Omio CNC Configuration Ruining Pieces

Technical
,
1

Hey guys whats up!, We have been having trouble with our cnc machine. It keeps ruining the pieces. Our config is on a Carbide Single Flute 4mm, at 24000 RPM, Feed rate at 1500mm/min, with multiple depths at 1mm.

If anyone has any idea on what can help please do tell!

WhatsApp Image 2023-11-01 at 4.53.38 PM
WhatsApp Image 2023-11-01 at 4.53.38 PM768Ă—1024 148 KB

1 Like
2

Try cutting your feed rate in half to 30 IPM and the amp down to 22k

1 Like
3
  • Is the problem new, or is the machine new? If you’ve just set the machine up for the first time, make sure the couplers on the three axes (stepper motor → ball screw) are properly tightened and not slipping.
  • Make sure your tool doesn’t have any aluminum welded to it, and that it isn’t chipped. If it is, replace it.
  • Is the tool known to be from a good source? Some inexpensive O-flute tools (well, tools in general) don’t have proper cutting geometry and won’t work well no matter what. Some of them will mush through wood and maybe plastics, but falter in aluminum.
  • Is the collet known to be good? Cheap collets can have a lot of runout and cause good tools to perform poorly.

Once you do all of these things, I’d go back to feeds and speeds.

On our Omio X8, we usually run 60 IPM (1500mm/min) at 15,000 RPM, 1.5mm pass depth for a 4mm single-flute cutter in aluminum. This equates to about 0.004" (~0.1mm) per flute chipload. I prefer about 0.003-0.005" per flute on similar cutters.

2 Likes
4

While I don’t have much experience with a 4mm bit, with 1/8” endmills I had a lot of success at 18k rpm and 30ipm, and about a .030” doc. A lot of that looks to be reweld from the chips. It could be they aren’t fully evacuating. What grade material are you cutting? Last time I saw reweld that bad on aluminum it was either a dull bit, the spindle speed wasn’t right, feed rate wasn’t right, or it was 5052 or similar aluminum.

Lighter cuts =/= better by the way, and what kind of mist are you using? In my experience, there should be no need for that much coolant on aluminum on a router. Coolant is designed to help keep the bit cool, but so are chip load calculations. Between the two, you don’t need much.

1 Like
5

It looks like your bit is just melting the aluminum and pushing it out of the way rather than making any chips. Is the bit flute full of aluminum welded on to the bit? Kind of surprising that the bit hasn’t broken yet, but the shallow 1mm DOC is probably saving it. Have you tried cutting with another bit?

1 Like
6

Are you using air to keep the chips out of cut? What lubricant / coolant are using? We use WD50. Other use isopropyl alcohol Once you start galling (rewelding) you need to stop. It will not get better. 1500 mm/min is a little fast. Back off to about a 1000 and work back up. I have not had a lot of luck rehabilitating a bit once it is badly galled.

The thread Omio tips and tricks has a lot of good advice.

2 Likes
7

This may or may not apply, but from your picture I’m not sure if your clamps are putting some upward flex into the aluminum sheet? If the stock isnt held down flat against the spoil board, it turns into a trampoline when the cutter moves by and tries to lift the stock.

FWIW, I’ve always preferred to run slower feeds and deeper cuts with aluminum, 20k RPM and 700mm/min at 2mm max cutting depth for a 4mm single flute mill. As mentioned above, I would try cutting your feedrate in half and doing some test cuts.

1 Like
8

I find this video inspirational, 6mm single flute at 150 ipm, 24krpm, mist cooling, 3mm depth.

IMHO a more prudent setup would be 15krpm at 30 ipm. :slight_smile:

1 Like
9

I have helped a few teams with this issue. Here are a few solutions.

  1. Confirm the spindle is turning in the correct direction.
  2. Make sure the spring collet is inserted into the collet nut first. You should feel a click as you push it in from the backside of the nut. Then put the nut on the spindle and then the bit in before you tighten.
    Inserting a spring collet into a router - Google Search
3 Likes
10

hey guys thanks for all the help, I will start trying the different solutions.

I just have a question for those who use omio cnc. Whcih post processor do you guys use?
We use fusion to generate our gcode.

Thanks!!

1 Like
11

I dimly recall using the generic mach3 post-processor, which you can get from the fusion cam repo

The WCP guide has some good advice, in case you haven’t seen it.

12

We use Fusion to generate G-code. No issues.

13

2 things:

  1. What brand endmill is this? A good endmill is vitally important here. It doesn’t need to be expensive but it does need to be good for aluminum. I recommend Grewin, Thriftybot, or WCP endmills, with Grewin being the cheapest by far per unit but requiring a $100 minimum order and a quote to order. I can always lend a few endmills out as long as I get some back.

  2. Don’t run your IPM too low. Minimum for me would be .001" IPT chipload, which means at 20k RPM, 20 IPM is the minimum speed. For a 6mm most manufacturers will recommend 0.003-0.006" IPT. If you want to reduce heat from the cut, your best bet is to reduce your spindle speed down to maybe 16k RPM, run at 32-48 IPM, use mist coolant or air blast, potentially reduce depth of cut (though 1mm is already really low for a 6mm) and, above all, use a good endmill.

5 Likes
14

GUYS!! I´VE OFFICALLY BECOME A CNC GOD!
THANKS FOR ALL THE HELP!
but on a real note, thanks to all the people who helped out. This are the specs that we used to get it to work without coolant.

When milling an 1/4" aluminum 6061 T6 sheet:
4mm Carbide end mill @ 24,000 RPM
Feedrate 1000 mm/min
Multiple Depth Maximum Roughing Stepdowns: 0.5 mm

3 Likes