How did Wendell make that CNC Machine?

As a preface, I work as CNC programmer and IT admin... so naturally, backwater jury-rigged CNC machines intrigue me... 

I'm very curious how he wired that mill to run CNC... what code it uses (FANUC g-code, I assume?)... and a general blueprint of how to make one, what programs he uses to run it, what table size he has, the accuracy of the mill itself, how much he has invested in that project, and if he's ever tried 3D contouring with it...

I don't know what level of machining experience Wendell has, but it's impressive (and adorable, it's so tiny and cute :) that he made his own CNC machine...

If he hasn't ever tried 3D contouring, I'd be willing to send him a small ballnose and a generic program just to see if it's capable assuming it can accept a FANUC post... I think it'd be awesome to have something to that can sling chips in basement... wanted to get a general idea of what all it would entail...

I am in, I would love to see Wendell's CNC setup.

This is pretty much my exact setup: https://www.youtube.com/watch?v=a37Gqjg6GgA

It's a cheap chinese cast iron mill that, with some love, can actually be pretty decent. I replaced the lead screws and put in antibacklash whatnots as the first order of business.

 

Just off-hand, looking at the feed rates it doesn't look to be capable of surface milling, but it's still kind of awesome...

Would it accept Haas FANUC G-Code?

What's the max RPM / IPM on that thing?

What's the maximum table size?

What tools do you have? and in what material?

Might get bored one day and write you guys a program for a Tek Syndicate sign out of aluminum or something... looks like it could handle 3 axis fairly well... but without the specs it'd just alarm out... it's cool though...

Man those step motors are a lot less expensive than I thought they would be.

How was the backlash on the screws of the HF mill, did it just need some adjustment?

I doubt it would accept fanuc g-code unmodified, but I can probably get pretty close. 2000 rpm and Very Slow IPM when milling, but I can do a pretty zippy 100+ ipm jogging :) the hardest material I feel comfortable milling is aluminum (with compressed air cooling). Mostly the blown foam plastic for robot parts (sometimes you see this as "fake wood" in hobby shops. It's pretty rigid). It's a tabletop mill, so the milling area is approx 5.5 x 11 x 8 or 9 inches depending on how I've got it setup.

I have various two and four flute endmill sizes from 1/8th up through 1 inch. Mostly carbide or high speed steel. 

I milled the parts necessary for CNC conversion on the mill itself (lulz) and, since I don't have a lathe, milled some parts to make a jig to turn an old craftsman drillpress into a lathe to cut the few parts I needed to turn to complete the cnc bits. 

I keep the speeds and feeds pretty low to be easy on the steppers/regulators and to go easy on the endmills, especially when I'm cutting out of metal. 

I have all the parts for a 4x8 XY router table type setup but I never have gotten around to building it and milling the last few parts I would need to mount a rotozip or laser or whatever on the cutting head. That would be a toohed belt driven xy table, so not super accurate but good enough for government work.

I have done some surface milling for finishing before on small aluminum parts, and for some widgets that had tight fit tolerances that worked fine. 

I don't have any fancy bits like t slot bits or gear cutters or anything like that. I do have a 4th stepper I could make a rotary table for the mill for aluminum gear gutting.. I am ready to do that but a need hasn't popped up vs/avis just ordering gears or toothed pulleys for what I need. 

Well... I generally program with Mastercam with a HAAS post-script... I know general FANUC code off the top of my head but surface machining would be impossible off the top of anybody's head

I know you're a math guy, but still... :P

So, what do you use to post? if you have a .pst file that'll run it, send it to me...

I kind of didn't expect you to have carbide available given the budget, but that's awesome! I do realize the rigidity of the setup is likely terrible and really you do what can there... but you should be aware that a lot of people think running things slowly is safe for the cutter... in reality, however, it just burns up the relief if you don't run the chip load that a cutter is designed for... let's say you're milling Aluminum (which is really, really soft and CNC can run the hell out of on a rigid machine, which you don't have obviously)... recommended chip load on a Hanita carbide 3-flute 1/2" cutter is around .005 per flute... which is really just vender-based bullshit optimal conditions (LOC and DOC being optimal in and a high-speed toolpath taking full depth cuts at nominal steps)

So, from personal experience in a mainly proto-typing shop, on a belt driven Haas VF2 that doesn't have much torque, we generally order 3-flutes at a 2.5x diameter LOC so we can use them for pretty much anything... the Hanita Varimill cutters are rated at .0018 chip load with a 4-fluted cutter on 1018... it runs well, if not a bit slow at that rate, and doesn't burn up the cutter unnecessarily. So, adjusted for aluminum, it's about a .003 chipload to be "safe" at a SFM of 1000... 1000 SFM on a 1/2" cutter would be 7640 RPM... which you can't run given your max RPM... your max SFM on a 1/2" cutter would be ~261 which, with the same chip load puts it at ~9.6 IPM... which is REALLY slow on aluminum, so you're doing yourself a solid there... the real question is how you could increase the RPM... 

So you have a 4th Axis? Man... the things I could do with A axis + FANUC G-code :(

SEND ME YOUR POST FILE!

I assume you know all the SFM/chip load formulas? Would a table of suggested chip loads be of any use to you? Obviously it's based on specific cutter geometry and material and whatnot, but it'd give you a basis to go off... I've also got an excel table of materials and projected SFM at work (though it doesn't go below Delrin, it does include 6061 and Brass)...

As a side note... Pretty sure you could machine 12L14 on that without any trouble on that mill... as it runs almost the same speeds at aluminum... and 360 brass would be doable should the need ever arise... 

Also, I would consider something like this: http://www.travers.com/85-500-006?Category=UserSearch=85-500-006&gclid=CjwKEAiAv7ajBRCIldS7rp7wzFkSJAAA1n4DPcBs2IJptQKi44KkDsabVOMA9FegZX8_Qt78Pd6xexoCBSjw_wcB

research the price, and they make a mess of sticky coolant everywhere, but you could definetely expand your machinable materials with that...

If you have any specific questions regarding machining, I'm not an all-knowing God of machining, but I do a lot of G-code programming and have for several years as well as working for several years as a machinist... if you want all the SFM/IPM/Chip load formulas I'd be happy to give you those as well...

How did you post a surfacing program? If you didn't do it using CAM it's fucking amazing the patience you have... I literally can't imagine how long that would take and I was an engineering major :P

Lol this is awesome. I am not a fancy machinist. More later but for now I use an ancient copy of AutoCAD I picked up from a surplus auction with some autolisp routines I wrote for things like pocket cuts and surface milling. Mostly I just draw what I need on paper punch in the coordinates then export as dxf. Emc on Linux converts to a toolpath and gcode. I think its AutoCAD 12 or 14 or something like that. 

Openscad I have messed with and think it will work for CNC much the same way. It works great with the 3d printer because I can program a script to draw a gear and this was too hard with autolisp. 

Oh and mostly I use teeny cutters. Dremel bits even. I have an autolisp routine that masks a trace from eaglecad so I can mill PCB circuits. For that I use a carbide bit meant for a dremel. Works great. Two sided pcbs are cake. 

My carbide bits are cheap Chinese crap from eBay. Lol. 

 

Ahhh... well you should be aware that all carbide is certainly not created equally :) ... we've tried all kinds of different endmills and Hanita just trumps everything. The cool thing is if you don't do stupid things with your machine and just mill aluminum or softer materials, you'll never need to buy but one endmill per diameter.

http://www.ebay.com/itm/HANITA-TR-4C43-1-2-3-Flute-Carbide-TiAlN-0-03-Corner-Radius-End-Mill-H20/121232809304?_trksid=p2054897.c100204.m3164&_trkparms=aid%3D222007%26algo%3DSIC.MBE%26ao%3D1%26asc%3D20140407115239%26meid%3Df19ea6613e2e4dca883202a3d2b9fafc%26pid%3D100204%26prg%3D20140407115239%26rk%3D7%26rkt%3D30%26sd%3D281502190095

That's a good example of what I use for Aluminum... we use a longer length of cut (LOC) because they serve as multi-purpose end mills and don't chatter too bad at 2.5x diameter (for example, a 1/2" would have 1.25" LOC), but that's a very good price for it and I doubt you'd need much more than that for that mill... if you're finishing, and the endmill is on size (hasn't been reground), you can step down the finish passes by the LOC and still get a clean finish... I don't know the sizes of stuff you generally machine, but 2 or 3-flute carbide is great for non-ferrous metals... I prefer a SHARP 2-flute HSS endmill for plastics...

I realize the prices of software are absolutely stupid, and I haven't tried any Linux versions of CAD/CAM, but we generally design in Solidworks and export a parasolid to Mastercam. The parasolid comes in Mastercam with the geometry traced and a solid model. I like to separate the geometry and solid into two layers and use a third for toolpath lines. from there, you just trace your toolpath lines from the geometry and create toolpaths (which keeps you from bastardizing the model).

For surfacing, you can rough/finish in 3D with the 3D toolpaths, It will ask for a drive and check surface. The drive surface is what you want to machine, and the check surface is used when you don't want a cutter to hit a wall or something in the way. If the toolpath insists on going out of your boundary, you can trace a containment line around your drive surfaces. For most applications you can use 3D parallel for flat surfaces (which steps over gradually and traces your surface in YZ axis) and 3D contour for steep surfaces (which steps up or down gradually and traces the surface on XY axis)... note that turning on create curves in all axis in your tolerance menu will greatly shorten the G-code, as otherwise it plots it in tiny XYZ increments.

For surface machining, you have to remember that the bigger the tool, the bigger the step you can take and create the same scallop height (the distance between the crests of the ballnose). So while a 1/2" ballnose can take .014 steps and still leave an easily sanded finish, a 1/8" ballnose would require a .0035 for the same finish... but you were likely well aware of this...

A couple programs that are nice to have handy that automatically calculate speeds/feeds:

http://www.cimco.com/download_registration.php3?area=1&id=20&prodname=CIMCO_Feed_and_Speed_-_Freeware

http://www.emastercam.com/board/files/file/777-chip-thinning-calculator-for-windows/

 The chip thinning calculator is for high-speed toolpaths or very light depths of cut... since your endmill isn't engaged much in the part, your speeds and feeds can increase sometimes astronomically... otherwise you're basically just burning up the edge on the cutter or producing alot of unnecessary heat on the part...

Of course, you'll always be limited by your 2000 RPM, but those give you a more mathematical option to calculating speeds and feeds other than "I'm gonna go turtle" :P

If you're using teeny cutters you'll just plug in 2000 RPM automatically and figure out a chip load that works...

Off the top of my head, in standard 1018 (cold rolled steel)... 1/8" should handle a .0008 chipload, 1/4" - .0012, 1/2" - .0018, 3/4" - .0024... those are conservative enough for overnight production runs. your Surface Footage a Minute (SFM) for Aluminum on that mill SHOULD be around 600 (keep in mind you can run it up to 5000 SFM with the right setup/cutter/machine), but small cutters will want more RPM... calculate off the average diameter in contact with the dremel bits... you can certainly ramp up your chipload from a conservative 1018 standard on plastics and aluminum, but it's all depending on what tool you're using and the rigidity of your setup.

But yea, most plastic runs better with air cooling unless you're running some obscene SFM which can melt the plastic while it's cutting... Aluminum, however, tends to gawd up a cutter without coolant. if you ever get ahold of brass, it machines like butter, but beware of the chips... they're the herpes of machining... it's like fucking glitter man :)

Typical SFM for Carbide/HSS in our shop

1018: 400/80

Aluminum: 1000/200

Delrin: 2000/400

Nylon: 1250/250 (namely cause it's spongy and you can't hold on to it without it flexing in)

UHMW: 1250/250 (see Nylon for why so slow)

360 Brass: 600/120

...use the HSS SFM for drills and if you're working with weird impregnated plastics, just look up the machinability in comparison with one of the aforementioned materials and calculate by percentage...

Seeing as it's just a hobby and you're not mass producing PCB circuits, I don't know if any of that was even helpful... but it is what it is... happy machining! :)