Cutting bit keeps overheating

I’m using a 1/8" Diameter End Mill Single Flute Spiral Upcut with these Fusion360 settings.

good catch @AngusMcleod

Which is the correct bit for profiling? End mill single flute, double flute etc.

Making better progress today with MDF. I took the advice of RobertA_Rieke and now cut faster and shallower - seems to be a lot better.
Thought I make my first cut into acrylic. Just a hexagon profile 2mm deep in 3mm thick acrylic. I set the speed to 600mm/min and the depth at 0.5mm/pass. All is OK for the first 1mm but then it starts to melt the walls of the cut as it gets deeper. I’m using a single flute 1/8" spiral upcut end mill.

On the acrylic cut, you must use slowest RPM, same again, shallow cut and fast feed rate. You have to pass cutting area before start heating.

How slow?
Thanks for the advice so far. Feeling more positive after some success this evening.

Take a look at this post. (warning: knowledge bomb ahead)

A really interesting article @Milbot - thanks.
I’ve carried out a little more research and it seems that the spindle speed of the Inventables spindle is not fast enough for most materials. I have been advised by a UK router cutter manufacturer that spindle speeds in excess of 18000rpm is required to cut acrylic with a 1/8" bit. Cutting MDF requires 24000 rpm and a feed speed of 2500mm/min.
Is this correct?

24,000 rpm for MDF is faster than my calculations show it should be. When I look at 98 inches per min feed rate with a .125 bit in MDF I get about 16,000 RPM or less depending on the number of flutes.

With a .125 bit in MDF you should try to get a chip load between .004 and ,007

Your Chip Load = feed rate in ipm) / (Spindle RPM X number of flutes)

That matches with some successful cuts I’ve made in MDF - a .125 bit at 12000rpm and a feed rate of 60 ipm with a single flute cutter. The cutting depth I’ve used is 0.5mm so not sure if I can go deeper than that per pass.
What I really want to cut is 6mm acrylic. I have seen a two flute Trend cutter (S66/10) which is supposed to be designed for the job but that’s supposed to run at 18000 rpm (so they say). What chip load should I be looking at for acrylic?

Chip load for Acrylic should be between.003 and.006, For an RPM of about 15,000

It’s taken me a while but your advice is spot on ! Even though I checked the other day and convinced myself it was correct, it actually wasn’t. Now I’ve swapped the wires the X-Carve has come alive!
Thanks. If I see you in the pub I’ll buy you a beer or three!

1 Like

Allen

may I ask, where are you getting the chip load targets you are referring to?
is there a guide somewhere, or is this stuff you just know?

trying to understand…

Here is a spreadsheet I put together using standard chip load values for common materials and tool sizes.

You can set the feed rate you want to use and it will show you what the speed setting on Dewalt would need to be for that feed rate. What you will find most of the time is that the Dewalt will not spin slowly enough for the feed rate you want to use. It may be that 120 ipm is the slowest feed rate that will work with a speed setting of 1. In those cases you need to just understand that the X-Carve is not capable of that feed rate in most materials so you will use the fastest feed rate you are comfortable with and a speed setting of 1 and just know that your chip load is not optimal.

Having an optimal chip size is more of a target to try to get close to not an absolute requirement, You can get very good cuts with non-optimal chip loads. It just may be giving up a little tool life in exchange. If you were running a production mill and you needed to get every hour possible out of your tools then you would want to be as close as possible to optimal chip loads, but for a hobbyist, ballpark close is OK. Especially since that is the best we can do in some circumstances due to the operating RPM range of the Dewalt.

CNC Speed Calculator for Dewalt.xls (38.5 KB)

I’m glad I asked;
I had found that same chip target source at http://www.pdsspindles.com/engineering-speeds
and was thinking of building a very similiar spreadhseet,
so you have saved me a great amoungt of work and I thank you.

One question I still have is that the chip rate target bottoms for tools at .125,
which is 1/8th of an inch.

I bought a 1/16th carbide tip fishtail which is .0625;
any advice on how to set up for a tool of that smaller size?

The chipload data from that source stopped at .125. For tiny tools like .0625 the real limit set by not wanting to break the tool. So I don’t worry about chip load for the tiny tools and just keep the speed at 30 to 40 ips and the DOC to no more than .03. The Dewalt speed can be a little higher but I would never take it over 3.

I don’t remember where I found it, but I’ve always shot for a target of .003-.005" in hardwood and .003-.010" in softwood. After doing feed and speed testing with each bit and wood, I also feel the bit to see if it’s warm. Usually, after 2-3 minutes it’ll be slightly warmer than when it started, which is good. If I burn my fingers, I know I need to either drop the RPM or increase my cut speed.

1 Like

Allen
I had some quality time in an airport
so I spun the spreadsheet and added a tab which calculates the optimal feed rate based on drop down inputs for:

  • DeWalt Speed
  • Number of flutes
  • Material type
  • Tool Diameter

The file is attached; the work I did is is the tab ‘Feed Rate Calcs’.
CNC Speed Calculator for Dewalt.xls (58.5 KB)

I note that the minimum feedrate I can see is around 65.
What do you think the max feederate of a properly tuned Carve is?
do we have any empirical evidence from existing users what federates they have been able to sustain?

The max possible feed rate depends on what is being cut and the DOC.

I have cut high density foam at 140 ipm with no problem, but I would never try to cut hardwood faster than 90 ipm (with a decent DOC) and that is more than I would normally do, I get the most reliable cuts in hardwood closer to 60 ipm. But that is just my machine.

What shows up immediately when you start looking at the chipload numbers is that the Dewalt min RPM setting is just to damn fast. Your spreadsheet demonstrates that really quickly,

If I tell it I am cutting hardwood at a speed setting of 1 with a quarter inch tool, it is recommending a feed rate of about 300 ipm. The X-Carve can’t even get near that. You really need a spindle that can run at about 8,000 rpm

Thank you kindly for the excellent article Milbot.
I had bought a new automated cnc, and I went through ore than a dozen end mills.
The solid carbide ones would overheat and become dull after a few sheets of materials, and the carbide tipped ones would break.
I kept slowing the feed down, and increasing the spindle speed, but nothing helped.
After reading your article, I realized that I was doing thinks backwards. Using your formula, I slowed my spindle down, and doubled the feed rate.
Now, I am making very nice cuts, and the end mill is not getting hot anymore.

Thanks gain,
Jalal