Cutting bit keeps overheating

I’m new to X-Carving and have only been working with it for about a month but all I seem to have made so far is smoke - I seem really good at that!
I’m using Fusion360 and Zapmaker Grbl Controller. I’m using a 1/8" flat end mill bit from Inventables and cutting out a 430mm shape (a sort of star shape with cutouts) in either 6mm plywood or 6mm mdf (the final project will be acetate but practising on cheap materials first).
I always do a step cut of 1mm and I’ve tried slow and fast passes but it always ends up the same, i.e. about 50% through the cutting the bit starts overheating and then smoke appears which is the time for the panic button and another failed project. I’ve seen some fantastic stuff cut on the x-carve so I conclude it’s got to be the operator (me!).
At a bit of a loss what to do now as I can’t seem to make any progress.
Any advice would be greatly appreciated.

Thanks in advance.

As far as I can think of, decrease your depth, increase Feed rate speed. You may see couple more turn to finish the job, but your bit will be okay. I wish you put depth and feed rate information. We can determine easier.

Before we can suggest starting feeds and speeds, we need to know more about what you are using. What spindle are you using? What feed/speed? Is the bit the 2-straight flute bit, or is it upcut/downcut?

For instance, when I had the basic spindle (discontinued) and used the 1/8" 2-straight flute flat end mill bit, I would have to cut MDF shallow and quick (.024" at 64 IPM), while using the 1/8" 2-flute upcut ball end mill I would have to cut MDF deep and slow (.062" at 36 IPM)

Even if we come up with a suggested feed/speed for you, it would be in your best interest to find the best feed/speed for yourself. It will vary slightly for every machine, and you will need to find what works best for each bit in each different material. I use a modified version of this procedure suggested at Precise Bits (

As @RobertA_Rieke says, we need a little more info.

One possibility is the cutter is clogging up with the sawdust which means instead of cutting, the bit is rubbing itself to death. When you withdraw the bit, are the flutes clogged up or are they clear?

Try another bit. Milling bits have a finite life and will become blunt quite quickly on some materials. The small end mills are basically disposable for DIY folk these days, buy them on eBay in packs of 10 and chuck 'em when they’re blunt.

One of the woodworkers commandments is “Thy tools must always be sharp” - this is doubly true for small DIY machines.

Another possible issue, that I did myself, was having the spindle spin backwards. I am using a 220 volt spindle with a VFD and if that is your problem then just swap any of the 3 leads going to the spindle.

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


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
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?