Good morning. Our team is just getting into the CNC game with our OMIO X8. One of the first things we tried to do was drill 50 rivet holes into a piece of 1"x2" tube (After doing practice holes 3 at a time). We got some tool profiles from another team as a place to start with the speed and feed rates. We are using this single fluted 1/8" end mill and trying to mill .201" holes. During the milling process, the end mill broke after around 20 holes. This happened a couple of times.
Any suggestions on what settings we might want to tweak given that it fails after about 20 holes? Is it a heat build up thing or is it just random when it broke? We have air and coolant mist blowing on the end mill during the process. Our current settings are 20,000 rpm, 56 ipm feed rate, and 18 ipm plunge. Pass depth is set to .015 inches so I think the CAM software says it’ll take 5 passes to go .075 inches down. There doesn’t appear to be any chip welding on the end mill after it breaks. The CAM is set to do a profile cut with ramping at 5 degrees. What other settings are important to know?
Why not use a drill? We use a stubby split point cobalt drill and can drill 20 holes in under a minute. I like colbalt over carbide drills because drills always get dropped or the occasional jogging errors. One McMaster 28765A61 can drill a robot worth of holes easily
You’re feeding .0028ipt, which is an extremely high load for an 1/8in tool. Getting closer to .001ipt will prevent excessive tool deflection. I am assuming that you’re using a 1-flute tool. If not, I strongly encourage the use of 1-flute carbide tooling on routers, especially 1/8in diameter.
By using just a .015in DOC you are concentrating all of the tool wear in that first .015in of the tool. Rather than discrete step-downs I would suggest helical bore operations for all of these holes, then a .005-.01in cleanup pass on the diameter at full-thickness DOC.
As a point of reference, when I route aluminum I usually run:
24krpm
24ipm
air blast
full DOC on sheet (up to ~.09in)
6° helix/ramp angle
A tooling change might also help immensely. A real drill bit or 3/16 router bit will be stiffer and more robust.
Not using a drill bit is probably due to lack experience. When we ordered the OMIO we were told we’d want some different sized end mills, no one mentioned the ability to use drill bits in it. I did read an old thread on here this morning that mentioned the idea so it’s something I’m willing to try. When using a drill bit, I assume we should switch to a drill operation as opposed to a profile cut in the CAM software. The McMaster 28765A61 has a size of .191", if we truly want holes .201" would we better off with the McMaster 28765A57, which says is .201"? Which size collet would I put either of these drill bits in? Is it better to use a collet sized a little bigger or smaller than the shaft size? Sorry if these are silly questions, I’m a computer guy trying to take a dip in the mechanical ocean. Thanks again for your advice.
Thanks James. I think I understood at least 90% of this information and should be able to decipher the other 10% after a little more research. I was using a 1-flute Carbide end mill (link in original post). I’ve read a lot of references to the helical bore operations. I’ll have to look into see how to do that on Aspire 9.5, which is the CAM software we are using. I don’t have the software on a computer with me right now, would that be a different operation choice as opposed to the profile operation I had chosen? Or is it a setting to change for the profiling operation? I’ll also attempt using drill bits as recommended. Thanks for your feedback and ideas.
In more industrial-oriented CAM packages ‘helical bore’ is its own operation. You may be able to effectively get a helical bore by doing a full DOC profile operation with a helical plunge. However, I am not familiar with Aspire 9.5, so experimentation with exactly what that CAM kernel outputs will be required.
You would want to use a drill bit sized for the hole you want. If you want 0.201" holes, use a 0.201" drill bit and use a drilling toolpath to make only vertical moves. Collets have a clamping range that maxes out at the stated size and goes lower than that. For a 0.201" tool, you would want a 7/32" collet. Here’s a McMaster page for ER-20 collets showing the clamping range. I think the OMIO uses ER-20.
Despite the huge feature list of Aspire, you might not be able to find a helical bore operation in it. Aspire seems targeted to the v-carving crowd making signs and 3D art. You might want to consider trying Fusion 360 for CAM.
If at all possible, I’d recommend not using a 1/8" endmill to cut aluminum. I’ve found 4mm endmills to be much more robust than 1/8" and there are very few features needed on an FRC robot that need a tool diameter less than 4mm.
Thanks. I do have a few 4mm 1-flute end mills so I could definitely give it a shot. I don’t think the tool database file we got from the other team included any 4mm tools defined. Would you happen to have any recommended speeds and feeds for a 4mm end mill? Would using a profile operation with ramping still be the preferred operation? Should I try to do the full DOC with a ramp as suggested by @JamesCH95 with a 4mm end mill?
If we’re only doing a couple holes we interpolate with a 4mm endmill but always use a drill if there are more than 20 or so holes.
0.201" is a little big if you’re riveting CNCed parts to CNCed parts with 3/16" rivets, which is why we prefer a #11 drill. A #9 is probably the biggest I would go.
We use a 5mm collet for a 0.193" Drill. A general rule is you never want to use a collet smaller than the tool, but you can safely use a collet about 0.02" larger than the tool. I wouldn’t run an off nominal size collet for an endmill but it’s fine for a drill. Some metric collets will even have a range marked on such as “5-6”
Thanks for the education and insight. I think the .201 size came from a youtube video I was following for CADing the drivetrain and the other team helping us mentioned using this size for their rivet holes. Since we are in the learning process, I’m willing to try a number of things to size what works best for us. I’ll order a #7, #9, and #11 and try them all on some test pieces to see how the riveting goes.
FWIW we make most of our 3/16 rivet holes .201in, easily replaced with #10-32 if required. It has never caused an observable issue for us either way though.
If you are set on using a Jig or CNC for these holes, I might suggest CAMing the job with multiple step-downs (passes essentially), instead of using the normal climb-style of bore cutting. If y’all are already doing this, try making the step-downs smaller. Might help to use some lubricant like WD-40, also. Additionally, lowering the feed speed of the CNC could help eliminate some of the transverse (and possibly axial) load on the bit. If none of these solutions work, then I’d agree with some of the other people here in saying that a drill would probably be better. Also, the page for the bits that y’all use doesn’t even mention anything to indicate it can (let alone should) be used for cutting sheet metal or drilling metal. The endmills y’all are using also seem very long, which could be a lot of transverse load for y’all’s particular application.
One more take to add here because we routinely cut holes this size with a 1/8" bit. We got through all the parts for last year’s robot without breaking any bits.
There’s a non-obvious effect on the feedrate when you interpolate a circle with a bit that is close to the finished hole size. This Haas video has a nice explanation, but it boils down to the difference between the programed path that the center of the cutter follows and the point at the edge of the cutter where it meets the finished hole. That contact point moves much faster than the programmed feed rate and you need to adjust for this effect.
For the example you have given, bump up your spindle to 24k rpm and drop your feed rate down around 15 IPM. Your step down can be larger (.03-.06 in) and I will second the recommendation to use a helical plunge. That’s how I run it.
Please just remember that such a low feed rate will help make small radius cuts but is too slow for linear cuts and hence should not be your default.
These endmills look awful. I don’t think you’ll be able to do very well with these. Try and get some Huhao, Onsrud, WCP, or Thriftybot endmills. 4mm is best. Cheap 1/8" endmills abound on Amazon and they can barely cut plastic. I’ve tried a few brands and apart from HQMaster, they are AWFUL.
Using a real drill but as mentioned is good too. You can get great split point short drills from McMaster.
I have good results using the uncoated carbide speed and feed chart at the bottom of this page:
Also, running at 18K - 20K spindle speeds isn’t going to really slow you down that much in overall time. I have found that I get better results running at that spindle speed than running the max spindle speed with the Huhao or HQMaster bits. Others show different results so you need to find what works for you.
Router bits like to cut sideways. If you want to cut vertically and make normal holes, use a drill bit. #9 is my favorite for 3/16" bolts and rivets for a nice clearance fit, but might not fit into your collet setup.
The helical bore parameters that others have posted seem aggressive… maybe we should to try being more agressiver.
Thanks for the assessment. Were were advised to get some cheap ones to start off to get a feel for how the work flow goes so I just randomly picked some. I actually have some HQMaster ones scheduled for delivery today and I do have a couple of the WCP 4mm and 6mm ones. I was saving those until I knew what I was doing I’ll play around with some of the different techniques to see the differences and make sure I switch to the good end mills when it comes time to do more than drill holes. I ordered 7, 9, and 11 drill bits from McMaster that should arrive tomorrow. I’m liable to go with them for drilling rivet holes.
Getting REV 2x1 would save the work since the holes are sized for #10 hardware and 3/16" rivets.
Edit: measured the holes on the pieces we have in the shop and they are .201. The only thing with the REV 2x1 and 1x1 stock is it only comes in 47" lengths
I’ll play around with some of the different techniques to see the differences and make sure I switch to the good end mills when it comes time to do more than drill holes. I ordered