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.