Introducing CNC Explorer 1.0
To make clean efficient cuts on a CNC Router, picking the proper feed rates and spindle RPM is crucial. But many are not sure how this is accomplished and end up using settings that lead to poor cuts and premature wear on their tools. The CNC EXPLORER is a tool to help understand various settings on a CNC Router. Interactive adjustments encourage the exploration of different settings and trade-offs. The tool monitors settings that would create over-stresses on the CNC system. The result is a set up within the capabilities of the machine tooling producing a good efficient and safe cut.
Features of CNC Explorer 1.0
- Graphical Materials Table for 1/8″, 1/4″, 3/8″, and 1/2″ Router Bits with an Area for Custom Materials.
- Suggested Router Spindle RPM Settings.
- Chip Load Values for each Material and Bit Selection.
- Ability to configure 2 different Router/Spindle Limits for A/B Comparison.
- Editable Section for the CNC Feed Rate Limits.
- Sliders and Scroll Buttons to Experiment with different RPM and Chipload Combinations.
- Scroll Buttons to Select Bit Diameters and Number of Flutes
- Ability to “Dial” down the Settings to a SAFE mode Reducing Feed Rates and RPM Speeds,
- Toggle Buttons Course and Fine to program Depth of Cut and Width of Cut.
- CNC Explorer will Calculate A Chip Thinning Adjustment and can be applied to your Setup.
- Surface Speed SFM, Material Removal Rate, and Required Motor HP are Calculated and Displayed.
- Spindle Wattage is Monitored and Warnings Reported Against Programmed Limits.
- Spindle RPM and CNC Feed Rates are Calculated with/without Chip Thinning Compensation.
Compatible with Excel 2003 and up and with Free LibreOffice 6.4.
Offered with free upgrades until next major revision.
Free Limited Version
Using CNC Explorer 1.0
CNC Router Basics
A CNC Router cutting or milling operation moves a rotating cutting tool bit along a programmed path that controls how fast the tool is spinning, how fast it is being moved, and how deep into the material is being cut. This is generally called a path. To complete a milling operation, it often takes many passes of varying depths. The depth may be dynamic as in the case of a 3D carving but the amount of material removed can be called the pass depth. Related to the depth of a pass, stepover controls the overlap the cutting bit makes on each pass. Fine steps result in a high-quality finish but require many passes. Making the stepover larger results in faster cut times but leaves small ridges on the surface that will be cleaned up with a finishing pass with the smaller stepover setting.
But the intention of this instruction set is not to explain all that entails CNC Router applications as that is a book onto itself. But rather to explore some of the things that affect the cutting operations and to gain a better understanding of how and why the CNC settings are chosen.
CNC Explorer has 3 major sections
- The Materials Section.
- Spindles and CNC Definitions and Limits
- CNC Explorer Dashboard
The first consideration has to be what type of material are you going to mill. Each type of material requires a unique set of parameters and settings to optimize the milling operations. While not required choosing a good set of parameters will result in the best finish. That is not always possible however given the limits of your equipment. Often compromises and trade-offs must be made. And that is what the CNC Explorer is all about.
Included in the tools is a sample table of materials. For each type of a set of graphical ranges for 4 different diameter tool bits, 1/8”, ¼”, 3/8”, and ½”. You can select the material you are working on and the ranges will be copied next to a chart of “Chip Load” per cutting edge ranging from 0.001 in. to 0.030”. Depending on which diameter bit is selected the corresponding range for that tool will be highlighted in YELLOW. Comparing this range with the Chip Load chart will determine the optimum range of Chip loads to use. In the above example “Hard Wood” was selected with a ¼” or 0.25” bit. Matching with the Chip Load chart we can see the optimum range would be 0.010” to 0.012”. Also, note the Dark-Green highlighted cell in the Chip Load chart. This is the exact target picked for the calculations.
There is an editable section to the right to add custom materials and bits.
Router/Spindle CNC Configuration and Limits Section.
The left side is the section to input information for your Router or Spindle. The light blue cell can be edited. There are to columns for Spindles which allow you to compare to different units to help understand the limits of each for the kind of milling you want to do. Typically, the choice is either a Trim Router such as the Makita RT071C or a water-cooled 3-phase Variable Frequency Drive controlled unit. The trim router is the cheaper option and for the most part, it works well except for the larger diameter bit that needs slower speeds. A spindle can run at a much lower RPM but not as fast as the trim router and cost considerably more. Often stated the other benefits of a spindle are much quieter running and less maintenance. After naming your spindle and or optional second, you set the minimum and maximum RPM range. Lastly, you enter the power of the spindle in Kilowatts. (KW)
The third column is for your CNC machine. You can also name it but you need to put in the min/max capability of the machine to move the spindle in inches per minute (ipm). Now the CNC Explorer knows the limits of your machines. If any configuration exceeds your equipment ranges a Red Flag will trip in various locations letting you know you will need to back off on some setting for your system to be able to make the milling operation. With experience with your CNC, you might know for a particular cut you machine has much lower limits. You can always change the limits to match the conditions. Or perhaps you want to be ultra-conservative and you can adjust the limits as well. You will note some of the cells are highlighted in green. This will be described more later but the CNC Explorer always keeps track of your equipment ranges and those are highlighted in green as you make adjustments.
CNC Explorer 1.0 DashBoard
The Dashboard is the main control and display section. In the left area is a slider control of the Spindle/Router RPM. Speed of the Spindle/Router can also be typed in directly in the blue box above. Next to that box is a switch to select which of the configured Spindle/Routers will be used in the power limit warnings. The Green box shows the current Chip Load Target selected. The target can be set in a few ways. The value can be typed in directly in either the green readout box above or in the Chip Load Selector window. Clicking on the grey button will open a drop-down selection scroll list where the target can be selected. And finally just clicking on the selector and using the Keyboard Up and Down Arrow keys will cycle through the Chip Loads. The target will be displayed and also highlighted in the Chip Load list used to match up with the material/bit ranges.
The middle area of the Dashboard is the cutting parameter controls. There is a dropdown list of Router Bit Diameters to chose from. Also, the number of Flutes or Cutting edges on the router can be assigned. A Tunning Slider modifies the RPM and Feed Rate from a SAFE 80% of the calculated results all the way up to 100%. Depending on the CNC design and Spindle along with the type of cut it is advisable to program in the Safe Mode. If the CNC controller on the machine has a similar function, using the Tunning might not be needed. But at times spindle power will be high to Max and the settings need to be tuned down. This is a useful way to accomplish it.
DOC% and WOC%. These sets of buttons are used to enter the Depth of Cut as a percentage of the bit diameter. There is a Course and Fine button for each, with increments of 10% and 1% respectively. FCD or Full Cut Depth can be entered and the number of passes required at the current DOC is displayed.
CNC Explorer Readouts and Calculations.
This is the heart of the CNC Explorer where all the results of the control settings are calculated and displayed. The Readout section will display a number of calculated results and offer some warning indicators when limits are reached.
Surface Feet per Min. (SFM)
This is a calculation based on the spindle RPM and the diameter of the cutting tool used.
Surface Speed (SFM) = BitDiameter(in) * π/12 or 0.2618 * RPM
SFM is important and refers to cutting speeds recommended for the type of material being cut. Each material has an optimum SFM speed to mill with. Most of the hobbyist CNC websites generally suggest a certain RPM for different materials. CNC Explorer does not have a control to set SFM directly but rather it is calculated as a function of RPM and bit selection using the above formula and displays SFM as RPM is adjusted.
MMR (Material Removal Rate cubic in. per min.
MMR is the rate the router bit is removing material cutting. It is dependent on how deep the bit is cutting and how wide the cut is and finally how fast is the bit moving
Material Removal Rate Cubic in./min = DOC * WOC * Feed Rate (ipm)
This is an estimation of the HP required from the spindle motor to cut. The higher the MMR the more HP is required. It may be that a cut you want to make exceeds the capability of your equipment so it is a good thing to monitor.
HP( Motor) = MRR * Unit Power * Efficiency
A couple of notes. The first efficiency will vary from manufacture to manufacture. CNC Explorer uses 80% as a conservative guess. Second Unit Power is related to the machineability of the type of material and can vary between 0.1 to over 1. CNC Explorer uses a baseline value of .5 for the calculation. However, on the far top right there is a box to enter a better value if you know what it is.
Spindle 1 or 2, KW Power
It is often more connivant to express HP in terms of KW for hobbyist machines. These readouts check the power against the limits your set for your equipment. Depending on which router configuration selected, if the power required exceeds 80% of the limit, the indicator with show a yellow warning indication your motor might run too hot if the cut is a long extended one. If the power exceeds the limits then the indicator will show RED and it is not a safe condition to operate under. Spindle power can be used as a gauge as to how much stress in being placed on the machine. the more HP required for a cut the more stress being applied to the router bit and CNC. Staying under 80% for most cuts is a good idea. Pushing cuts near the max is risky for breakage.
Motor KW = Motor HP * 0.746
DOC (Depth of a cut as a percentage of router bit diameter and Depth Type Indicator
A safe depth cut is always related to the diameter of the cutting bit. In CNC Explorer the cut depth is always programmed as a percentage of the chosen bit diameter. The DOC displays the actual depth for the selected bit and the percentage requested. Selecting a different diameter will automatically rescale the DOC value. This way you will always be setting the cut to the same percentage of the bit. The Depth Type indicator will show GREEN FINISH, YELLOW ROUGH, and RED PROFILE depending on the percentage being programmed.
1-20% FINISH CUT Generally safe to cut at high speeds assuming the WOC cut is also a FINISH TYPE cut
21-39% Rough Cut A more aggressive The general rule for a cut depth is to never exceed 50% of the diameter of a bit.
40-100% PROFILE CUT A very aggressive cut and you should never make such a cut without ramp cuts and monitoring very carefully.
It is often better to make more shallow cuts rather than trying to make a deep cut pass. It will take longer to machine the job but it will be safer. For production cutting, you can optimize the cuts for speed if needed.
WOC (Width of a cut as a percentage of the router bit diameter and WOC Type Indicator
The width of the cut again is always related to the diameter of the cutting bit and the readout will indicate in. but will be automatically scaled by the bit selection. WOC is often also referred to as STEPOVER or overlapping the cuts. The smaller the stepover the more finished the cut is generally to a point and depending on the geometry of the bit. A flat bottomed mill would not benefit from a small stepover but a ball nose would. The general rule of thumb for WOC is not to exceed 40% of the diameter. There is one type of cut where that rule must be broken and that is a slot cut where 100% of the bit is engaged cutting. The condition happens frequently whenever a part is being cut out with a profile cut. You will note the MMR and power requirements for this type of cut can be quite high and often requires making many shallow depth cuts at a slower feed speed. There is also a Type of Stepover indicator showing the following values:
5-20% FINISH Generally safe to cut at high speeds assuming the WOC cut is also a FINISH TYPE cut. Minimum cut is 5%
21-39% Rough Cut A more aggressive The general rule for a cut depth is to never exceed 40% of the diameter of a bit.
40-100% SLOT A very aggressive cut and you should caution and monitor very carefully.
40-100% SLOT A very aggressive cut and you should caution and monitor very carefully.
Feed Rate (ipm)
Feed Rate is the speed the Spindle is being feed into the material expressed as inches per minite.
Feed Rate (ipm) = PRM x number of cutting edges x Chip load.
So to cut faster and maintain the same Chip Load the Spindle RPM needs to be increased. To slow down the RPM needs to drop as well. Moving the RPM slider and or the Chip Thin Selector you the relationship is shown clearly.
Chip Thinning – An Advanced Feature of the CNC Explorer
Chip Load from earlier was the recommended amount of material being removed by each cutting edge per revolution of the router bit. But as it turns out for any WOC <50% the cutting edges are not fully engaged in the material. this causes the cutting edges to take shallower and shallower passes depending on the WOC. On very shallow WOC cuts this can be fairly drastic with only tiny shavings being cut that can clog up the cutter causing excessive heat, burning of the material, and tool damage. The solution is to use a higher feed rate to load up the cutting bits compensating for the thinning effect. CNC Explorer calculates the correction and you chose whether to apply.
Plunge Rate (ipm)
This is the last indicator in this section and it displays a suggested plunge rate in (pm). This the rate you would program into your G-code file that controls the rate the bit is moved downwards into the material. CNC Explorer will recommend the plunge rate to be the cutting Feed Rate/number of Flutes or cutting edges of the bit selected and the calculated Feed Rate.
CNC Explorer Summary Report
To the far right of the tool is a section that reports all the results and settings in one location. There is a box to enter a name of the cut. A copy of the sheet can be made and saved to record the settings.
And bonus an handy inch to mm and back converters are in this sections as well.
Advantages of Using the CNC Explorer
A lot of research and development went into the CNC Explorer. The goal was to present in one view the many parameters that go into configuring a CNC cut. The target is more for the Hobbyist Level machine that lacks the raw power of a big commercial system. The use of the tool hopefully will impart some knowledge of the Speed Feed calculations and safety margins. I am hopeful over time if the tool is accepted more advanced features can be added. I will be releasing a Video covering this material so look for a link. Better yet purchase the tool or subscribe and you will be notified by email when I do.
I just get and empty spreadsheet in XL10
George, I just sent you a new copy.