What's slowing down our milling speeds?

My team got an Omio X8 router at the beginning of this season, and we are slowly trying to be more efficient at using it. Please bear with me here, as I am definitely new to manufacturing and such (this is the first CNC machine my team has successfully used).

When we first got the router, people in the CNC router thread here said they were able to cut at ~40ipm at ~.05" DOC with a 4mm Huhao endmill (if I recall correctly). When we tried to step up our feed rates to get to this number, we were not able to get anywhere close with our setup before bits started breaking. During the season, most of our parts were cut by a 6mm Huhao endmill at 0.0625" DOC at ~25ipm. When we tried to push it any faster, our bits would start breaking again.

Just recently, I saw the post below:

Our setup is not dramatically different from what is shown here, but there are a few potential differences. First, our coolant setup is just the operator spraying some water-soluble coolant from McMaster with a spray bottle (no auto misting setup for us yet). Second, our router is not very well secured to anything – it sits on a table and it’s not bolted down.

What differences could lead to such dramatic differences in cutting speeds between the OzzyBoards video (and the recommendations from before the season) and what we’ve done in the past?

Could you elaborate a little on how the bits were breaking? Were you finding the flute packed with aluminum?

A coolant mister does two things: the coolant cools and lubricates the part and tool, and the air blast helps remove the chips from the cut. Of the two clearing chips is the more critical function, as recutting chips is really bad for tool life. You can easily get plenty of coolant into the cut with a spray bottle, but you won’ t be clearing chips as well as a steady stream of pressurized air.


Proper coolant is incredibly important! Invest in a decent mister, or better yet, a FogBuster or similar.


If I recall correctly, early on, the bottom of the flute (the part that was cutting) would have aluminum welded to it when the bits broke. Our plan is to set up a proper airblasting and cooling setup over the summer.

The main reason I was asking this was because early on, when we manually blasted the cutting path with air while the machine was cutting (in addition to spraying coolant), we still had bits break and chips of aluminum instantly stick themselves to the stock around the material as it would cut (I believe this is what chip welding is?). This only stopped when we slowed our feed rates and DOC, and the air blasting didn’t seem to make a difference at that point.

What alloy are you cutting?

It’s all 6061-T6 aluminum.

What spindle speed are you running when you see this occur?

Yeah as @solomondg mentioned a decent mister will help dramatically. We put a fogbuster on ours and haven’t had any issues with chips welding. Prior to getting the fogbuster we’d have somebody squirt the tool coolant (from a safe distance) and keep the general area wet with coolant. We went through a ton of coolant doing that though.

Once the aluminum starts to gunk up the flutes bad things happen. We scrape out any material every time we stop the machine even with the mister.

I think our spoil board swells up quite a bit by the end of the season so that may be something to watch for over time. We usually don’t care and it doesn’t impact our work though.

Either have the person next to the machine spray more, or add a mister. You’re right that what you’re observing is chip welding.

Try decreasing your DOC and increasing your IPM. I find that .04 or .03 DOC is fine even up to 50IPM and higher.

Slightly off topic, but how does the MDF waste board react to coolant mist? Is it enough to make it swell or require skimming more often?

This is where we were at most of the season. .03DOC and 50-60ipm. And we were not using and misting or coolant.

Granted we did most of our cutting with a .25" or .125".

Heavy misting definitely swells the wasteboard. A lot of times you can safely ignore it, as the aluminum protects most of the MDF, and few parts need accurate depth anyway.


So unless you have a problem with your machine( ie bolts etc loose causing tool deflection and then breakage) the main problem your having is either that you are simply running too slowly which is causing rubbing and welding of the tool or that your sheet material is moving.

Using the 4mm Huhao you should be able to do about 50-60IPM with 0.04" DOC very happily with no mister, vacuuming up the chips as the tool goes around is a good idea as is something like WD40 or water soluble coolant. If you want to increase DOC you will definitely need a mister. I have found that the coolant concentration makes a big difference to both cutting rates and finish, you want a rich solution in your mister.

With the 6mm Huhao as with any 6mm single flute endmill you really want to be using a higher DOC, around 0.1" at least when slotting and far higher IPM. Sheet material can happily be cut in a single pass but you do need to have plenty of screws/clamps to hold your stock down in your machine. Running less DOC then this is basically causing all the load to be right on the tip of the tool causing it to get worn out prematurely. The 6mm Huhao also has a different tip/flute shape that causes it to get aluminium stuck directly on the top of the tool and more vulnerable to chip welding then proper aluminium cutting 6mm endmills, so you sort of need a mister in order to use it properly.

Cutting aluminium is sort of a paradox, within reason you need to push the tool faster( and harder) in order to get greater life. It is probably the case that your simply running far too slowly and you never got up to the sweet spot( for cutting dry) in your testing. The ability to change feedrates and spindle speed in the Mach3 Console is a very good feature that you can use to your advantage when wanting to push your cutting speeds to the max.

In regards to a mister damaging your waste board/spoil board, I run lots of air and coolant as it allows you to cut really fast especially with just 4mm tools( might do a video on this) this does decrease the spoil boards life substantially but I do things to improve the life. After a job I usually use a wet and dry vac to remove as much coolant as possible, I also use a Rasp Plane to simply and quickly remove any swollen areas or bumps. All the swollen spoil board really causes is a bit of Z inaccuracy, this doesn’t matter at all if you only do 2D or small 2.5D parts.

If you send me a PM I am happy to check over your feeds and speeds and help you get cutting faster.


The only impact we have is depth of cut. If I had to do something sensitive late in the season I would do a skim cut but the way it works out is that we naturally are just doing cut through parts by the time the swelling affects us.

But we also tend to go heavier on the coolant than we probably need.

1 Like

We run our 6mm endmills at 16000rpm (we used 1678’s tool database as an initial guide). When we’ve accidentally run them at higher speeds we got sounds we were uncomfortable with and more chip welding.

is there a specific reason people don’t use plastic spoil boards like polycarbonate, or HDPE? I feel like this would solve the warping problem, and it would be easier to clean.

I found that plastic spoil boards make it harder to screw down into, and the lumps left over after screws come out are more pronounced.

It sounds like OP isn’t able to hit this and doesn’t know why. Maybe you have some ideas about why a router might miss this mark?

We have moved to 5mm for pretty much everything now, and part of the reason was to be able to push harder than the 4mm bits would allow. I think your recommendations above were more aggressive than what we ran.

Note that Ozzy’s recommended DOC is a little smaller than the OP’s; this plays a big factor in chip welding in my experience. Vacuuming chips up can also help, although personally I’m a fan of spraying PG2000 or WD-40 often as the tool cuts as well.

This topic was automatically closed 365 days after the last reply. New replies are no longer allowed.