hello ive noticed that my cut times are very long i cannot push my lowrider past 12mm/s with my current router if i go anyfaster it will get caught skip steps and ruin everything
ive been looking into water cooled spindles and before i purchase one and spend hundreds of dollars i would like to know if this would increase my speed and if so could i push up into like the 24mms speeds or am i way off and that is way too fast i was also looking at what the main differences are between the 110 and the 220 i can easily install a 220 outlet in my workspace
Hi Danny
I have the Makita router and get good speeds in mdf and ply and plastics - certainly much quicker than 12mm/s without too many problems. I can’t recommend a better router as I don’t have experience with other options.
Maybe not helpful, nor answering your question, but I think you might be swapping one set of problems for another if you go with a water cooled spindle. If you’re prepared to investigate why you’re limited to 12mm/s there might be a simpler/cheaper fix.
I just looked at my last cut in ply and I cut 3mm deep at 30mm/s, single flute 3.175mm bit. That was using the LR3 an a Makita router.
Probably not a router issue unless the router is actually bogging down when you are cutting. I had to increase my stepper current to prevent skipped steps. You just have to make sure you keep the temperature of the steppers <~40C to prevent damage.
Hello @dan_tha_man, what material are you cutting? What bit size and type are you using? Have seen Philipp get great results with new sharp carbide single flute upcut 1/8" bits, but have also seen Philipp struggle when unknowingly using a dull bit. Am running low rpm with vac to help reduce heat from dulling bits.
I keep it way down at the bottom end maybe 2, or even 1. Not sure how that equates to the Dewalt. As @staffordj says, I have also upped my current a little to stop skipping steps. I can get the drivers a bit warm - not hot, and the steppers themselves never get warm. I think I’m running at 1 amp at the moment. Maybe a bit more in the past. I cut in a cool garage though and it never gets really warm here in Scotland.
Feeds and speeds are very dependent on the end mill that you are using, as well as the material, DOC (axial depth of cut) , cutting width (radial DOC - think slot vs. pocket) and router speed.
The thing that you want to shoot for is the correct chip load for a given material. Use of a F&S Calculator will help (I use G-Wizard - free for a month trial, a reasonable subscription fee for the first year - wait for the sale price of $59, and lifetime free usage after the first year). It has a bit of a learning curve, but there are lots of articles and resources on the site to assist.
Changing the end mill to a 2 flute from a single flute could also help you bump up your feed rate. but again, you need to make sure that your chip load is within the correct range, so trial and error is not the best way to approach things.
A dull mill (bit) will certainly cause issues. Especially likely if you haven’t calculated chip rate correctly and then do some cuts.
Lastly, stating your feed rate in mm/min rather than mm/s is helpful, as Marlin uses this parameter (I suggest setting up your tools in Estlcam to be the same)
As an example, I just finished cutting 10mm DOC slots through aluminum at 2250mm/min (37.5 mm/s) using Trochoidal milling at 20000 RPM (about 4/6 on the speed dial) with a single flute 1/8" mill. It worked great! But it took me a few hours to figure out the correct feeds and speeds before I started. A straight (non-trochoidal) cut would be much slower, more in the range of 475mm/min (7.9 mm/s) at 20000 RPM, and slowing the router to 1 or 2 (10000-12000) would require about half that feed rate.
If you’re using the DeWalt 660, it has a fixed speed in the range of 29,000 RPM. Using any bit larger than 1/16 inch will make the freed rate pretty high.
One choice is to put a speed controller between the mains power and the router. That will let you slow the RPM, but the torque will also diminish.
You can try a number of the suggestions above. Remember, contrary to what we may think, faster RPM or feed rate is not always the answer.