First off, Huge THANK YOU to Ryan and the community for this amazing project! My LR2 is complete and I’ve made a few cuts and now I’m hoping to garner some advice to address a couple issues / confirm a few things. Here is a bit of background:
Everything was purchased here except the printed parts.
No, I’m not using a cordless router anymore… Though the first cut went reasonably well, changing batteries every 20mins is obviously not ideal (especially with the LCD display becoming non-responsive for a number of minutes after un-pausing the print).
Router is a Ridgid R2401 (don’t hate)
I’ve read many threads here WRT feeds and speeds and want to confirm a couple things that until now seemed a but counter intuitive to me. I’ve made a lot of smoke and burn out a couple bits on the last few tests trying unsuccessfully to make new Y-Plates.
When I move the router through MDF by hand, Ryan’s ¼” single flute upcut goes through like butter (4mm DOC), though when in the LR2 for the Y-Plates, it made a lot of smoke. Settings: 8mm/s xy feed, 4mm DOC, 2deg ramp into material, 30000rpm router speed, slotting operation (Fusion 360 2D contour). I suspect you’ll say the 30000 rpm is to blame, but it worked without smoke the first time around, all while using a 2-flute up-cut. I also don’t get the concept of chip load (fz) or cutting speed (vc)…
Questions:
Are we limiting xy federate to 8-12mm/s because the LR2 steppers can not generate enough cutting force? Faster feed rate = skipped steps? If not, why do we have limit the federate to 8-12mm/s?
Do we need slower spindle rpms to account for the slower feedrate?
Once I figure out settings that work, am I good to play with variables in the FSWizard while keeping the cutting force below 1kg? Seems like the holy grail for the LR2 is combination of a slow spindle rpm, slow feedrate, deep cut, and a tool cutting force as close as possible to 1kg?
I skip steps in the x axis with a dull tool before the y axis skips. Would a stronger stepper motor on the x-axis permit higher forces / higher feedrates, making up for the single x motor vs the dual y motor setup?
I’ve found that sometimes the gantry runs with one z stepper slightly higher than the other. When at rest, everything sits flat and square. Only thing I can think of is that there are gaps between the z-screws and stepper shafts and when Z starts to move, one side starts to rise before the other. Should I reinstall the couplers with more stretch to hold the shaft tighter to the screw? Should I lube more/better?
I wired the shaft of the router (bottom bearing is conductive) so I don’t need to attach the alligator clip for the z-touch plate. Any concerns long term? If the connection breaks, will the probe function just try and drive the bit through the touch plate / material?
Last question: I installed an e-stop for obvious reasons. Is there any way to prevent the router from crashing into the material when the z-steppers lose power or do you just have to catch it?
Sorry for the lengthy first post with many questions. If I can provide any more info / photos / videos / etc. let me know. I’d like to not wreck bits or workpieces every fifteen minutes!
I have an MPCNC instead of a LR2, but I think you can go a LOT faster in MDF. I documented a small speed test here: Maximum side load. At 2.75mm DOC I could go up to 64mm/sec. My steppers are not that powerful, and I was running them in series. Don’t be too afraid to try out higher feed rates in test pieces.
My understanding of chipload is that it’s the thickness of a single chip. If it’s too thin, your endmill is rubbing more than it’s cutting and things may get too hot.
Re 2) Yes, that can help. Also single flute instead of 2-flute can help.
Re 3) I’m not sure about the deep cut. I had more success with a shallower but faster cut. I could go up to 4kg according to FSWizard. (In practice I’d stay well below that.)
Re 6) If the connection breaks the Z motor will just keep on driving, yes. Until it skips steps or something breaks.
Re 7) There’s no good solution I’m aware of. Happened to me today, and left a nice hole in my material…
Disclaimer: I’m a bit of a beginner myself still… and my experience is on an MPCNC.
Yes, me too. But today, I hit the switch, and the router was still in the process of slowing down while falling. I was cutting foam so it went straight through… less of a problem in wood though.
I had a problem with my Lowrider, where static from the dust collection would cause the control board to “reset”. I have the router on a relay so both it and the steppers shut down simultaneously, but the router had enough momentum to drill right down until the z axis hit bottom.
Good idea! I’ll wire an outlet to my E-Stop to kill the router as well. I figured the material / bit (or worse) are toast anyways if I’m killing the machine so might as well stop the router from spinning.
For what it’s worth, the material may not be toast. It would depend on the operation, but if you were making a through cut anyway, a hole may not be a problem. However re-starting the job does require the ability to reset the machine to the exact same zero point.
The smart money does this by powering up the machine in the exact same physical position (on a lowrider this may be up against the Y axis belt holders, and the x tight to one end of the gantry). Then, just before zeroing out the machine for the job, note down the coordinates. That way you can jog the machine back to the same place to start over.
I’ve not always been smart enough to do this myself, but it’s a good habit, in my opinion.
Regarding feeds and speeds, I do think the rpm needs to be reduced to eliminate the burning. Making smoke will kill router bits in a hurry, and could start a fire. When you say
you were routing by hand? You were probably moving the router faster.
You’re welcome to experiment with faster feed speeds etc. but in my opinion it is better to try deeper cuts rather than faster. Cutting deeper works more of the cutting edge of the bit, which spreads out the wear, so they last longer. Also, the steppers lose torque at high speeds, so they are more likely to skip steps. Ryan says every build is different though, you may be able to get away with faster feed rates as well.
I have not been using the feed and speed wizards or calculators myself. I usually start with the router at a pretty high rpm and reduce it if I smell burnt wood or note any burnt (darkened) wood in the cut. I’ve never made any visible smoke. YMMV, but I find I can smell “cooked” wood almost immediately…
Okay, you are at a tough spot, trust me. Once you get this you will be fine and everything will be easier (except metal).
Take two steps back, do a cut in pine or something similar, then maybe ply or walnut, MDF is the hardest to get right. So as you refine your settings in the other two know that MDF will be slower and or shallower than the other two. I think I do MDF at 9mm/s 6mmDOC but I turn my 611 way down to 2-3 even with a single flute. The single flute cheaper one noticeable dulls in about 45 minutes but will last a few hours. The better one lasts more hours than I keep track of.
If you are getting burning slow your RPM until you can not go any lower then your only other option is to move faster. Depth is not as much of a factor, the more rigid your machine the deeper you can go but only effects chip evacuation in a real cut (to simplify all these settings a bit) Stick with 2-3mm DOC until you get no burning with RPM and feed rate, then increase DOC.
1-No, but increasing speed vs decreasing rpm will loosen your part tolerance.
2-Yes, but more to account for the endmills spec just as much as feedrate. Chicken or the egg…
3-…yes and no but you are on the right track. Find what load your build can handle and then yes absolutely use that number…but running it at the bleeding edge all the time will result in screw ups. I am safety bob, I much rather get a complete finished job that takes 20 minutes longer than to have a screw up and waste material and time. Find something useful to make as a test piece (cup coasters for friends?) and make a ton of them in the same material. Change something every time and you will quickly learn the “right” settings for your machine. You would be surprised at how much time you save making efficient CAM is compared to 2mm/s faster cutting. Look for things like minimal moves, and minimal passes (of equal depth). I see so many people do two 5mm passes and then a 1mm pass, you could easily do two 5.5mm DOC and save 1/3 the time.
4- I do not think so, You should absolutely be no where near skipping steps that just shows you are really really far off with feeds and speeds. If you do feel that is an issue you can simply turn up your X axis stepper…surprise I under power them by a lot.
5-There should be no gaps, have a run through the instructions again. Also try turning each leadscrew by hand to set them under slight tension before running the job.
6-Nah
7-not as is, you can change to a single start lead screw but you will be sacrificing Z speed.
Not to mention blood, vitreous/aqueous humor, fully functional body parts (or at least nothing more than normal wear and tear), insurance deductibles (except for you poor bastiges living under socialist domination), tearful earfuls from SOs, etc., etc. Plus, the extra cursing scares the dog.
Would reducing the number of micro-steps on the Z motor driver compensate for this?
I’m sure this is an old topic, but I’m curious what the trade-offs are here (especially as I accidently ordered a 2-start screw for my MPCNC). Is there a type of work where Z speed is important? I’ve only just started, and my Z axis only ever moves a few mm, with long cuts in between Z moves.
It would alleviate the demand on the microcontroller, but the steppers will have more resistance as they move faster, which will mean they can max out the power supply at lower speeds. The steppers themselves also are more likely to skip steps when rotating faster.
It’s not a huge deal. If you just make sure your Z doesn’t move too quick, you will have more torque than the rest of us in Z. I would say try to limit it to 4mm/s to start. You can change the maximum mm/s with M203:
M203 Z4 ; Change the setting until reboot M500 ; This will save the setting.
