Hey all, I have a bunch of large catchalls trays to carve. 16 x 20 x 2 inches. It requires a lot of wood to be hogged out. CC says it will take over 6 hours to just rough out the trays with a 1/4 flat endmill with default settings.
I am asking the group on how you would attack removing all this material.
IE: Push the speeds, feeds, and stepover and what bit would you use?
First step would be to push your DOC - CC is very conservative, you can very likely go to .100 or even .125 (1/2 the width of the bit). Feedrate can likely be higher as well, in the 100IPM range. Try both on a piece of scrap.
Default values in CC with 50% stepover give a Material Removal Rate (MRR) of .3 cubic inches / minute.
With a DOC of .1 and a feedrate of 100, you 1.25, so over 4 times faster.
You could try doing the bulk of the cutting with the McFly and then switch to the 1/4" using Rest Machining and 1.0" as your previous tool. The more aggressive cutting with the 1/4" as suggested may be quicker, but depending on your material being cut, you could probably push the McFly a little harder as well.
I don’t think the cutting geometry of the McFly is suited to large-scale material removal — it doesn’t have much in the way of flutes to clear chips — the design seems optimized for surfacing.
I used it recently clearing a large area for a serving tray/cutting board and it saved time over the 1/4" (default settings), but the depth was only 0.09".
I see what you mean, where digging out 2" it wouldn’t be very efficient.
I bought a bowl and tray bit with the intention of doing something similar. I haven’t used it yet and read concerns online about their ability to really evacuate the chips as well.
So I thought maybe I will hog it out with something different and then use the bowl and tray bit for the final cleanup and to get the appropriate radius on the bottom.
Usual preface, I’m with PreciseBits so while I try to only post general information take everything I say with the understanding that I have a bias.
There are a few version of these. They are much more common in larger cutters. You’ll find them listed under “roughing”, “corncob”, and “chipbreaker”. Be careful with those last 2 though as they are also common terms for types of composite and metal cutters that are not intended for things as soft as wood. A quick rule of thumb would be that if it’s more than 3 flutes with those terms it’s probably meant for metal or composites. 2 and 3 flute ones you’ll need to check.
In general these run on the idea of breaking the flute engagement during the cut reducing total bit deflection (less time being pulled into the cut per flute). You can kind of think of it as each section of the flute being it’s own small cutter. That usually comes at the cost of cut quality and can cause weird effects with variable chipload. The exception to this was that chipbreakers were originally intended for a similar purpose but with the breaks in the flute being overlapped by another flute to give a smooth edge. However, it will depend on the manufacturer if that is true for any given bit. They were also usually designed for deeper cutting than you may be able to achieve.
In terms of overall ability to cut faster you’ll be deflection or power limited first.
So things like those cutters could help. However, you will probably get a lot more out of adding a flute as long as you have the feed to use it. e.g. like for like (RPM, tool geometry, etc) if you are cutting at 50IPM with a 2 flute you can cut 75IPM with the 3 flute with the chipload and hence forces and deflection being the same. There will be some other difference depending on cutting depth and helix as there's less time between flutes and you could engage more in a rotation.
You can also look at things like getting tooling with a higher helix (tighter flute twist). This will increase the force into the Z. Obviously you have to balance this so that you aren't overloading any given axis. Additionally, there's will be a limit before you start to chip out material.
The last one easy one, but hard to qualify is a higher rake (angle of attack of the flutes). The higher the rake is the less force it takes to cut the same chip. It comes at the cost of flute strength but in this size tooling you have a lot of wiggle room.
Hope that’s useful. Let me know if there’s something I can help with.
Hey All that is awesome information.
I will take that and do some more reading
@TDA thanks, Yes they seem to be more for bigger machines and yes I believe the idea is to break the chips up so we can get them out of the way faster. yes it leave a very rough cut but that the job of the finishing bit to fix
I saw a cheaper one on the interweb it was cheap enough to try one, I guess
I have found I can push an 8mm quite a bit harder through ply and hardwoods than a 1/4" before getting the “I’m going to snap” noise
I have a 2.2kW spindle however and am lucky enough to be able to run 1/2" cutters, for lots of wood removal I can’t do with the table saw or thicknesser, I use one of these as a cheap cutter for bulk removal
I run 3/4 to 1" mortising bits with 1/4 shank.
Operated about 13000rpm and feed rates between 700 and 1000 (in mm of course). Plunge rate of 200 to 250. Stepovers are 40% of the bit. I shave off over 75% of the time on average.
I suggest a mortising bit because they allow for great chip extraction and also allow the bit to plunge without jamming up the machine.
That is interesting but makes sense. I thought they might be to big but then I use them all the time in my hand held routers.
I have to think more on this as my bits I have to ramp in. there is no cutter in the middle of the bit. and then there is the chip removal. maybe a bowl bit, I will have to look in my collection Well I guess I will have to try some things
Thanks, you got me thinking
Go buy yourself the cheapest mortising bit you can find. I get them from a local place here in town for $4.99. They are inexpensive and last a long time.
Just slow down the plunge rate if you like. Mortising bits have cutters on the outer edges and nothing in the middle so you don’t really need to worry about ramping them in.
You can also get a cheap bottom finishing bit and use the to hog out material if you can’t control your plunge rate. Remember that these larger sized bits run better at lower RPM. I run the 1/4 inch bits between 18 and 19000 but these larger bits I run around 13000 to 15000.
So I thought I would ask the experts here