Datron Programming Guide

My guidelines and examples for programming a Datron style high speed gantry mill.

Disclaimer: This is Fusion focused but if you're in an integrated CAD/CAM environment this will transfer more directly. I used a similar methodology within SolidWorks and CAMWorks for 2.5 years. In an environment with separate CAD/CAM programs most of the fundamental concepts still apply. Get stuff sorted out, make templates, and make use of a few specific programming methods and you'll have success on a Datron.

Part 1. Collect your fecal matter in one place.

• Create a tool library that works for you. Not "works for you". A good tool library will help you make more money. Make it WORK for you.
  • Every tool needs a concise description, a manufacturer, and sourcing information. Fusion makes this easy. It's the first tab of the tool's page.
  • Accurate geometry. If the manufacturer is European you've got it easy mode, you just don't know it yet. Euro manufacturers use standard methods of communicating info about tools. Eventually you'll start to pick up on it and you'll get brainwashed and love it. American and Asian manufacturers are a bit less standardized so you might need to get out your calipers. When in doubt use whole numbers and round down for flute and shoulder lengths and add more stick-out than you think you'll get away with.
  • Every tool get's a holder. Three axis guys don't think this is necessary for them. It is. In my experience like 30% of getting to reliable first runs with no edits or pucker moments is to have accurate tool assemblies in CAM. Emphasis on ASSEMBLIES.
  • Cutting data. Keep it simple and easy to understand. The formula for naming your presets is "Material - Operation". You have 8 or 9 operations. If you don't use pocket roughing regularly for roughing you can skip that and just manually edit parameters from Flat Finishing. Only drills, taps, thread-mills, and reamers, get the appropriate presets.
    1. Material - Flat Finishing
    2. Material - HEM Roughing
    3. Material - Traditional Roughing
    4. Material - Wall Finishing
    5. Material - Helix Boring
    6. Material - Surfacing
    7. Material - Drilling
    8. Material - Reaming
    9. Material - Threading
  • Post Info. These are usually just your offset numbers. This seems like the dumbest area to explain but actually I do have two pieces of really clever advice for this.
    • If your machine uses arbitrary names use the numbers to separate tools by type. So 0000-0999 can be end mills and 1000-1999 can be ball mills. This makes sorting through your library a little easier. This is really applicable for Datron and Heidenhain users.
    • If your machine does not allow arbitrary tool names then only the second piece of advise applies. Have TWO tool libraries per machine. One for your standards and one for "flex" tools. Say you're running a Fanuc control with 40 tools, have 1-20 be standards that live in machine and will be numbered as such in the library. That is one library in CAM. Tools 21-40 will be your flex tools where you can have conflicting numbers in CAM because you're going to swap them in and out in the machine. Things like drills and reamer sets usually live in this second library for me, usually one number apart.
• Create a basic work-holding library.
  • If you're a Fusion user you DO NOT need to go all Phil Mestenhauser on this. Watch his talk for sure. Understand the container method for sure. But please realize that those guys are working at a level that is by necessity incredibly silly and over the top.
  • If you're on a Datron, start by making a dummy vacuum plate with a bunch of holes or sketch points that represent the center of the vacuum zones. Those will be anchor points for your setups. You'll be able to snap a joint to them or pick them as translation points nice and easy. You will use this in your capital "S" Setup as the fixture. This will give you a nice forewarning if you messed up a feature depth and milled through your vacuum table.
  • For your vise work take whatever vise you like using, get the CAD, simplify it as much as you like, and joint/mate that thing up to work like a vise. Make sure you have a couple Joint Origins or Mate References or what-ever you CAM system uses on the jaws to let you quickly joint up your stock and part.
• I lied. You need to make a container.
  • So I said you don't need to go to the lengths that the A Team goes to. Those people need that to be as fast as they are. You just need to get faster, period. So a basic container is a huge step in the right direction. You also don't need to go to the lengths that I have gone where I have toolpaths baked into my container that let me program the stupid simple blocks with holes in like 2 minutes. You just need something that eliminates the hassle of going through the process of creating your capital "S" Setups inside the manufacturing workspace.
  • So start by making that new file, creating the Part container component, an OP10 fixture component, and OP20 fixture component, and a Stock component.
  • I like to joint/mate the stock component to the origin of the part container component and raise it up .25mm. That bakes in my facing stock into the template.
    • The stock model itself is going to be driven off of parameters. This does make things a lot faster and easier.
  • I then bring in my work-holding and joint it to the stock for OP10 and the part container for OP20.
    • This is where the hackjob container doesn't work as slick as the "Full Phil" but it still makes you a lot faster. If you need to swap out these workholding components to create a part that used vacuum for op 10 and vise for op20 there is an annoying amount of manual repair of joints to do. It is not a lot, but any amount of reworking we have to do to get trustworthy simulation is annoying.
  • For the OP20 work-holding you might need to re-mate it each time, unless you're using something like a vacuum plate. In that case you can just mate it to the part container origin and it'll usually work for every setup.
    • You Can go into the vise model and drive joints by parameters and then joint it to the origin of the part container and it will often work for square block parts. That's what I do. Not necessary for a very basic container though. But also not too difficult so I find it worthwhile. Especially because it's task you do once that pays back in time saved very quickly if you know your way around your CAD/CAM environment.
  • Now when you bring in your part you can just move it to have it's top face at the origin of the part container component and it'll automagically have the facing stock set and be in the middle of your stock.
    • This is often good enough for most vaguely rectangular parts that were drawn by at least a somewhat competent designer. This is often not the case so you can futz around with where you snap the joint to or offset it this way and that to get it centered. Or just add excess stock to the sides and let you're automatically generated 3D roughing toolpath take care of it if need be. Remember, if you're running a Datron you are a prototype machinist, getting the part running is more important than getting it running optimally.
  • From there you can adjust your stock parameters and move into the manufacturing space.
    • If you're in a CAD/CAM environment where these are separate programs most everything you've done up to this point has happened in your CAD program, probably in an assembly, and you should be able to transfer the entire assembly over to your CAM program just by opening or importing the native assembly file. I know this works with most CAD programs and MasterCAM. The Esprit family can actually do some very cool things with importing features form the most popular CAD programs. Edge CAM, HyperMill, Tebis, etc. All the big players can do this. If your CAM system CAN'T do this. You need to get a more modern and powerful CAM program.
  • In the manufacturing workspace we just need to define an OP10 and OP20 setup using the part container, stock container, and fixture containers in the setup parameters.
    • I also like to setup my WCS at this time in a consistent spot. For vacuum work that the bottom of the stock in op10 and bottom of part in op20. For vise it's a corner of the fixed jaw in both op10 and op20, but I have probing built into my templates for 3 axis vise work.
  • Save the file. Congrats you have a very basic Container based template. It's got part, stock, and some basic work-holding defined. From here you can go crazy adding in templated tool paths. BUT I strongly encourage you to just build out good "right click templates". Especially threaded holes, precise helix boring based on tool diameter, and a ramping or "waterjet" or "router" style tool path with roughing and finishing.

Congrats. If you followed along to this so far you're about one third of the way to stealing my job as a high speed gantry milling specialist.

Part 2. It's a light machine so you need to machine things slow... LOL JK you can fucking send that things at Mach stupid. Here's how...

• S&F. Start by forgetting what you hear about feeds and speeds on YouTube from fake Texans. We DO NOT power mill or full slot with our ultra high speed spindles. We peel material off in small bites but we make up for that by taking a LOT of bites. So program with lighter feeds and faster speeds. Usually I'm running above 30k RPM. With a 6mm tool that's over 500 SM/m. Which is FAST. And with a proper single flute tool from the likes of Datron or Hoffmann Group, I usually take a .12mm to .14mm feed per tooth with that 6mm tool. Plug all that into the F&S formulas and you're looking at running that tool at over 4 Meters per minute feed rate. If you don't hate the sound you can even get away with those feeds and speeds on a high quality 2 flute and go even faster. You just sacrifice ramping capabilities with more flutes. Make sure your tools are either inherently balanced or specially designed for balance at these high RPMs. It is far too easy to damage your spindle by running a tool with poor balance.
• Tool Choice. Single flutes and 2 flute tooling give you the best chip evacuation on a machine like a Datron and you NEED that chip evacuation. You don't have torque for large drills so you're doing a lot a helix boring. No coolant to flush chips out of pockets, so the chips have to get out from the pocket by the flutes and the air blast. And to go fast you need to have a massive chip gullet to let you take a large bite with each flute. So don't really go over 2 flutes and really I recommend a super high quality, balanced single flute. You're single flute options really are Datron 4-in-1 tools for anything 3mm and up, Hoffmann Group Garant Master Alu single flutes, and Datron standard single flutes for tools smaller than 3mm. For 2 flutes I recommend again, Datron tools, Garant Master Alu, and Fraisa Tools. When we start talking about micro your options get weird and niche, but if you're doing micro on these machines you don't need me to tell you how to pick tools.
  • Be warned! I need to repeat. More than one flute sacrifices ramping abilities on these machines. I DO NOT CARE what your Ghuring rep told you. Just because they can take a Diver series end mill in a milling chuck and ramp into a pocket in 1018 steel on a 4020 VMC does not mean you can attempt a similar thing in aluminum on a high speed gantry mill. You DO NOT have the torque, you DO NOT have the rigidity, you DO NOT have the lubrication of coolant. We need to rely on the tool geometry to do a lot of the work of clearing chips. So stick to single flutes and 2 flutes. We will talk about the one exception in a minute.
  • A Tangent About Datron 4-in-1 Tools Skip the 006880(x)E and 006880(x)L unless you Really Really need it. Also skip the 006880(x)A because the K will take the same speeds and feeds and give you a somewhat practical flute lenght.
• DOC and WOC. Radial chip thinning is your best friend. The numbers I mentioned earlier are mostly taking that into account. Really they are compromises between traditional pocketing with about a 40% WOC and high efficiency milling with probably a 10% width of cut. Knowing that we can crank it up just a tad bit more than the book recommends. So you can use radial chip thinning and a 2xD or greater depth of cut to really peel material off when roughing an outer profile or an open pocket. For closed pockets I tend to keep it under 2xD for my depth of cut unless I'm using a multi-flute, but again, we'll talk about that later.
  • Speaking of the book. If you are running a high speed gantry mill get your hands on the DATRON HIGH SPEED CUTTING GUIDE. It is on their website as a free download. It has F&S recommendations for their most common and popular tools. Take those recommendations and apply them to the closest Hoffmann Group Master Alu single flutes and you'll get fine results unless you're running a finish pass. If you're running a finish pass take those numbers and halve EVERYTHING. Surface speed and chip load. That applies to Datron 4-in-1 tools as well. Trust me on that one. If you are a smart cookie or have a lot of free time you can extrapolate out their ratios and turn those into a formula to use in your speeds and feeds presets, but that's a lot of work that I don't bother doing.
• Time to talk about multi-flute tools and why they ROCK. They chip pack super easily when ramping. They don't clear chips as well in tight pockets. They can't take as big of a chip when high efficiency milling. If they have variable flute pitch they tend to get a weird harmonic which can hurt finishes (and maybe your spindle?). Overall they are kind of a pain in the ass to get running reliably on a high speed gantry mill without coolant. Maybe if you run a really slipery straight vegetable oil based MQL you could get better results because of the added lubricity. But for ethanol mist or a light weight emulsified oil MQL system they don't really work great. However there is ONE WONDERFUL exception. Three+ flute bull nose end mills. Or hog nose if you're running CAMWorks for some reason. Corner radiused end mills if you're a pedant. A bull nose end mill with a large radius to diameter ratio can be one of your BEST friends on a high speed gantry mill. Think of it as your high feed mill. My go to sizes are 6mm with a 1mm radius and a 4mm with a .5mm radius. With the 6mm tool I take a .2mm - .24mm feed per tooth at 36k RPM. Being a 3 flute tool that gets me 21,600 mm/min or 21.6 METERS per minute. Essentially maxed machine feed rates with maxed accelerations and the machine can't keep up with the programmed feed rate. It's acceleration limited. On a giant 4020 or a fixed bridge mill that's scary. The machine will try to dance around the shop floor. On a super fast gantry mill where the moving mass is super light, it's quiet and drama free. What you sacrifice though is DOC. It's pretty miniscule. 80% of the radius is what I use up to 1mm DOC. So a 2mm radius? I cap it at 1mm DOC. 1mm radius? .8mm DOC. Dang the depth of cut is tiny... What about the WOC? Well funny you should ask. That goes way up compared to HEM with a single flute. We are more rigid now since we've got more carbide, and we're not using as much torque to cut so we can REALLY increase that step over. Instead of 5% WOC for HEM I use 60% WOC for high feed milling. This really isn't any special recipe, it's just applying it to a machine that doesn't normally get to use high feed mills. What is special on a Datron is that sometimes you're cutting some really thin parts on vacuum and they want to chatter on the floor finish. This pushes the part into the vacuum chuck instead of lifting it off and really helps get a better floor finish.
  • So to sum up. A 6mm with R1mm tool can take up to a .2mm Feed per Tooth pretty easily with a .8mm DOC and 3.6mm WOC. You will probably need to dial it back just to make sure your machine doesn't dance around to much.
  • A 4mm with R.5mm can do .16mm Feed per Tooth with .4mm DOC and 2.4mm WOC.
  • Note: you can go wider, I just find that floor finish suffers when I go with a wider step over. Since I'm using a traditional pocketing operation I tend to go straight to my finish pass with these tools whenever possible.

Part 4. Drilling is scary and you should do it on your Datron.

• If it's scary why should I do it? Cause it's faster and more reliable then helix boring with tiny end mills. Also makes your thread milling more reliable. With the 3.3 kW GMN spindle on an M8 Cube you can go up to a 6.6mm drill in 4140 steel if you're careful. At least I have. In aluminum I regularly use a 6mm drill down to a 1.0mm drill. It saves me a lot of time and reduces the number of crazy aspect ratio tiny milling tools I need to stock.
• Okay... but HOW? Pretty simple. Forget that you're using a high speed gantry mill and pretend you're using a super dinky benchtop drill press that happens to have the ability to retract out of a hole at 20 meters per minute. In less obtuse terms I use the recommended cutting speed for the drill which will almost certainly be less than 20k RPM. And then I use the recommended chip load for tools up to about 4mm, over 4mm I usually halve the chip load. BUT the secret sauce it to use pecking. At most I use 1xD pecks. For really small drills I'll use .5xD. When pushing "larger" drills, say 5.5mm to 8mm you NEED to pilot with a drill that is at least the web diameter. If you don't know what that means I suggest watching a This Old Tony video on drill sharpening. That'll explain what I'm talking about.
• Got it. But what tools actually work? OSG Ex-Sus-GDS screw machine length drills. EDP numbers usually start with 615xx. The "xx" is usually the diameter. So a 5.5mm drill is a 61555, a 4.2mm 61542, etc etc. They do get kinda wonky where OSG hacked in more EDP numbers into the range but for the most part you can find the drill you need with the formula "615"+"drill diameter with no decimal point". That's great for drills between about 2mm and say 8mm. For anything ~2mm and smaller use M.A. Ford PCB drills. these are the 302 series. Most commonly you'll find these on McMaster-Carr as "quick change shank drills". They all use an 1/8" shank and have roughly the same overall length for use in PCB routing machines. Both of these tools work great on a Datron and are cheap.
• Things to note: Avoid carbide drills larger than say 3mm, avoid 3 flute drills, avoid any coating that has an Al in the abbreviation when machining aluminum, and avoid reduced shank drills. In you are on a Neo with the 2 kw spindle you really probably don't want to push a drill any bigger than 5mm. Over 5mm the 3.3 kW M8 spindle starts to bog down a bit as the holes get deeper so you definitely don't have as much head room. If you're using the drill I recommend you don't really need to spot with the HSK spindle if you're using the Schunk Tribos holders that Datron distributes. If you're using some other holders they better have as good of runout or better than the Tribos or you might need to spot. No clue what the runout on the Neo spindle is but I'd imagine it's pretty damn good if you're careful about cleaning tool shanks and adapter collets. Maybe shoot me a message on Instagram and let me know how that goes.
• The full retract pecking is important because drills require more torque the deeper they go. That's for 2 big reasons 1) there is more margin in contact with the hole causing friction and 2) the chips are filling the flutes and trying to stick back to the material... causing more friction. So by using full retract pecking with a minimal pecking depth we minimize the friction build up and thusly minimize the torque required to drill the hole.

Part 5. Finishes are Fickle. Here's my advice.

• Make sure you're not recutting. This is basic advice for good finishes on any machine, but since we don't have good coolant flushing to help, we need to be strategic about how we finish surfaces. For really deep pockets I'll run a semi-finish pass as a super steep ramp. Go 30 degrees and ramp down the wall leaving .05mm on the wall just to kinda of plow the chips out of the pocket. Then come in and take that .05mm off. When ramping a part out I'll just do two finish passes offset by .05-.1mm to do the same thing. Plow the chips out of the way.
• Slow that Shit Down. Just halve your surface speed for finishing to start. If you also halve your chip load you'll give the air blast time to get chips out of the way. Cutting back on your speeds and feeds for a finish pass is a well known trick and it still applies here. If your tools are dull this will not help you. Dull tools will just create a smeared mess. So keep your tools in good condition and change them when they start to dull. Duh.

FIN.

That is what I have for now. Watch this space for examples and more up to date information on how to eek the most out of uncommon machines.