Feed, speed, deflection and machine power spread sheet

There are a number of spreadsheets available that calculate the chip-loads and surface speeds, as well as estimating the cutting forces and bit deflection, but I made this one with all the data entry in metric. Although the data entry is metric, all the calculations are presented as both metric and imperial to make matching to a tool data sheet simpler.

There are two spreadsheets, one for VFD-based spindles and brushless routers, and a second spread sheet for brushed routers (such as the Router11). Spindles and brushed routers have a very different speed-torque-power profile to brushed units, so it is important to use the right sheet. I have put some example calculations in and based the feed-rates on what hopefully is viable for something like a LEAD machine. For the spindle spreadsheet, I based the values on a typical 1500W 24k rpm spindle, and for the 'brushed' spreadsheet, a best-guess at the Router11. My machines have very different mechanics and spindles, so if anyone finds better 'tuned' parameters for actual OpenBuilds machines, it would be great to know

With the spreadsheets, the first 14 rows are the most important for configuring the characteristics of the bit, the cut and the material. There is much good information on chip-loads and surface speeds for different materials from tool suppliers. Suggested feeds and speeds such as in in the OpenBuilds SharkBit data base can be entered in and then chip loadings and surface speeds calculated, or rpm and feeds can be adjusted by hand in order to match chip-loads and surface speeds as seen in tool information from suppliers such as as Amana tools and Harvey Tools etc.

The problem with most tool information databases is that they are often created by the manufacturer for a group of similar tools, rather than a specific bit. The tool data sheets often specify a chip-load based on cutting at a depth of one tool diameter. If a 3mm diameter tool had a flute length of 6mm, then cutting in most materials to 3mm deep or more will be quite straight forward. If the 3mm tool had a flute length of 25mm and therefore a bare minimum of 25mm stick-out, then a 3mm depth of cut for slotting in oak is likely to put a fair bend in the bit! The spreadsheets therefore estimate the deflection the bit may experience for a given tool stick-out length, hopefully reducing the number of broken bits.

For configuring a new tool or material, the process is generally to first enter the diameter, number of flutes and intended cut-width of the tool, then set the rpm of the spindle/router to give a sensible surface speed (e.g. as in Surface Feet per Minute). The feed rate can then be adjusted to give a useful chip-load. Lines 6 and 14 of the spreadsheet for the tool stick-out, and the material K factor can then be entered (and guessed-at in the case of the K factor), and when a Depth of Cut is set in line 11, then the machine power loading and deflection calculations can be checked to see if it is likely that either the tool will be bent too much, or that the spindle/router risks stalling. The deflection and power are very dependent on the estimate of the material K factor, so the deflection and power are for 'indication' mostly, however still very useful!
The chip-loads are calculated based on the actual width of cut as well as for slotting operations, so the machine loadings for High Speed Milling with shallow width but large depth of cut can also be estimated.

Evan

 

Thanks Peter, will do.

 

feed/ flutes/ rpm is mathematically the same as feed/ (rpm x flutes), so there is a chance that either will be used. Chip load will vary as stepover gets small as chip thinning effects need to be taken into account, and the spread sheet has a commonly used formula in for that (the line under the basic chip-load value shows the thinned chipload for low step-overs). The depth of cut is a bit more tricky and it depends on the exact cutter shaping as to how chip load may change, but generally reducing the chipload by 30% for cutting 2xdiameter deep, and by 50% for 3x diameter deep is a good starting point (often best to do the reduction by keeping rpm the same and reducing the feed-rate). The depth of cut has most impact in practice on the force experienced by the end of the cutter, and therefore whether the cutter will bend or even break if going too deep, rather than overheating due to the wrong chipload. The spreadsheet estimates the tool deflection, and the depth of cut and stick-out are primary factors that change that.