OMIO CNC Tips, Tricks and Questions

Thought it might be worth putting this thread together to keep the OMIO CNC Router discussion in one places as well as allow individuals and team to share what they have learnt.

I have had my machine for a bit over a year and have cut a lot of aluminium parts on it with varying strategies.

Originally when I got the machine I was using 1/8” single flute endmills, with just a shop vac for chip clearing this didn’t work very well and I was limited to about 35IPM and 0.5-1mm DOC, the small endmills where great for boring small holes but terrible at slotting.

Later I was given some 4mm single flute endmills the experience, I was able to bore and slot much faster. I also later added one of the cheapo gold misters, this worked well for the air blast but didn’t mist well. I was cutting at about 60IPM and 1mm DOC.

I then started experimenting with larger 6mm single flute huhao endmills, but the shape of these meant that they gave more plunge and boring performance but where decent slotting. I also used some of the Grasshopper endmill giveaway 5 flute ¼” bits to do slotting in thick mild steel. Running these at between 5000-8000rpm(the minimium where the spindle still has torque) I was able to cut the 10mm thick mild steel at about 60IPM with 0.5mm DOC. Once I got the feeds and speeds dialed in it seemed to work very well and I could probably do 60IPM at 1mm DOC in mild steel with this machine.

After this I started sourcing and trialing a lot of different types of 4 and 6mm Endmills before settling on the ones I currently sell.

In regards to the current setup of my machine and tips/tricks I will split it into sections.


Use supplier bolts and tnuts to bolt a 20mm thick MDF spoil board onto the bed, planning to change to a recycled HDPE bed but even with a lot of coolant the MDF lasts ok and you can just use a hand rasp to smooth it. I use screws to attach my aluminium to the MDF and often put screws in the parts as well after boring with the 4mm endmill to remove the need for doing tabs.

Current machining strategies/recipies

At the moment for parts, I use a 4mm Single Flute to bore holes, this works really well and is very fast. This way you can make any size hole without the need to using multiple drill bits or changing tools. For slotting and pocketing I also just use the 4mm Endmill unless I am making a lot of parts in which case I do all the bores first and then change to a 6mm but usually a 4mm suffices. Changing the tool isn’t usually worth the hassle or time when a 4mm can cut very fast as it is. 6mm does seem to give a better finish but usually the parts are pretty much mirror finish anyway. I have a good mist cooler, a BPV-3000, I highly recommend this. It is much better than the one that uses pneumatic flow restrictors for both air and oil, really easy to control. I bought I bunch of these and was planning to sell them but never got round to it, might do so soon or even give them away for close to cost price. I use a small, cheap 750w silent compressor to run this and even with the max air setting this compressor is capable of keeping up while being really quiet which is nice. I use a soluble coolant, need to check the name. I have found that if you use the recommended dilution of 10:1 it doesn’t work as well as doing 5:1. Having the coolant rich is good, and really really helps with the finish. Using a load of coolant means that pretty much every surface is beautiful and reflective. I use a shop vac to clear up excess coolant from the material and spoilboard after which reduces swelling.

Spindle water pump/cooling

I used the use the included water pump, the bucket wasn’t covered the swarf broke the pump. Bought another, the hose kind of all kinked and broke after a lot of use. I stopped using the water pump, but left water in the system. Have used the machine a lot with no pump, works fine. If your not cutting for a long time without a break don’t worry about it. If you cut fast enough your part will be finished by the time it gets hot. I recently made an all in one unit which bolts to the top of the gantry, with PC water cooling parts. Couldn’t get the pump to cycle properly, going to get a more powerful on and try that.


CNC’ed polycarb on a larger router to go round the sides and back. 3D printed square nuts for the sides and then pressed M5 nylock nuts into them this works well. For the back I designing a special 3D printed sliding thing which goes into the table t slot to hold the rear panel and allow it to be removed easily to put longer stock into it. Will modify the CAD of the enclosure polycarb and stick it here soon, need to make it small enough to me made on an OMIO. This enclosure keeps most of the aluminium in, but stuff still comes out the front so need to add another cover that is easily removable. If your running fast with a 6mm endmill though, a lot of chips will still go out the sides of back. 4mm chips are kept in just fine.


I use fusion360 CAM, works well. I use the CNCROUTERPARTS-MACH3MILL post processor, use this one it works well and doesn’t crash the tool into the bed.

A tip for teams new to use ER collets, your supposed to put the collet into the collet nut first, then put the tool in and then put it into the spindle taper.

Would love for other teams to share what they have done with their machines and get a discussion going.

Will put some videos together showing the whole workflow from step file, CAM, cutting in Mach3 in a few weeks.


Thanks for the information and starting this thread. Can you and others post their feeds and speeds here with comment.

It would be nice to have more detail, such as feed rate, spindle rpm, endmill (brand, flutes, diameter and stickout), coolant, depth of cut, step over and operation type (this might be mainly 2d coutours).

This information may exist in other places, but it would be nice to have a central location with discussion on best practice.


Just use single flute tools for everything, you can get away with 2-3 flute tools if your using large 1/4" tools but you will have to slow down your spindle and then you won’t have the torque to cut fast.

My current feed rates are the following:

For the 4mm Single Flute Ozzy Endmills(this should be the same for the WCP’s probably which are different but similiar quality). For small tools keep the spindle speed at max rpm always. Slotting with mist coolant, be usually 1.6mm/0.060" doc and 80-100IPM, could be more but this works well and is reliable. Pocketing/Clearing full doc in 1/4 or even 3/8" 1.6mm/0.060" stepover at 80-100IPM.

For the 6mm Single Flute Ozzy Endmill, again you can use these speeds for similiar 1/4" tools etc from other suppliers. 20-24krpm and 100-120IPM, 1/8" DOC. I usually tweak the feed and speeds in Mach3 as well. Pocketing, full DOC and 0.1" stepover at 120IPM.

I seem to get a very good finish with zero welding or burrs with these speeds in combination with lots of mist.

Here are a couple of videos as a reference, feeds and speeds in the description. - could be plunging much faster

4mm Huhao, on an X6 which is a bit more rigid than a X8

Hope that helps.


We’ve mostly been running basically one part at a time— I’ve seen a few strategies for doing multiple/nested parts in F360 but didn’t find anything that really seemed great— what are people doing for this?

I end up making an assembly file in SW instead and import that.

1 Like

What I’ve been doing is probably (hopefully?) not the best way, but I do it in Fusion after importing my STEP files. Basically I joint together all of the unique parts such that they sit in the same plane. Then I delete those joints and move the parts around to allow a bit fitting in between but such that there isn’t too much wasted stock. If I have to make a bunch of the same parts (like last year’s elevator gussets for us) I lay the parts out in a tileable way and then copy paste a bunch of the parts together. If fitting into the remaining stock on the sheet is tough, I keep measuring the distances between the parts that are farthest from each other and make sure they’d fit.

If that doesn’t make sense I can clarify further.

I hope there’s a better way to do this but after a while I got really fast, so time wise it wasn’t terrible even if it was super tedious.

Thanks for this post

If you get a chance to get the name and source of the 750 W silent compressor we would appreciate it. We have mostly run ours with just a vaccuum which really limits the IPM - similar to your wxperience.

Having bought and used several 750w compressors from different brands within China and Australia I can tell you this. They are pretty much all the same, all the ones on the market in Australia or the US no matter how they are branded are all just white label Chinese compressors.

Something to think about is some of the smaller silent compressors don’t have a regulator which can cause problems if your wanting to use them for pneumatic tools, but makes no difference for a mist cooling system.

Mine is just a generic cheap ebay model which was about $100 works fine and is really quiet in comparison with the large direct drive compressor I was using previously.

As long as it has the all in one round compressor + motor thing and has good rubber shock mounts between the motor and the tank body it will be nice and quiet no matter the brand.

Something like this is what you want:

Would definitely recommend a small silent/oil-less compressor from any brand for running a mist coolant system or for running pneumatic tools in your shop.

Is it possible to wire in additional E-stops? I’m currently working on an enclosure design for the X8 (hoping/praying that gets approved soon :crossed_fingers:), and would like to be able to mount some E-stops around the machine. This would prevent us from needing to reach for the control box should (when) we need to stop the machine, as the control box will likely be mounted below the router.

Also, what size are the T-Slots in the bed?

My team’s looking at getting one. Is there anything that doesn’t come in the box that we’ll absolutely need? (other than endmills and material) Is there anything that we don’t necessarily need but might as well pick up?

I’ll probably be ordering one soon too. This is what I’ve got on my list currently:

The precision vises will be for doing 2x1" box tubing, and the dial indicator for tramming in said vises, along with any other stock or clamps we need squared with the machine.

I’d love to hear others thoughts on accessories for the OMIO. Any issues with the ones above? What else am I missing?


Ours just came in today (despite getting stuck in Hong Kong last week) and our order is really close to what you got. We also ordered the OzzyBoards TubeMagic, though (not sure if that arrived, yet). And I didn’t ask for a mister but that is something I’d guess we’ll need so I’d love to hear opinions on it.

It’s probably going to be a couple of weeks before we can try to set it up, but I am pretty excited.

Other than MDF and t-nuts to bolt it down, you’ll want a large diameter router bit to resurface the spoil board. They even sell purpose bits for resurfacing on Amazon or AliExpress.

Also don’t forget a 5 gallon bucket with lid for your water pump.


Just added that to the list, thanks!

Also for anyone interested, I managed to modify a model of a 6040 router to something that I believe is close enough to represent the X8 (for planning purposes at least). I’m slowly working on a design for an enclosure, but figured I’d leave this here incase someone else is looking for a CAD model.


What characteristics make the omio cut exponentially better than other routers at that price point?

1 Like

Have a look at the product page for some pictures to help. To start, the OMIO X8-2200L (really all their models) have an extremely robust construction. Heavy plate aluminum really adds to the rigidity of the machine. On other similar price point machines, the construction is often much less “beefy”. If you’re trying to make accurate cuts in a relatively hard material such as aluminum, the last thing you need is the frame of your router twisting and moving on you as it cuts.

The 2200L also uses HG20 linear guide rails vs the much more common hardened steel rod/bearing or extrusion/bearing setup on other machines. Again helping increase the accuracy/rigidity of the machine.

The drive system on these machines also use ball screws. These help reduce backlash in the system, increasing the machines repeatably. Moving over to the spindle, the X8 comes equipped with a 2200W, water cooled spindle. This helps keep the spindle cool when making heavier cuts.

Overall, the OMIO is a very robust machine that uses higher quality parts than other options in it’s price range.

This is my view on what makes the OMIO such a great option. I’d love to hear others reasoning too. Never hurts to have a little extra ammunition to throw at the powers that be when working on getting approval for one of these. :grin:

1 Like

Is the extra rigidity the ‘edge’ on allowing the omnio to cut aluminum so quickly? If not, what other factors affect cutting speeds. My school currently has a CNC Shark HD4 that is terrible at cutting aluminum. Are there any accessories that work well with the omio, like a laser zero finder, touch plate to find the tool, or any other accessories that make operation quicker?

The E-Stop should just be a regular switch. You could wire a few more in series


I’m no expert, but shouldn’t the switches be wired in parallel? If they’re wired in series they all need to be pressed for the signal to get through. If they’re in parallel then any of them being pressed will let the signal through.

1 Like

Umm. I’m not a wiring expert either, but I’m pretty sure that it’s the opposite of what you said. :grimacing: