It is important to check that your tool isn't going to collide with the work holding before you run every program. Fortunately it is super easy, and there are many ways to do it. The most reliable method is to handle jog a tool to the deepest point of your program and carefully move it over the vice.

Start by probing your origin and all your tools. Then, to find the deepest z of your program you can simulate the toolpath. In simulation make all the toolpath visible and show all the different parts of the toolpath. It can be helpful to turn the stock off and make the model transparent so you can see all the toolpath at once. Then you can click on the lowest point in the toolpath and the simulation will jump to that point.

Once you are at the deepest part of your toolpath go to the info section of the simulation to find the z height.

Use the handle jog to move the tool to the deepest z somewhere away from the vice. Then slowly move towards the vice, while checking if the tool with collide. When it gets close a piece of paper or a ruler can help you check if it will collide.

If there is minimal gap, check both sides of the vice jaws, because they can be different heights.

You can use the same method to check clearance to other objects in x and y: for example if there is a second vice mounted in the machine.

Bad work holding

• Avoid having excessive stock stickout
• Ensure there is minimum 3mm stock in the vice
• Clean everything well to avoid getting chips between the part and the vice
• Serrated jaws increase grip
• Some jaws have a dovetail on top, and you can cut a matching dovetail in your stock for extra strong work holding

Long tools

• The rigidity of the tool is proportional to the diameter to the power of 4 and the stickout to the power of 3. So doubling the tool diameter increases rigidity by 16 times and halving the stickout increases the rigidity by 8 times
• Try to use the shortest possible tool and holder for the job to minimize vibration
• If you need a long tool try to use the biggest size possible
• Higher flute count also makes tools more rigid because there is less material removed
• There are fancy tools with variable helix angles that can help avoid resonance

Excessive tool engagement

• Less stepover reduces cutting pressure.
• Adaptive clearing can reduce (but doesn't eliminate) sudden spikes in tool angular engagement.
• Use "feed optimization" setting to slow the feed rate on corners. See the advanced feed and speeds module for more information.
• If there is vibration due to excessive tool engagement it is much better to reduce the stepover than the feed, because reducing feed can cause rubbing.

Runout

Runout is a measurement of how concentric the tool is with the spindle center of rotation. It can be measured (in microns) with a dial indicator.

Runout is especially dangerous when cutting small chip thicknesses because it changes the amount of material each flute removes. This can overload one cutting edge and cause wear or breakage.

Rubbing

Rubbing happens when the cutting tries to cut a chip thickness so small that it rubs against the material instead of cutting. Rubbing can be fixed by increasing the feedrate. There is more information on rubbing and chip thickness in the advanced feeds and speeds.

Bad force distribution

Cutting mainly on the tool tip (traditional milling) causes more deflection than cutting deeper and spreading the load along the whole side of the endmill (high efficiency milling).

Cut stability (Expert content)

As an endmill rotates the flutes contact the material and while they are in contact the endmill experiences a sideways cutting force. Because the flutes are not always in contact with the material the cutting force will vary through each revolution, causing vibration.

If the cutting force is low and your setup is rigid vibration from bad cut stability is not usually a problem. However if you want nicer surface finish or are experiencing vibration issues it is good to check your cut stability.

Check your cut stability

Bad cut stability

Low depth of cut, large width of cut, single flute endmill: the one flute contacts material 50% of the cut and there is no contact 50% of the cut. The endmill is experiencing periodic force which can cause vibration and possibly resonance.

Ramping

Vibration

Vibration is the most important factor for improving surface finish and is discussed in its own section above.

Stepover cusp height

The next most important factor is stepover when doing surface finishing using ball or bull nose endmills. Due to the rounded profile small cusps are left between passes creating surface roughness. Use a cusp height calculator to determine how high these cusps will be.

The best way to reduce the cusp height is to use the largest radius tool possible. You can also reduce the stepover but this will increase the machining time.

Feed per tooth

The feed per tooth for all tools affects the theoretical surface roughness on vertical walls in exactly the same way as cusp height with ball mills. Between each circular cut there is a uncut cusp of metal. Higher feed per tooth increases the height of the cusp and therefore increases surface roughness.

You can use the same calculator to determine feed per tooth cusp height, just enter the feed per tooth where it asks for stepover. However, the theoretical surface roughness from this factor is very small (0.001-0.3 Ra), much smaller than realistic milling surface finishes. This is because bad surface finishes are mostly caused by vibration, not feed per tooth.

Tool sharpness

In soft materials (aluminium, brass, plastic...) sharper tools will create a better surface finish.

In hard materials (ferrous, titanium...) sharp edges are too fragile and break or dull quickly, which leaves a worse surface finish. In hard materials it is better to use a coated tool that is less fragile. The coating adds a radius to the cutting edge, so coated tools will always be duller than uncoated tools.

No tool cuts what was programmed perfectly: tools bend due to cutting pressure and tool diameter wears over time. In order to hit a desired tolerance you have to measure and account for the errors of your tool.

1. Roughing: remove all material except for twice the thickness of the finishing stepover.
2. Test cut: Take a cut identical to the final cut, same stepover, feed per tooth and speed. Leave one finishing stepover stock to leave.
3. Measure: you can measure manually or use the probe.
4. Adjust final cut depth: you can manually edit the stock to leave in fusion or update the tool wear in the controller and set the fusion toolpath to wear compensation.
5. Final cut: if the test cut size was inaccurate the cutting pressure in the final cut will be different to the test cut.
6. Measure: Always check before you remove the part from the machine.

Example: I want to make a bore between 49.995 and 50.005mm. I will use a 0.5mm finishing stepover. The finishing stepover can't be too small otherwise the difference between the test cut stepover and the final cut stepover can be a large percentage.

1. Rough all material with 1mm stock to leave. The toolpath is aiming for a 48.000mm bore.
2. Finishing contour removes 0.5mm and leaves 0.5mm stock. The toolpath is aiming for a 49.000mm bore.
3. I measure the bore and it is 48.900mm. This means the tool is cutting 0.05mm less than the target.
4. I program the final toolpath to aim for 50.100mm, so a -0.05mm stock to leave. Or I could enter 0.05mm wear into the controller if using wear offsets.
5. The final cut removes 0.55mm, which is 10% more stepover than the test cut.
6. I measure the final bore as 49.996, which is within tolerance but slightly small than the expected 50.000. This is because the final cut had 10% more tool pressure that the test cut.

It is also good practice to measure the bore at multiple depths to check if it tapers. Multiple finishing passes can reduce tapering.

Machine base leveling