

4. Load and Set Up in the Machine

• Mount the vise (if not permanent) and indicate it in parallel to the axis of travel

• Clamp the stock with appropriate parallels

• Load your tools in the correct pockets

• Measure and enter all tool length offsets

• Use edge finder or probe to set X/Y work offsets (G54)

• Set Z zero (typically top of stock)

5. Prove Out the Program

The first time you run a new program, do not run it at full feed rate.

Set the feed rate override to 25–50% on the machine control. Walk through the program slowly, watching every move. Verify:

• The tool is going where you expect

• Coolant comes on when it should

• Depths look correct

• Tool changes happen smoothly

On Haas machines, the Single Block mode (press SINGLE BLOCK button) runs one line at a time — you press CYCLE START for each line. Use this for the first few critical moves of a new program.

6. First Part — Inspect Everything

After the first part, measure it. Every critical dimension. Compare to the print. Typical things to check:

• Width and height of part

• Hole sizes and locations

• Depth of pockets

• Thread engagement

• Surface finish (visual check, or profilometer if required)

If something is off, diagnose why before running more parts. Is it an offset issue? A feed rate issue? Tool deflection? Thermal growth of the material?

7. Dial In and Run Production

Once the first part is good, verify offsets are still correct, set feed override to 100%, and run. Watch the first few production parts carefully. After that, sample-check every 5–10 parts, or at whatever frequency the job requires.

---

Safety: The Things That Can Hurt You

I want to end this series here because this is genuinely important and gets glossed over in tutorial content.

CNC machines can kill you. They are powerful industrial equipment that will continue doing what they're told regardless of what's in the way. A chip the size of a fingernail launched at 300 feet per second will go through unprotected skin. A broken end mill is a projectile. A part that comes out of the chuck is a projectile. Coolant mist over time is a respiratory hazard.

Safety non-negotiables:

• Eye protection, always. Safety glasses at minimum when the machine is running. Face shield for turning operations.

• Never reach into an enclosure while spindle is moving. Not for one second. E-stop first.

• No loose clothing, gloves, or jewelry near rotating equipment. Spinning chucks grab things. A ring on your finger near a lathe chuck can remove the finger.

• Know where the e-stop is before you press CYCLE START. Every operator, every time.

• Never leave a machine running unattended with new programs or new setups.

• Chips are sharp. Use a brush to clear chips, not your hand. Aluminum chips look innocent and have edges like razor wire.

The machines that injure people are almost always doing exactly what they were told to do. The error is in the setup, the program, or the inattention of the operator. Pay attention. Slow down. Verify before you run.

---

Where to Go From Here

You've finished the mini-course. Here's what I'd suggest for next steps depending on where you are:

If you want hands-on experience: Look for a local makerspace with CNC equipment. Most have training programs. Getting time on a real machine — even a small router — is worth more than all the reading in the world.

If you're buying a machine: For home shop, look at the Tormach 440 or 770, or a desktop CNC like the Nomad from Carbide3D for lighter work. For a serious small shop, the Tormach 1100MX or a used Haas Mini Mill are excellent starting points.

If you want to go deeper on CAM: Spend time in Fusion 360. Model a bracket with multiple features, create a full toolpath sequence, simulate it, and post-process it. There is no substitute for doing the work.

If you're going professional: Consider a community college machining program. The fundamentals — manual lathe, manual mill, measurement, print reading — taught in a structured environment are irreplaceable. Many programs have excellent equipment and experienced instructors.

Machining is one of those disciplines where the more you know, the more you realize how much there is to learn. I ran a machine shop for years and still regularly encountered situations that required research, experimentation, or calling someone smarter than me.

That's what makes it interesting.

— Dr. Scott

---

This is Part 8 (the final installment) of the CNC Machining Mini-Course. The full series: