Routing plywood: conventional or climbing cut?

[626Pilot]

I'm routing some Baltic birch plywood, .68" thick and I think 13 plys, on a Probotix Meteor CNC machine. This job is not too fancy. A 3/8" center-cut end mill will drill a few holes, then plungebore a few 1/4" holes, and finally mill a few pockets. I keep hearing different stories about whether plywood should be routed with a conventional or climbing cut. For this particular application, which would be better - or does it even matter?

PS: Fixturing is fun! I'm going to post a thread later about how I got everything properly aligned. That definitely took some figuring out.

[geneb]

If you're cutting outside, do climb with a .001 offset and then follow it up with a full depth conventional cut, no offset. Use conventional/climb if you're doing an interior cut.

This technique is good for any material when using a CNC router. Basically what you're doing is cutting in such a way that the bit deflection is away from the work. By offsetting the cut by .001, you're giving the follow-up conventional pass the opportunity to clean up the edge as it goes - the bit will be nearly unloaded so no deflection will occur. You'll end up with a nearly perfect edge.

What software are you using to do the toolpaths?

g.

[KAS]

That's interesting, climb cutting by hand is looked down on because of the chatter and opportunity for the wood to catch. I would never thought differently using CNC.
They designed compression bits that simulate climb with the safety of conventional. I'm sure the bit size matters though, I'm using 1/2" shank in a OF 2200

http://www.rockler.com/freud-double-com ... router-bit

[626Pilot]

Sketchup, with a free CAM plugin called Phlatscript. It was developed by people who like to turn blue foam board into model aircraft. It's pretty good for free software! They developed it for their Phlatprinter, a tractor-feed router, but they've added gantry router settings and other stuff that could only be useful to people who don't have a Phlatprinter. I like these guys a lot.

I did some test drills with a climb cut. It cuts like butter. There's no fuzz or tear-out. The end mill has some kind of fancy coating with lots of letters in it that's supposed to make it last longer. When the router does a plungebore, it drills the center out first and then does a descending helix to take out the remaining material. Seems like a good way to extend the life of the end mill.

I have read that climb cutting is fine if you use a CNC router. This things has HUGE steppers. I doubt any human could win a tug-of-war with one of them.

[geneb]

I've never used a hand router for anything other than trimming material.

I've got a ShopBot PRT Alpha 96 and I've run a LOT of plywood, MDF, and OSB through it. I almost always use a downshear cutter as it won't lift the parts off the table during cutting (I use a vacuum hold down system). For a 1/4" bit on Baltic Birch, I'll run it at about 1.5-2.0 in/sec @ 12k on an Onsrud "O" flute cutter. I get awesome edges that way. The 'bot sports NEMA 34 motors and rapids at 30in/sec. When it's homing, you tend to want to leap out of the way just in case.

The clean-up pass will remove any chatter marks.

A compression bit in a CNC router is a good choice if you need to make sure there's no tear-out on the top & bottom surface of the material. This is often used when doing cabinet work using expensive plywoods with "delicate" top & bottom veneers.

I use Aspire from Vectric. It's THE best CNC router toolpath software I've ever seen. The workflow in Sketchup makes me crazy so I haven't used it much.

g.

[KAS]

All my woodworking is done by hand although I would love to pickup a cnc someday.

[Fractured_Flicker]

The decision to climb or conventional cut depends in large part on whether the machine can handle it with the material in question. Climb cutting is more efficient since the edge of the cutter is helping to pull the material into the cut and this generally works well with CNC machines. Having spent several years working in a machine shop with conventional machines I found out the hard way that the backlash(slop) of the lead screw on a manual milling machine would allow the cutter to pull the material into the cutter in jerks during climb cutting which would leave gouges in the workpiece and possibly damage the cutter.

Phil

[626Pilot]

I use Aspire from Vectric. It's THE best CNC router toolpath software I've ever seen. The workflow in Sketchup makes me crazy so I haven't used it much.

Sketchup's internal resolution limit has made me hopping mad on several occasions. The inference engine likes to subtly tweak geometry so that it's 0.01 degree off, and then suddenly nothing works right, and you have to redo 45 minutes of work because there's no way to un-tweak it. Sometimes the only thing for it is to blow a part up 10x bigger, work on it, then shrink it 10x. I've just got so adept at dodging those problems that I don't feel motivated to learn another, although I hear DraftSight is nice.

In any case, you can get Sketchup for free, and Phlatscript is free. And LinuxCNC is free. You could theoretically run Sketchup on wine (if it feels like running) and have a 100% free CAD/CAM toolchain. Probotix sold me this thing for about $4500, including tax and ~1,500 miles of freight. They included a full computer with LinuxCNC. If they had to pay for a Windows license and professional machine control software, it could've added $500-1,000 easily.

I like the ShopBot. It costs more, but it looks like you get what you pay for. Built-in stand, six legs rather than four, better support for the spoilboard, more welds and fewer bolts. Looks like it has a few more inches of Z. Bigger motors, too. The ones on the Probotix are 420 oz-in. NEMA 23s, and it does rapids at 200 inches/min. If I was going to start a serious business machine shop, I would definitely look at getting a couple of ShopBots.

The Probotix is pretty easy to wrench on. All the places you need to put an Allen wrench are easily accessible. I learned this when I saw the X stage jerking - turns out one of the set screws on the stepper coupler was loose, probably from shipping. The motors are pretty noisy when they're holding still - makes the whole room sound like a pipe with water rushing through it.

One thing I don't like: they set up the router and flood relays to be normally open. I don't quite get why they would do this. When you turn on the control box, the spindle starts by itself. That is a little scary.

Climb cutting is more efficient since the edge of the cutter is helping to pull the material into the cut and this generally works well with CNC machines.

I've read that it's better at ejecting the chips, and that it tends to push the piece down instead of pulling it up. The axes all have anti-backlash nuts, so I don't expect any slop.

[Polygonhell]

On most CNC machines it's common to only climb cut, because the backlash on the axis is so minimal when compared to manual machines.

[jlmccuan]

Outside profiles are clockwise and inside profiles are counterclockwise. With most tooling that will be climb milling. Laser and plasma cutting follow the same principle but, of course, it's neither climb or conventional.

[geneb]

The bit geometry determines if the part is pulled away from the bed or pushed into it. A downshear cutter will push into the bed while an upshear cutter will pull the part away from it. Compression cutters are upshear for the first half of the cutter and downshear for the rest. This helps ensure good top & bottom cuts without any tearout.

If you cut aluminum, always use upshear. It'll throw the chips away from the part and lessens the chance of reweld.

A Windows 7 license is about $80 and the last time I checked, Mach3 was around $175, so no - it wouldn't add $500-$1000 to the cost of the setup.

I'd be worried if your steppers are making noise while the machine isn't moving. I don't think that's normal.

g.

[626Pilot]

I'd be worried if your steppers are making noise while the machine isn't moving. I don't think that's normal.

I think it's just holding current. You can hear it a little in this video (not mine):
[youtube]http://www.youtube.com/watch?v=Eg7KOiB3XzE[/youtube]

Probotix has been pretty good to me. Before I bought the router, I read somewhere that if you ask them to extend the Meteor's X envelope from 25" to 35", they'd do it for FREE. Sure enough, I called and asked and they hooked me up! I guess everyone started doing that because now they sell a new model called the Nebula, which is just a Meteor with 35" of X for $500 more. (Worth it!) They are also really good with support. They always get back to me the same day, and they always have good advice about what third-party accessories are out there. I bought a SuperPID spindle controller, but haven't mounted it yet. (When I do, I don't think I'm putting it on the gantry.)

I think whoever said you should get the biggest router you can afford that meets your needs was right. I'm milling 200 12" wide plywood boards, and having enough X to fit three simultaneously is saving me a lot of time.

[jlmccuan]

I run Mach3 on my CNC router, lathe and mill. For CAM package I use HSMXPress for the 2.5D stuff, MeshCAM for 3D surfacing, and VCarve Pro to fill in the rest. The computers that run Mach3 are all WinXP and have no issues doing their job. Some folks run later versions of Windows after solving some timing issues. My router uses the 2-1/4HP Hitachi M12VC. Once you set the speed it has it's own system that maintains that RPM under load. I bought a PID setup but after installing the Hitachi never felt the need for it. I run mist coolant, shop vac and power to the router on relays and code those into my programs where needed. The mill and the lathe run mist coolant, but spindle control is done with VFDs which handle soft start, braking, direction and rpm. The VFD's are definitely the best setup by far.

[geneb]

The ShopBot's motors make no noise when it's not in motion. It might be just due to the size of the motor and the huge driver each one has.

Your first upgrade should be a spindle. I've got a 2.2HP HSD spindle on the 'bot and it's awesome. If you've got your speed & feeds right, you can talk in a normal voice right next to it while a job is running.

I used VCarve Pro for years until I cobbled together enough to upgrade to Aspire. They're both awesome products.

g.

[626Pilot]

Your first upgrade should be a spindle. I've got a 2.2HP HSD spindle on the 'bot and it's awesome. If you've got your speed & feeds right, you can talk in a normal voice right next to it while a job is running.

That sounds like a good upgrade. I've been using aviation headphones to keep the noise out, but that gets old after a few hours. Can you recommend a particular model? I want to cut wood, aluminum and acrylic.

I've been using a three-flute mill with feedrates around 50 in/min. Does that sound reasonable? Mainly, I want to extend the life of the tool.

[geneb]

None of the spindles I know about are small enough to fit on your machine. Any 3 phase spindle (You'll need a VFD to run it) that can fit properly on the machine will be a huge improvement over the router.

For good quality cutters, my go-to vendor is Centurion Tools - https://www.centuriontools.com/router-b ... -bits.html

I'd also recommend using a chip load calculator. That will help you get the optimum speed & feed rate for the bit you're using.
Here's a nice guideline for that kind of thing: https://www.vortextool.com/images/chipLoadChart.pdf

Pay attention to the sound the cutter makes. If it's really loud, it's screaming "I'm HUNGRY! FEED ME!". Either increase your feed rate or decrease the RPM.

I would recommend you do a number of test cuts on scrap material - it'll really help you dial in the feed & speed for each type of material you plan to cut.

The first thing you might want to make (if you don't already have one) is a dust collector foot that will attach to the bottom of your router or spindle. You connect a shop vac to it and it keeps you from drowning in sawdust.

Any time the router/spindle is running, wear safety glasses. You never know when the bloody thing might throw stuff at you. I got my ear nicked by a screw that a 1/2 cutter tore out of some particle board I was cutting - that reminds me - if you're ever going to cut particle board, run a metal detector over it! People have found all kinds of metal crap in particle board and it destroys cutters in the blink of an eye.

I tend to cut a lot more slowly than the machine is capable of - I run most plywood at about 1.5-2.in/sec (90-120 in/min).

Another thing to keep in mind is cutting depth per pass - you typically don't want to make full-depth cuts on the first pass. A good rule of thumb is to keep your pass depth the same as the tool diameter.

Go to http://www.onsrud.com and download their catalogs. They contain great info about speeds & feeds and how to adjust them based on pass depth.

g.

[jlmccuan]

I'll second Onsrud and a VFD spindle. The VFD also acts as a PID keeping your rpm constant and can brake your spindle to a stop so there is less chance of reaching in after a program too quickly and finding a still spinning cutter. I have a water cooled spindle on one machine, but the 60"x120" vacuum bed allows some really long run time programs. With a smaller bed you likely can stay air cooled. Dust control is another issue. You're not only putting wood dust in the air. There are preservatives, sometimes formaldehyde, and glues that are better not ingested and breathed in. The best solution is to take it from the vacuum shoe outside, but you can do well with a good shop vac with an added filter on the exhaust. I stuck mine through the wall into a utility room next door.

Use M commands to turn it on any time your spindle is running as a best practice. Probably the easiest to use is M8 which usually is used for flood coolant. So any time you use an M3 (spindle on clockwise) or M4 (spindle on counterclockwise), you use M8. Turn it off when you turn the spindle off with M5 spindle off and M9 all coolant off. It's easy to add the relay boards if you don't have them already. Mach3 also lets you manually start and stop with a simple screen edit.

[626Pilot]

The Probotix control box has a dedicated relay for that, and I can toggle it from EMC2. I have a Dust Deputy vortex dust collector. How do you suspend the vacuum hose?

[geneb]

The way I've seen it done on most machines is the vac hose is run along the same path as the e-chain on the Y carriage.

My ShopBot uses a long bit of 1/4" acrylic bent in an arch and all the wiring & 4" vacuum hose are attached to it. That will change (hopefully this summer) when I'm able to buy the hardened rail upgrade for the machine. I'm going to use 2-1/2" vaccum hose as a poor man's e-chain.

g.

[626Pilot]

I think I will use this for dust collection: http://www.amazon.com/gp/product/B0035Y ... UTF8&psc=1

I got one of them for my table saw. You turn on the saw, it senses it and turns on the vacuum for you.