Hey guys, First time this had happened to me and it's happened twice now. I'm cutting a 2D contour into some solid ash hardwood with a 1/4" spiral down cut bit (Amana 46202-K). I'm using the default feeds and speeds from the bit that is imported into fusion 360 and going at 1/8" deep per pass. After stalling I noticed the router had moved some in the mount so I fixed that, checked all my eccentric wheels, retrammed and am currently resurfacing my spoil board. Any ideas on what might be causing this? I hear the rule of thumb for cut depth is hard the bit diameter which is what I've done up till now. Should I go more shallow? Not sure if there are any machine settings or variables to look out for. Here's an image of one of the jobs. The piece was fixed to the spoil board but it looks like the router might have skipped a step or two because it ran over and cut into the part for a few passes. EDIT After thinking on this a little more I'm wondering if the machine stalled because it missed a step somewhere and started the next pass offset from the other and the depth was too much. I'm still not sure what would have caused it to move off the original path though. Just a theory, unfortunately I wasn't watching the machine when this happened.
What are the default speeds and speeds? Those are based on certain factors and may not be right for your machine.
Downcuts needs very good chip extraction to avoid packing the flutes. A compressor, an air solenoid and nozzle (docs:blackbox:connect-coolant [OpenBuilds Documentation] for example) Try a regular upcut endmill as a comparison With a downcut you'll have to a lot less aggresive with the parameters
My bit specs were imported directly into Fusion 360 with the manufacturer recommendations. This is what the feeds and speeds were set to based on that. Okay, I can give that a shot. At the top and bottom of my parts it's cutting straight across the grain and I was thinking it might have been struggling there and possibly skipped. Since it looks like it only skipped in the x-axis. I was reading some other posts where you mentioned the current to the motors might need increased slightly. Is that something you think could benefit me here? If so, would I slightly increase the current to all of the motors equally or just the x motor?
Sounds good! Thoughts on a compression bit like this? Amana Tool 46170-K CNC SC Spektra Extreme Tool Life Coated Compression Spiral 1/4 D x 7/8 CH x 1/4 SHK x 2-1/2 Inch Long 2 Flute Router Bit (Replaces item no. 46169) I'm usually cutting into solid hardwood ranging from 3/4" to 1.25" thick.
First just try a more conservative cut with a regular bit as a test - lower DOC or feedrate Are they assuming a $2000 machine or a $100000 machine?
Gotcha! I'm honestly not sure about that last question. Within fusion you can import or upload bits from their online library and I've never really second guessed those parameters. I'm fairly new to all things CNC and not sure how they determined the best settings for those so I just have left them alone.
My point is, manufacturer ratings might be on the aggresive side on a hobbyist router. Their main business might be machines a lot larger/stronger than yours. Derate accordingly
Honestly, I haven't ever really looked at these values to know what is ideal vs not. I've normally just ran with the defaults as mentioned. If there's any documentation ot video online that explains these in more detail I would appreciate it. Even better, if there's a rough guide for the Lead 1515 in terms of speed and feed rates that would be great. However, I understand that might vary depending on the machine use.
Did you mean to attach something? Thanks Peter, after going through this and a bunch of other charts and documents online, I think my main problem is thinking the manufacturers recommendations were fine with my machine. This is the first time I've had issues but also the first time I've cut a hardwood this hard. Do you know what would be a good average range feed range would be for cutting hardwood on the lead 1515? I saw another post on here about the lead 1010 where someone was running around 120 IPM which is decently slower than the 180 I was running. I also saw a few videos with some other hobby machines where people ran as slow as 60 IPM. So I'm a little unsure now of how much yo cut back on my machine. Do I cut it in half and start at 90 then work my way up until I hear the machine start to struggle? Or is there a range that's expected with this particular machine when it was originally designed? As always thanks for your help and knowledge. You've helped me through multiple issues on here and I really appreciate it!
How hard is a piece of hardwood... See you can't rely on a fix number all the time. Test cuts, experience and time I start any unknown material at 1000mm/min and then play with the override sliders. Make chips, not dust, but also don't overdo it
HA, I know. After spending hours today reading and seeing all these equations on chip load, speed and all that. There's just so many variables that seem to make those things impossible to go by other than running a bunch of test cuts on the machine for yourself. I'll give that a shot. I did order an upcut bit today as well and plan to try that out also.
You were cutting at 4572mm/min (180 ipm) That is very fast. For most woods, I started with 100ipm (2540mm/min). Why that number? It was the default number in Sketchucam when I did my very first cut. For 3D carves, I go up to 3000- 3500 mm/min with a 40% stepover for roughing and the same with an 10% stepover for finishing with no problems. However, these numbers I mention are for cutting at 1/2 the endmill diameter for your depth. I would experiment with your machine to get an idea of how aggressive you can cut. Also, dial in the acceleration rates. Pick a maximum speed that you think you need your machine to go, dial up the acceleration until the motors stall, then back off about 20%. This will greatly speed up 3D carves where there are a lot of short curves. I recently was cutting 12mm (1/2 inch) depth of cut at 2500mm/min with a 1/4" endmill on some Douglas fir 2x6 material and it was able to do it, but the cuts were not a very pretty. It was actually done accidentally. I screwed up the CAM for the cut and entered the depth I would cut for the finishing pass into the roughing pass. The finishing pass did clean it up though. The wood was very wet. With wet wood the chips were hard to clear. I had to pause the job and clear them out with a screw driver (lesson learned). Honestly, I think I could continue this with soft woods and would like to try it on dry wood.
Thanks for the detailed information! Just for clarification, when you mentioned dialing in your acceleration, are you referring to the feed rate like you mentioned running at 100 IPM? Most of my bits are recommended to run at 18000 RPM so I set that on the router11. If I'm running at a slower feed rate should I change the spindle speed as well?
The acceleration is how quickly the stepper motors spin up to the rpms necessary to move the gantry at the feed rate you told it to cut at. It is in your grbl settings and is the $120, $121, $122 values. The Wiki explains it better than I can. Grbl v1.1 Configuration · gnea/grbl Wiki
Just wanted to follow up on this. I tried again, this time using an upcut bit. The default speeds and feeds were actually slower than the downcut bit I was using before so I just ran with that. I ran 18000rpm at 100 ipm and it went a lot better. I think I'll stick to the upcut bit moving forward for thicker hardwoods. Here's a few images of my chips and pieces. The edges turned out a lot better along the endgrain than before.
