Hello,
Slight issue with our Omio CNC X8-2200
Were using Solidworks and HSMWorks to post process our code and using Mach3 to upload with a 4mm’ single flute endmill. We were Machining our Belly Pan for onseason in two half’s. The first half the bore came out big about 10-15 thou too big. When cutting the second half the bore came out on size with a 3 thou tolerance. Same code, same endmill. We’re unknown off the issue that’s causing this and wondering if anyone had any similar problems. We also calibrated the endmill before hand to with bear any under/over tolerance.
There’s a few things that can lead to this. Make sure the ball screw nuts are semi tight and the screw is tensioned. Next make sure your feeds and speeds aren’t too aggressive. Omios aren’t the best when it comes to fast curves. Lastly, this could have just been our machine but it did not like adaptive clear operation.
I havent taken a look at the ball screw nuts or screws yet ill try that, also found that when we calibrated the steps that Y was moving 40 thou over and the X was moving 20 Thou over. Seems like a lot and everything was working prior an hour. The holes we made previously were ovaly aswell, so that might have been contributing. I had to stop there but ill do some test cuts next time.
We were running 24k rpm, feedrate 60ipm
Make sure the coupling between the stepper motors and the ball screws is tight.
2 Likes
Did you change bit between bores? Collet runout could explain some of the issue (10-15 thou is a little big). The collets that ship with the OMIO are not the greatest.
Our problem was that we were breaking 1/8" bits suddenly when we switched to cutting 6061, we checked the runout and it was at least 0.006". When we purchased a better collet the runout was more like 0.0004"
1 Like
What is your belly pan material? what is your depth of cut? Are you using lubricant or air?
We’re running 6061 3/16 aluminum. Our Doc is .08” while using a coolant mister
We used the same endmill for both bores. I haven’t checked for collet runout, but were using some better collets then the original omio ones
I’ll leave the more mechanical questions of the OMIO to others since I haven’t really used one. What I’m curious about is what’s your full CAM process for the hole: what type of toolpath, stepover, doc, feeds and speeds, are you doing a roughing and finishing, how much material do you leave on your roughing, how many finishing passes (spring passes), etc
Also what’s your work holding looking like for your plate? clamps, tape and glue, etc.
1 Like
For Bore we just do one pass/cut with a plunge rate of 15ipm. For our pocket and contour, we do one roughing pass and then 2 finishing passes with a .01 stepover with ramping. Multiple depths with .08 step-downs. Using a 4mm endmill, we run a 60 IPM cutting feed rate with a 24000 rpm spindle speed. work Holding, we use an MDF Spoil board and screw the sheet metal, and part down
I been buying and returning collets for the last weeks… I have one good German made 7-6mm collet that will give me 0.001 runout 1.5" below the collet so I know the spindle is decent. Most of them I tested that were cheap were in the 3-10 mil runout 1" below the collet. This was with the collets and teh taper wiped clean… It does not take much to shift the cutting tip over enough to give the error you describe. Mine is the EPL stand alone version of the Omio so I don’t have cutter diameter compensation. I assume Mach 3 has that built in? One way to deal with this is to make a test cut piece each time. You can have a testcut.nc that makes a 1" hole and make test coupons that you run when you put in the endmill and then adjust the cutter diameter and re-post the the code before cutting something important.
Would you mind sharing a link to the collet you are using? Thanks.
We were getting “steps” in the workpieces and eventually found that both the X and Y couplers were not fully tightened on our new Omio.
Does anyone have a way to use cutter compensation in Mach 3/4 to dial in bearing diameters or do you just have to keep reposting code with different stock to leave values?
I’m pretty sure that the workflow most people use does all the cutter compensation in the post processor, so it pre-baked into the g-code and there is no way to compensate at the machine.
I just checked a random program that I ran on my Omio and it does not have the g-codes to know which direction it is cutting to allow for compensation.
The Mach 3 does have cutter compensation built in. The post processor seems to turn it off with G-code by default. I have never felt the need to dink with it. There are you tube videos on how to use it.
One thing I have found useful is to take 1 or 2 finishing cut with a spring cut. (a zero step finish cut.). The Omio with a small bit is not the most rigid of machines.If I need to adjust the hole size i do that with the stock to leave option while camming.