I am trying to machine the coaster project.
I am using 2 tools, a 1/8" and a 1/4". The 1/8" is a generic from amazon and the 1/4" came with the machine.
Which values could you please recommend me for:
- Depth per pass
- Plunge rate
- Feed rate
What material are you making the coaster out of?
For the 1/8" tool, how many flutes?
Like Will said, the material you will be cutting as well as the different specs of the tool such as flutes, cutting length, overall length, etc. all matter. Also, what kind of toolpath will you be wanting to do? are you trying to do a pocket or profile cut for example? Because that would effect WOC and DOC when determining F&S. The e-book Will posted is an awesome resource for sure and will make determining good starting values pretty straight forward. With that said, I would be happy to post what I use F&S wise on my machine (Shapeoko 4 XL) if you give that additional info above. You can then use those as a starting point but remember YMMV.
I am using some sort of hardwood. Its thickness is 0.75"
The 1/8" tools has 2 flutes. Description:
HOZLY 3.175x22mm UP &Down Cut Two Flutes Spiral Carbide Mill Tool Cutters for CNC Router Compression Wood Bits Pack of 5
I read from that information that you will probably want to do profile cuts 0.75" deep (all the way through?) with that 1/8" endmill ?
While the 22mm length of cut would allow it, slotting 0.75" with a 1/8th endmill in hardwood could turn out to be a big challenge. Even more so because you reference a compression bit, which has poorer chip evacuation than a regular upcut endmill
That said, here’s a summary of how I would approach the feeds and speeds, as mentioned in the ebook:
- pick a RPM value, the highest you can bear (with respect to loudness). When using a trim router my goto value as a balance between noise and efficiency is 18.000RPM
- select a target chipload. The ebook has a guideline table, but basically 0.001" is the answer in most cases, at least for a safe starting point
- feedrate is then derived from RPM, chipload and number of flutes, like so:
Feedrate (in ipm) = chipload (in inches) x RPM x number_of_flutes
so that would be 0.001 x 18000 x 2 = 36ipm in this example.
- plunge rate in hardwood: 30% of the feedrate should be fine in most cases
- depth of per pass: stick to 50% of the cutter diameter or lower. In hardwood, and considering the fact you will likely be slotting, I would say stick to 1mm or less with a 1/8", and 2mm or less with the 1/4"
As you experiment, you will be able to increase feedrate/chipload, and possibly depth per pass. The machine will tell you when you are entering the danger zone (shrieking sound/chatter)
Julien, thank you very much for your response!
I have not used a compression bit like that in any hardwood so I unfortunately do not have F&S to give you as a starting point. Julien is spot on with his summary on how to approach it. I would be extra careful with the depth per pass to avoid breaking the bit or producing too much heat.
This topic was automatically closed after 30 days. New replies are no longer allowed.