.25 End Mill Feeds and Speeds

Need a little help here. I’ve been doing a lot of profile cutouts in oak and maple with a .25 down cut end mill and I’m wondering what people are using so they don’t burn up their bits. If I had a bigger machine I’d set up at 18000 rpm and set my feed rate to 300 ipm and go. I don’t know what the onefinity and Makita are capable of but I know I can’t push 300 ipm out of either. I’ve tried slowing the Makita down below the 3.5 setting I generally use and taking more passes but I’m getting more dust than chips and slowly getting a discolored bit. What are others using? Should I profile cut with an 1/8" bit so my feed rate is closer to what it should be based on chip load.
For reference I’ve been experimenting in the .04-.06 depth of cut range/pass with a feed rate of 40-60 with the makita settings ranging from 2-3.5 and ramping all cuts 2 inches. Seems my ramps are generating more heat than the rest of the cut so going to go experiment with increasing my plunge rate right now.
Thanks in advance for any help.

I am using the same as my .125 endmil. 60ipm but going about .1 deep per cut, and it’s still noisy but does the job and the bit doesn’t heat up too much at 3.5 on the Makita.

I have been running my 46202-k at 18K rpm, 160-180ipm, .25" DOC, with stepovers around 0.1". Really just trying to stay as close to that .005" chip load as I can, but I think .003 to .004 is probably more ideal.

2 Likes

What kind of material are you cutting with those feeds and speeds?

Pine, cedar, oak, African Mahogany, hard maple, cherry, paduk. The last four probably need to be closer to .003 chip load, but I don’t feel a need to go below that.

1 Like

I would assume the endmills will dull over time, so how do you adjust chip load for the gradual dulling of the bit? I don’t have any inexperience in this but it seems logical that after a hundred hours of cutting, trying to maintain those feeds and speeds would lead to a bit breakage more easily. Definitely still trying to learn here! Thanks for all the insights!

With no CNC experience and 50 years of cabinetmaking under my belt, I can tell you that in hard/dense woods my bits go out for sharpening or get replaced after roughly 2 to 3 hours of the equivalent of continuous CNC use. A good sharp bit does so much better than one that has begun to dull. No burning, no tearing, no chatter, clean profiles, etc.

This doesn’t address the feed/speed question directly, but it might indicate that you can be a “bit” more aggressive with fresh tooling. (Sorry - couldn’t help myself)

I use Whiteside bits. I am starting the CNC journey with them and will pick up some of the Spektra coated Amanas along the way as experience and confidence build. Because they are coated, it does not appear that they are designed to be sharpened. It will be interesting to see if they stay sharp so much longer that they match a good uncoated bit over several sharpenings.

1 Like

Hi Jim,
Where do you get bits sharpened?

1 Like

I did some tests with cherry yesterday afternoon. I’ve been ramping 2” with a 1/4” end mill at .04 depth of cut, feed rate 60 ipm and getting burning in the ramps whether profile cutting or pocketing(Cherry). Ramps are associated with plunge rate not feed speed. So I figured since I’m only plunging less than 1/16” per pass, I could speed my plunge rate up and my ramp distance down. When I set my ramp to 1” and adjusted my plunge rate from 50% to 80% of my feed rate no more burns and after hogging out a 1/2 deep pocket in cherry the bit was not hot. Pretty darn warm but not hot.

I follow the feeds, speeds, and DOC charts available from Whiteside and Amana. So far so good.

Hi Ron,

Forrest Blades.

https://www.forrestblades.com/forrest-factory-carbide-saw-blade-sharpening/

Way down at the bottom of the list is router bits.

Jim

1 Like

Ahhh. Cherry. Its composition is such that it burns more easily than most woods. Your cutter must be sharp sharp sharp, and you want to move that cutter along quickly enough that friction does not build up. That should apply to plunge rate and feed speed. Again, no CNC experience here, but I notice you’re faring better with conservative depths of cut, and increased plunge rate and IPM. Perhaps the router spinning fast enough to give a smooth cut but no more than that - again, to reduce friction. FWIW, on a general note, I avoid climb cuts in cherry - that is an invitation to burning.

1 Like

You will notice when ramping your Feed Rate slows down due to the bit going down as it moves forward. The same goes for TAB cuts. Once it reaches the depth of the cut the speed will go back to normal. You are right on with your solutions. For 3D carves, I generally set the Plunge Rate = Feed Rate but I am cutting fairly shallow generally. For slot cuts it probably is a very good idea to plunge “Ramp” slower but as you are finding out there is a balance to be found. Thanks for the information something else to consider in the Art and Science of Feeds and Speeds.

I have a few of their table saw blades. Never had to page down that far :slight_smile: Thanks Jim

I have a friend who runs a production CNC shop and had him over this weekend explaining feeds and speeds. He explained it like this. If the wood is burning or chipping your rpms are too slow. If your bits are burning then the speeds are too high. The more rpm you can achieve without burning the bits up the faster you can move feed and plunge rates. This is all factored by the hp of the router or spindle and will be the determining factor on how far these can be pushed. Because we are using a router these speeds are limited by the router itself. The bits are designed to go this fast with reasonable ware compared to the amount of production done. So its a speed of production and how much you get out of a bit before it needs to be replaced vs how many projects you can produce is what they look at in a full production shop.

1 Like