I’ve been having trouble cutting aluminum without bits breaking and I think it’s a table rigidity thing. My table has a slight wobble when the gantry does large enough direction change, which I think is the culprit. Any suggestions on how to stiffen this table up?
Gussets at the corners will take out any racking forces. But I don’t think it’s the culprit honestly. Its most likely speeds/feeds issues. And possibly chatter. Also you could be chip thinning causing rubbing. Putting the heat into the chip, not the workpiece and not the tool… That is the goal. It takes a while to find the right settings.
You mind sharing your cutting parameters?
I’ve been making nice chips using 17.7 ipm / 12500 rpm / .5mm doc with a carbide 2 flute upcut bit, but I’ve tried many different combinations of feeds/speeds all ending up with broken bits. I get about 3mm into a cut and my bit seems to always break the same way, it appears as if it just stops while the spindle keeps going like it got snagged. My acme’s are tensioned well and there is pretty much no play in gantry or at the end mill. The only thing that I can think of is that my table is vibrating and on suddent direction changes the gantry and the work area vibrate differently, causing the bit to hit a side or something.
May also want to check that your spindle is properly trammed, i.e. that the spindle is perpendicular to the x and y axes. Doesn’t have to be perfect, but the more perfect it is, the easier it is on the bits.
Additionally check that all your axes are tight, you shouldn’t be able to feel any play in the gantry on any of the axes if properly dialed in, if you do feel some adjust those backlash nuts and ensure the screws are properly tensioned.
Plywood and cross members
@Brandon_Byrne those feeds and speeds seem off to me. What aluminum alloy are you using?
With a 2D adaptive clearing path in 6061 aluminum I have run the following: 24000rpm, 39.37ipm feed, plunge 15ipm, 1.6mm depth of cut, with a conventional tool direction using a helix/spiral lead-in to get to that depth.
I think you may be suffering from a heating problem, you’re going quite slow, your chip load is actually very low at 0.0007 (0.004 is recommended alu chipload for most 1/8" cutters - I find it hard to achieve that on our hobbyist machines without deflection issues though). A low chip load can lead to overheating because the bit is essentially rubbing on the material more of the time causing it to heat up.
The chipload from my settings above isn’t much better, (0.008 vs your 0.007), but the feed rate is much higher, so I’m spending less time in the same area, resulting in lower temperature at the bit.
My table also vibrates a bit on direction changes too, I have a very similar table design to yours. Since everything is bolted to the table though I don’t think its causing your issue.
If you upgrade your table add a torsion box on top of it. If you film your cut and post it with sound we might be able to help diagnose it.
@Ben_Delarre I’ve actually read a lot of your posts about the higher feedrates / spindle RPM and tried some of it out. Here is one attempt, and it worked really well, I had walked away and came back to a broken bit and really hot workpiece.
I am cutting 6061-T6. I’ve seen that a lot of people are using the smw3d 4mm single flute carbide bit so I am going to try that next.
What bit were you using at those speeds?
I was using some nice 1/8" Destiny Viper tool - https://www.carbidecart.com/products/v20804s
I never walk away from the machine when running alu…especially at those speeds. Out of interest, where is it breaking, at what depth is it at? Is the piece vibrating perhaps?
Also what collet are you using?
I was using the collet that came with the spindle for the 1/8 bits. I’ve ordered the 4mm collet to try with the 4mm bit from smw3d. I actually have one of those destiny 1/8 bits as well. The last three bits broke exactly where the collet holds it, and from what I’ve read could be a symptom of the collet being damaged.
@Brandon_Byrne could be the collet, could also be the seating of the collet. Did it properly snap into place in the nut?
Also, by where did it break I actually meant where in the cut did it break? Is it always in the same place? Same depth?
@Ben_Delarre I circled the place that they have broken. They usually break around 2-3mm depth into the cut.
6061 isn’t impossible but 2024 is easier. The area you are showing is a tricky spot. Make sure it stays clear of chips. I didn’t see the reason for that much room so I redrew it.
Thats a good point, chip clearance is definitely a thing you need to pay attention to. I usually stand and vacuum the whole time with alu, I tried compressed air too. I also occasionally spray with wd40 for coolant when things are hot.
check the old post, I added some new files there that might help.
Thanks Eric I’ll try it out next week when I replace my 1/8 collet. I don’t want to break any more bits when it’s possible the collet is damaged.
What feeds/speeds would you recommend trying with the smw3d 4mm carbide bit? I will take a video of it and maybe that will help when troubleshooting.
@Brandon_Byrne Some good speed examples here: https://docs.google.com/spreadsheets/d/1_WRXjA6vBs_S9UgIOEO2wtbqvcLWxgHOPgzzNYFg8u4/edit#gid=0
@Brandon_Byrne this is also a good read: https://www.smw3d.com/blog/what-is-the-right-feeds-and-speeds-for-my-cnc-router-kit/
@Eclsnowman Thank you for that article. It is well done.
@Brandon_Byrne Check that collet. The one I had was 4-3 (4mm to 3mm). Getting a proper 1/8" collet made loading easier and was tighter.