Ball nose VS two-flute

[lex]

I am finishing up a cut in MDF that includes about 300 smallish pockets with a 1/4" ballnose. (The coated one from Beckwith) It is basically taking two full 12 hour days to complete. I like the small radius at the bottom that the ballnose provides. However, time-wise it is pretty crazy. Would there be a large difference if I used a two flute?
Currently the pockets are taking three passes each and are either .5 or .3125 deep. The majority are .5 while the larger ones are .3125.

I could use different cutter sizes but some of the pockets cannot have larger than the 1/4" tool. That said at what point does if make sense to use a different tool considering the time it takes to change bits and re-zero? Not to mention making separate tool paths...

[garyb]

Would there be a large difference if I used a two flute
the BDP003 1/4 BN is a 2 flute tool. You need to look at your stepdown, stepover and your feed rates

you can take that tool to .5 stepdown just reduce the chipload by 25%
Gary

[lex]

I don't think I am ready to run 1 full .5 deep cut. Call me timid but I really hate the screeching sound when I cut too deep. (For my ears that is.) The attached is a similar drawer for my Vidmar style cabinet. http://www.talkshopbot.com/forum/attachment.php?attachmentid=26617&stc=1

[garyb]

If your getting screeching then your feeds and speeds are incorrect.
second thing for the above I would change to an endmill with corner radius (if you must have a radius on the outer edge)
toolpath with stepdown to .5 in one pass as a spiral ramp. (for 1/4 tool, holes under 1/2 dia profile spiral ramp inside vector, over 1/2 area clr spiral ramp)
Thats fine if you wish to remain timid in toolpathing but don't expect to reduce cut times down until you learn more efficient toolpathing and how to take the tool out to its working limits
Gary

[RossMosh]

First let's start with the obvious: Not all machines are equal. There are several different models and generations of machines which will make a difference in how you can cut. Also you have to take into consideration whether you're using a spindle or router.

That said, with a 1/4" bit you should definitely do the .3125" in 1 pass. The .5" you probably can and should, but that's up to you. One of the biggest lies with CNC routers is that you shouldn't cut deeper than the width of your bit. It's a complete lie. It may be a decent place to start but that's about it.

The next thing to talk about is understanding how cutting work. Let's say you want to make a .5" pass into MDF. Being conservative with a 1/4" bit the chipload calc spits out the following info. Now the calculation below is just a guideline. But the theory remains the same. If you want to cut slower than 108ipm, you'll likely want to slow down your router or use a single flute tool (which is less likely but still an option).

Feed Rate = .006 x 12,000rpm x 2 Flutes x .75
Feed Rate = 108 inches per minute

I can tell you after working with a few different machines, I prefer to go deeper, start conservative with the cutting settings, and then tweak from there. Not knowing anything about your equipment, I'd go full depth passes at 60ipm/1ips and 12000rpm, monitor things, and then increase the feeds as the job ran to see how things went. My gut says around 90-100ipm will be your sweet spot but you may find 120-150ipm works great for you.

[mrgadget]

If I might quickly ask, what is the material you're cutting for the tool shadowing in the above picture? I'm interested because I need to do the same to my toolbox. Certainly hope I'm not hijacking your thread, but enquiring minds want to know! Now, back to your regular scheduled programming.

Jay