CNC Setup: Workholding, Work Zero, and Tool Offsets

Setup is everything that happens before the first good part. You hold the work so it cannot move, tell the control exactly where the part is, tell it exactly how long and how wide each tool is, and then prove the program slowly. A good program with a bad setup breaks tools. Crashes and first-part scrap often trace back to one number entered wrong, so the habits here are about getting each number right and checking it before the machine moves fast.

What You Will Be Able to Do

• Work through a job package and choose how the part is held.
• Indicate a vise to the right target and set work zero with an edge finder or probe.
• Explain what each tool offset stores and set one by touch-off, presetter or tool setter.
• Prove a new program with a dry run, then single block and reduced feed on the first part.
• Correct size with wear offsets on a mill and a lathe, including the half-the-diameter rule.

The Setup Sequence

This is the order most shops follow on a machining center. A lathe follows the same logic with a chuck and turret.

1. Read the job package.
2. Gather tools, holders, inserts and workholding. Replace worn inserts now, not later.
3. Clean the table and mount the workholding, then indicate it.
4. Load and clamp the workpiece.
5. Load tools at the correct stickout (how far the tool sticks out of its holder) and in the correct pockets.
6. Set work zero.
7. Set tool length and diameter offsets.
8. Load the program and confirm its number and revision match the job.
9. Dry run.
10. Run the first part in single block at reduced feed.
11. Inspect the first part, correct with wear offsets and get sign-off.

Reading the Job Package

Read the print first, then read it again. Scrap often starts with a missed note or a misread tolerance. Check the revision on the print against the work order. Look for material, finish requirements and any geometric tolerance callouts that need a special measuring method. If the setup sheet and the print disagree, stop and ask.

Workholding

Workholding keeps the part from moving against cutting force. Choosing it is a tradeoff between grip, access for the tool and how fast you can load the next part.

Indicating a Vise

A vise that is crooked on the table cuts every feature crooked. Use a dial test indicator mounted in the spindle.

1. Clean the table and the bottom of the vise. Stone off any burrs.
2. Set the vise down and snug the bolts lightly.
3. Touch the indicator to the fixed jaw and zero it at one end.
4. Jog along the jaw and read the change over its length.
5. Tap the far end of the vise with a soft mallet to bring the reading down, then sweep again.
6. Tighten the bolts in steps, sweeping again each time, because tightening can move the vise.

Target: On general work, hold the change to 0.001 inch or less across 6 inches. On precision work, hold it to 0.0005 inch. If the setup sheet gives a tighter number, it wins.

Example: you sweep a 6-inch jaw and read 0.003 inch of change from end to end. That fails for general work. Tap the far end of the vise a little at a time, sweeping after each tap, until you are at or under 0.001 inch.

Clamping the Part

• Clean the jaws and parallels. One chip can tilt the part by more than your tolerance.
• Tighten the vise, then tap the part down with a dead-blow mallet until the parallels no longer slide.
• Leave enough part above the jaws for the tool to reach every feature, and enough in the jaws to hold it.
• On a lathe, use the jaw pressure on the setup sheet. Too little lets the part spin or fly out. Too much crushes a thin wall out of round.
• Remember that a chuck loses grip as RPM rises, because the jaws are pulled outward. Stay under the chuck's rated speed.

Warning: A part that comes loose at speed becomes a thrown object. After clamping, check the part by hand, and check that the chuck is fully closed before you start the spindle.

Setting Work Zero

Work zero is the point on the part that all the program's numbers are measured from. The setup sheet tells you where it goes. You find that point and store its machine position in a work offset, such as G54.

Using an Edge Finder

An edge finder is a two-piece spindle tool. Its tip wobbles while it runs off center, then runs true, then kicks sideways the moment it touches the part. When it kicks, the center of the spindle is exactly half the tip's diameter away from the edge.

1. Put the edge finder in the spindle and run it at about 800 to 1,000 RPM, or the speed its maker lists.
2. Jog slowly toward the edge in X using a fine handwheel step.
3. Stop the instant the tip kicks sideways. Back off and repeat to confirm the reading.
4. Note the machine position, then add or subtract the tip's radius to find the edge.
5. Store that number in the X register of the work offset.
6. Repeat for Y.

Worked example with a tip 0.200 inch in diameter, so its radius is 0.100 inch. You move in the plus X direction toward the left edge of the part, and the tip kicks at a machine position of X -18.4620. The edge is 0.100 inch farther on in the direction you were moving, so the edge is at -18.4620 + 0.100 = -18.3620. Enter -18.3620 in G54 X. If you had come at an edge moving in the minus direction, you would subtract the radius instead. Many controls have a measure key that does this math, but you should still know what it is doing.

To find the center of a round bore or boss, sweep it with a dial test indicator in the spindle and move the axes until the reading stays the same all the way around.

Setting Z

Z zero is usually the top of the finished part. Touch a known tool or a gauge block on that surface and enter the result. If you use a block, remember to take its thickness out of the number. How you enter it depends on whether your shop keeps the height in the work offset or the tool length offset, covered below.

Using a Probe

A spindle probe touches the part and sets the work offset in seconds. It runs a stored routine and stops when the stylus contacts the part. Three habits keep it accurate.

• Calibrate the probe on a known bore or surface on the schedule your shop uses.
• Position it close to the feature by hand, using a slow feed. A stylus that hits something at rapid speed will break, and the probe can be damaged.
• Check the offset it wrote. A probe with a bent stylus gives a confident wrong number.

Work Zero on a Lathe

On a lathe, X zero is always the spindle centerline, so you do not hunt for it. Z zero is usually the finished face of the part. Face the part or touch the face with a tool, then set Z from there.

Setting Tool Offsets

Tool Length Offsets

Every tool in the magazine is a different length. The tool length offset stores a Z distance from a reference point to that tool's tip, so the control knows where the cutting edge is no matter which tool is in the spindle. The program calls it with G43 and an H number. If a value is wrong by half an inch, the tool goes half an inch too deep, and it may do that at rapid speed.

Shops use one of two methods. Learn which one yours uses before you touch anything.

• Length stored from the part. Each tool is touched to the top of the part and the machine Z position goes in its H register. G54 Z stays at 0. For example, tool 1 touches at Z -11.2750, so H1 is -11.2750. Tool 2 is longer and touches at Z -9.8640, so H2 is -9.8640.
• Length stored from the spindle. Each tool's true length from the spindle gauge line goes in its H register, such as H1 = 4.1250. The distance down to the part goes in G54 Z once. This suits presetters, because tool lengths do not change when the part changes.

You can set length three ways.

A tool presetter measures length and diameter away from the machine, optically or with a contact, while the machine keeps cutting. You enter the numbers or send them over a network, so setup time on the machine drops.

Tool Diameter Offsets

When a program uses cutter compensation (G41 or G42), the control shifts the tool sideways by its radius so the side of the tool cuts on the part's line. The D register stores that size. Three things to check:

• Your control may expect a radius or a diameter. For a 0.500-inch end mill, radius mode wants 0.250, and diameter mode wants 0.500. Enter it the wrong way and every wall is off by a large amount.
• Some CAM programs already include the tool size. In that case the D register holds only a small correction, close to zero. Ask how the program was posted, and put a full radius in only if it calls for one.
• Check the real diameter of a reground tool. It may be smaller than the number printed on it.

Lathe Tool Geometry

A lathe tool needs an X and a Z geometry offset, set from a real cut.

1. Take a light cut on the diameter and stop the spindle.
2. Measure the diameter with a micrometer.
3. Enter the measured value in the X measure field for that tool.
4. Touch or face the end of the part and set Z.

Tool Nose Radius Compensation

A turning insert has a small rounded tip, not a sharp point. On a straight diameter or a flat face, this does not matter. On a taper, chamfer or arc, the rounded tip cuts in a different place than a sharp point would. Tool nose radius compensation corrects for that, using G41 or G42 in the program plus two values on the offset page.

• R is the nose radius. You get it from the insert, not from memory. The last digit of an inch code such as CNMG 432 gives the radius in 64ths of an inch, so 2 means 1/32 inch. In a metric code such as CNMG 120408, the last two digits give tenths of a millimeter, so 08 means 0.8 mm.
• T is the tip orientation number, which tells the control which way the tool points. Your offset page or manual shows a diagram.

If the R value is wrong, straight diameters and faces still measure correctly, which can fool you. Tapers, chamfers and radii come out wrong, because the control is correcting for a tip that is not there. As an example, a 1/32-inch value entered for a 1/64-inch insert leaves a 45-degree chamfer off by about 0.009 inch along each axis. Whenever you change to a different insert, check that R and T still match.

Proving the Program

Dry Run

A dry run is a full run of the program with no cutting, so you can check the toolpath and clearances before a mistake can break anything. A programming or offset error found here costs nothing. Depending on your shop, you may run with no part loaded, or with a raised work offset so that every move stays well above the part and clamps, or with the control's graphics. Some controls also have a key labeled Dry Run that changes feed rates, so learn what it does on your machine.

Watch for:

• Tool changes in the right order, with the right tools.
• Rapid moves that come close to the part, vise or clamps.
• Anything that looks unlike what the setup sheet describes.

Single Block and Reduced Feed on the First Part

The first real part is run by hand, one line at a time.

1. Turn on Single Block. The machine now stops after every line.
2. Set feed override to about 50 percent, and turn rapid override down as well.
3. Keep one hand on feed hold.
4. Press cycle start for each line and read the next line on the screen before you press again.
5. As a tool nears the part, compare the distance-to-go display with the gap you can see. If the screen says 2.000 inches to go and the gap is 0.500 inch, press feed hold. Something is wrong.
6. After a tool has made its first cut safely, you can release single block for that tool if your shop permits it, but keep the feed down until the tool has proven itself.
7. Stop if anything looks or sounds wrong.

Run slowly. You can always speed up later, but you cannot undo a crash. For a tight diameter, you can also put a small extra amount in the wear offset for the first part, so it comes out slightly oversize. You then measure and bring it down to size without any risk of cutting under.

First Part Inspection

1. Take the part out and clean it.
2. Look it over for burrs, tool marks, missed features and poor finish.
3. Measure every dimension on the print with the right tool. A caliper suits general dimensions. A micrometer suits about plus or minus 0.001 inch or tighter. Use pin gauges for holes, thread gauges for threads, and a height gauge or CMM for complex features.
4. Record the results as your quality system requires.
5. Correct the offsets so dimensions land near the middle of the tolerance, not just inside the limit. That leaves room for tool wear.
6. Get sign-off from your lead or inspector before you run more parts.

Wear Offsets

Geometry Versus Wear

Each tool has two sets of numbers. Geometry offsets say where the tool is. Wear offsets are small corrections added on top. During a run, change wear, not geometry. If you change geometry and later replace the tool, your baseline is gone. When you change an insert, reset the wear value as your shop directs.

The Half-the-Diameter Rule

A diameter is cut from both sides of the centerline. If you move a turning tool 0.001 inch closer to center, the radius drops 0.001 inch and the diameter drops 0.002 inch. So to fix a diameter error, the tool has to move only half the error.

What you type depends on how your control is set up.

• Diameter mode: The X wear offset is in diameter values, as on most lathes. You type the full diameter error, and the control moves the tool half of that.
• Radius mode: The offset is in radius values. You type half the diameter error yourself.

Find out which mode your machine uses before you touch an offset. The same number moves the tool twice as far in one mode as in the other.

Lathe examples:

Notice the bore rows. A boring bar cuts on the inside, so the signs work the opposite way from an outside diameter. Lengths are not doubled. If a lathe shoulder is 0.005 inch short, enter the full -0.005 inch in Z wear.

Wear Offsets on a Mill

With cutter compensation, a smaller D value makes the control treat the tool as smaller, so it moves closer to the wall. That removes more stock whether the wall is on the outside of a boss or the inside of a pocket. A width or diameter has a wall on each side, so the half rule applies there too.

If you are correcting a single wall, measured from a datum, the tool moves the full error. For depth, a pocket that is 0.003 inch shallow needs the full -0.003 inch in the tool's length wear offset. Depth is never halved.

How to Make a Wear Correction

1. Measure the part carefully, ideally on two or three parts so you do not chase one odd reading.
2. Compare the result to the middle of the tolerance, not to the limit. If the print says 1.000 plus or minus 0.002 and you measure 1.0015, the part is good but the error from the target is +0.0015.
3. Decide whether the feature is a diameter or width, or a single wall or depth.
4. Decide the direction, then the amount for your control's mode.
5. Enter the change, using a decimal point. Many controls have two keys here, one that replaces the value and one that adds to it. If the wear value is already -0.0015 and you replace it with -0.002, the tool only moves 0.0005 inch.
6. Make small corrections, usually 0.001 to 0.005 inch at a time, and check the next part.
7. Record the change on your log.

A big or sudden correction is a warning. Tools wear gradually. If a part needs 0.010 inch all at once, look for a broken insert or a loose part before you touch an offset.

Common Setup Mistakes

Check Your Understanding

1. You sweep the fixed jaw of a vise and read 0.002 inch of change over 6 inches. The job is general work. What do you do?

Keep adjusting. The target is no more than 0.001 inch over 6 inches for general work. Tap the high end, sweep again, and sweep once more after the bolts are tight.

2. An edge finder with a 0.200-inch tip kicks at machine X -9.2100 as you move in the plus direction. Where is the edge?

The spindle is one tip radius, 0.100 inch, short of the edge. Add it in the direction you were moving, so the edge is at X -9.1100.

3. Your lathe runs in diameter mode and an outside diameter measures 0.005 inch oversize. How far must the tool move, and what do you enter?

The tool moves 0.0025 inch closer to center. In diameter mode you enter -0.005 in X wear, and the control moves the tool half of that. In radius mode you would enter -0.0025.

4. After an insert change, all the diameters on a lathe part are correct, but the chamfers and the taper are off. What do you check?

The tool nose radius value and tip orientation on the offset page. Straight diameters are not affected by a wrong value, but angled and curved surfaces are.

5. The setup is proven in a dry run, but this is the first part with material in the machine. How do you run it?

Single block on, feed override around 50 percent, rapid override turned down, one hand on feed hold, and compare distance-to-go with the real gap as each tool approaches.

Key Takeaways

• One wrong number can break a tool or scrap a part. Check each one before the machine moves fast.
• Indicate a vise to 0.001 inch over 6 inches for general work and 0.0005 inch for precision work.
• An edge finder kicks with the spindle half a tip diameter from the edge.
• A diameter error needs the tool to move half that amount. Know whether your control wants the full error typed or half.
• Dry run first, then single block at reduced feed on the first part.
• Use wear offsets during a run, aim for the middle of the tolerance, and write down every change.