"

9.9 Spindle Speed, Feed Rate, Depth Of Cut And Finish Allowances

Micky R. Jennings

Spindle Speed

Milling machines have the same spindle speedcalculation as the rest of the rotational tools in the shop. Based on surface feet per minute (SFPM) of a tool and the cutting conditions, the operator can calculate the appropriate RPM.

On the left, the end of an end mill is shown from a top down view, questioning the number of clockwise rotations. On the right is a clock showing one minute of time.
Figure 9.132. On the left, the end of an end mill is shown from a top-down view, questioning the number of clockwise rotations. On the right is a clock showing one minute of time. / Image Credit: Micky R. Jennings, courtesy of Wenatchee Valley College, CC BY 4.0

Milling machines are machine tools that can utilize carbide tooling. In these instances, it is always a good idea to consult the manufacturer for the correct surface feet per minute for the tool in a specific material. If there is no technical data on the tool to be usedavailable, a conservative starting point would be 4x the SFPM of HSS.

For example, the calculation for cutting mild steel with a 1/4 carbide end mill would be:

Another example is the calculation for cutting aluminum with a 3/4 HSS end mill.

Feed Rate

On the left, the end of an end mill is shown from a top down view, indicating the distance traveled along a workpiece in inches. On the right is a clock showing one minute of time.
Figure 9.133. On the left, the end of an end mill is shown from a top-down view, indicating the distance traveled along a workpiece in inches. On the right is a clock showing one minute of time. / Image Credit: Micky R. Jennings, courtesy of Wenatchee Valley College, CC BY 4.0

Manual milling machines have a side cutting feed ratethat is expressed in Inches Per Minute (IPM). This feed rate is completely independent of the rotation of the spindle. The formula to calculate the feed rate is:

The end of an end mill is shown, engaged in the work, from a top down view. Giving an indication of the chip size, in thousandths of inches, that a single cutting edge would remove from the work.
Figure 9.134. The end of an end mill is shown engaged in the work from a top-down view. An indication of the chip size, in thousandths of inches, that a single cutting edge would remove from the work is shown. / Image Credit: Micky R. Jennings, courtesy of Wenatchee Valley College, CC BY 4.0

The chip load per tooth (CPT) is another area where the manufacturer will have some helpful information about their product. If that information isn’t available, the following generalized conservative estimate can be used to get the operator started.

As the tool size gets larger and stronger, more CPT can be taken with the tool without damaging it.

For example, let’s calculate roughing out aluminum with a 2 flute 1/2″ carbide end mill.

First, the RPM:

Now the CPT:

Now the feed rate formula can be calculated:

Author’s Tip

Whenever I am calculating spindle speed in RPM or feed rate in IPM, I take my answer and round it to the nearest 50 RPMs or nearest whole IPM. This makes sense for manual equipment because the machine isn’t accurate to single RPMs or decimal points of IPM, but it will also make sense later on if you utilize a CAM system to aid you in writing technical programs for CNC machines. This rounding generally won’t hurt the tool or the part.

Depth of Cut

On top, the end of an end mill is shown engaged in the work, from a top down view, indicating the radial depth of cut in thousandths of an inch. On bottom, the side of an end mill is shown engaged in the work, from a front view, indicating the axial depth of cut in thousandths of an inch.
Figure 9.135. On top, the end of an end mill is shown engaged in the work, from a top-down view, indicating the radial depth of cut in thousandths of an inch. On bottom, the side of an end mill is shown engaged in the work, from a front view, indicating the axial depth of cut in thousandths of an inch. / Image Credit: Micky R. Jennings, courtesy of Wenatchee Valley College, CC BY 4.0

Depth of cut is the amount of the tool engaged in the work while making a cut. On a milling machine, the depth of cut can be axially or radially measured. Depth cuts axially use the tip of the tool more heavily and have a tendency to wear the tool out prematurely. Radial depth cuts use a larger portion of the cutting edges and are generally preferable as the tool will last longer.

On manual milling machines, heavy depth cuts in steel are best performed with roughing end mills. In aluminum, depth cuts can be taken with standard finishing end mills. Aluminum cuts more freely, and the machine can handle the forces of the cuts much better than large steel cuts.

Roughing cuts in steel and aluminum can be taken at 1x diameter radially and ½x diameter axially, or ½x diameter radially and 1x diameter axially. This is just a starting point. The operator can adjust to suit different machines and situations.

For example, when roughing the side of a ½” thick piece of steel with a ½” HSS roughing end mill, the operator could cut ¼” step over at the entire ½” thickness of the material.

Another example is roughing a 1″ slot, 1″ deep, in aluminum, with a ¾” end mill.  In this case, the operator could cut the full width of the endmill at ⅜” depth cuts.

Finishing Allowance

The side view of a part with finishing allowance on floor and wall indicated in red.
Figure 9.136. The side view of a part with finishing allowance on floor and wall indicated in red. / Image Credit: Micky R. Jennings, courtesy of Wenatchee Valley College, CC BY 4.0

The finishing allowance is the intentional amount of material left on surfaces by the roughing tool. Leaving an allowance for finishing is essential for getting a quality final cut. If too much material is left for finishing, the surface finish and/or accuracy may suffer. If too little material is left, the finishing tool may not completely clean up what the roughing tool left behind. Following a few basic guidelines, and experimentation, the machinist will have success.

When using roughing end mills, the machinist should leave 1/32″ to 1/16″ on the walls and 1/64″ on the floor of features. This is because the rough texture left by roughing end mill leaves is deceiving and impossible to measure accurately. After the roughing end mill removes material, a finish end mill will need to be used to clean up the sides before an accurate measurement can be made and the true finish pass can be executed.

When cutting with a finish style end mill for roughing cuts, the operator should leave around 1/64″ on the wall and floor of features. Finish style end mills are much more capable of accurate cuts than roughing end mills. These values can also be used for a semi finish pass after using a roughing cutter.

In between the roughing and finishing passes, the operator should accurately measure the part to make sure they know how much material is remaining and calculate how to adjust the machine to remove the excess material.

The finish pass should take the final amount off the walls and floor simultaneously so that the tool only runs across the surfaces one time.

Conventional Milling and Climb Milling

On top, the end of an end mill is shown from a top down view, indicating the cutting edges entering the material thick and exiting thin. On bottom, the end of an end mill is shown from a top down view, indicating the cutting edges entering the material thin and exiting thick.
Figure 9.137. On top, the end of an end mill is shown (top-down view) indicating the cutting edges entering the material thick and exiting thin. On bottom, the end of an end mill is shown (top-down view) indicating the cutting edges entering the material thin and exiting thick. / Image Credit: Micky R. Jennings, courtesy of Wenatchee Valley College, CC BY 4.0

Conventional milling and climb milling are different ways to remove material when cutting with the side of a milling tool. It is important to know the difference because it can determine whether an accurate part with good surface finishes or a rough-looking scrap part and/or potential broken tooling will result.

Conventional milling happens when the base material is moving in the opposite direction as the cutting teeth. This method of cutting often leaves a poor finish. This is because any chips that may get recut and pounded into the surface will do so at a position where the cutter is entering the finished part. When chip fragments are imbedded into the surface the finished part appears cloudy or rough. The cutter enters the material at its thinnest point on the part’s surface and exits at the full chip load thickness at the point where the chip is removed. Although the finish isn’t great, this is a much safer cut on a manual milling machine. This is because the cutting action of the tool is pushing directly against the lead screw, keeping the backlash out of the equation. Conventional milling is great for all the roughing operations that need to be made on a manual mill.

Climb milling happens when the base material is moving in the same direction as the cutting teeth. This method of cutting leaves the best finish. This is because any chips that may get recut and pounded into the surface will do so in a position where the cutter is entering waste material. The cutter enters the material at the full chip load amount and exits thin at the finished part surface. Because the work is moving in the same direction as the cutting teeth, machines with backlash will have a tendency to automatically pull the material into the backlash slop. This involuntary movement prematurely increases the size of the chip load, causing a runaway chain reaction that could break the cutter and ruin the part. For this reason, climb milling on manual machines is best left for light finishing cuts of no more than 1/64″.

Traditionally, a machinist will make all the roughing cuts using conventional milling, leaving .005″ to .015″. Utilize precision measuring techniques while the part is still in the machine. Then climb mill the remaining material for a finish pass.

Attributions

  1. Figure 9.132: Rotation per minute – milling machine by Micky R. Jennings, courtesy of Wenatchee Valley College, for WA Open ProfTech, © SBCTC, CC BY 4.0
  2. Figure 9.133: Feed rate – milling machine by Micky R. Jennings, courtesy of Wenatchee Valley College, for WA Open ProfTech, © SBCTC, CC BY 4.0
  3. Figure 9.134: Chipload per tooth – milling machine by Micky R. Jennings, courtesy of Wenatchee Valley College, for WA Open ProfTech, © SBCTC, CC BY 4.0
  4. Figure 9.135: Depth of cut – milling machine by Micky R. Jennings, courtesy of Wenatchee Valley College, for WA Open ProfTech, © SBCTC, CC BY 4.0
  5. Figure 9.136: Finishing allowance – mill by Micky R. Jennings, courtesy of Wenatchee Valley College, for WA Open ProfTech, © SBCTC, CC BY 4.0
  6. Figure 9.137: Climb vs conventional illming – milling machine by Micky R. Jennings, courtesy of Wenatchee Valley College, for WA Open ProfTech, © SBCTC, CC BY 4.0
  7. Video 9.21: Micky R. Jennings, courtesy of Wenatchee Valley College, for WA Open ProfTech, © SBCTC, CC BY 4.0
  8. Video 9.22: Micky R. Jennings, courtesy of Wenatchee Valley College, for WA Open ProfTech, © SBCTC, CC BY 4.0
definition

License

Icon for the Creative Commons Attribution 4.0 International License

Introduction to Machining Copyright © by SBCTC is licensed under a Creative Commons Attribution 4.0 International License, except where otherwise noted.

Share This Book