If you’re preforming a 2D Profile/Contour cut (to cut out a part), how would you factor in stepover? Since the cutting path is just the size of the bit, would the stepover be zero (or very small)? What’s the best way to factor that in for Feeds and Speeds?
Stepover is irrelevant for a contour cut since there is a single pass per depth.
But indeed slotting is hard and may require to adjust feeds and speeds compared to e.g. pocketing at 50% stepover. You could dial down feedrate a notch, but you need to keep chipload above a certain value, so I when slotting I choose to reduce depth per pass instead, and then I can actually increase feedrate (and RPM) to compensate for the lost time of cutting shallower.
For example, with a 1/4" I would typically slot at 2mm depth max, and it will be fine
2 Likes
slotting is… pretty harsh and does not have the concept of a stepover
but one could do a small outside offset shape at 1.5x endmill diameter and then do a pocket… and then you have a lot less force on the bit and will have the concept of a stepover
2 Likes
Definitely some good tips already. There are some rules of thumb but generally just start really conservative.
Material type matters, slot depth matters, flute count matters. Basically your number one concern will be clearing chips. The deeper you go, the more its important.
In aluminum this means that single flutes are king, especially with dry cutting. In wood (although i haven’t cut nearly as much as some) single flute compressions really did well.
I try and go with the extra dimension… set an outside contour slightly larger than the bit diameter and pocket that down to where I would set my tab height. Then do the profile cut with tabs…
It seems to me that if I try “slotting” my profile, when bits and pieces of stringy fiber go through the bit the side surface of the profile will have “dents” from the extra material deflecting the bit slightly.
When adjusting for Feeds and Speeds, how would you say that the WOC correlates to the DOC? Within the @gmack SFPF Workbook, adjusting the WOC value affects the IPM, but adjusting the DOC value does not.
That’s because this adjustment relates to chip thinning, which only depends on WOC , so when targetting a specific chipload, calculators bump up the feedrate based on WOC value when using WOC lower than 50%, to bring the effective chip thickness back to the desired target.
The indirect correlation between WOC and DOC is the material removal rate (MRR), which depends on both, and is limited by the machine (machine rigidity & spindle power). Typically, on a Shapeoko you can cut a large DOC if you use a narrow WOC (e.g. in adaptive toolpaths), or cut shallow (DOC <100%D) with large stepover (e.g. slotting), but you will likely run into trouble if you run deep AND wide, the extreme example being slotting at >200%D DOC.
1 Like
Thanks for helping to clear that up. 
1 Like
This topic was automatically closed 30 days after the last reply. New replies are no longer allowed.