Engraving Tools: Speeds, Feeds, and Tips! | WW237

hi folks having really good looking really crisp and gravy can be a really nice touch for either product or job shop work let's take a look at four different engraving tools including speeds and feeds and Tips & Tricks welcome to the Wednesday widget [Music] decking off our piece of material with the superfly and then picking up our zero with the himer I do recommend double-checking your hi MERS overall length as well as being very meticulous when you check your tool lengths because thousands of an inch to matter with engraving we're starting with my favorite the lakeshore car by 20 degree engraver it's the tool that we use for our fixture plates as well as general engraving around the shop and we've been really happy with the performance and life of the tool this particular version has a twenty thousand seven inch ball and they make it in a ten twenty thirty and sixty two ball our preference is the twenty and we buy it as a double-ended tool for twenty three dollars which actually makes it a very competitively priced tool in my opinion we're using the trace tool path in fusion 360 despite being in the 2d menu trace can actually engrave along a three axis surface that has varying Z height running it on the 770 at ten thousand rpms one thousandth of an inch feed per tooth it is a two feet tool that puts us at twenty inches a minute and under the passes tab axial offset we're taking a two thousand seven inch depth of cut next up kind of an old machinist secret which is to use something you might have already laying around a high speed steel center drill this is a number one center drill again they're really comment they're pretty inexpensive you could buy a brand new one from McMaster for under six bucks or the Amazon probably Chinese special five of them for seven bucks I would suspect some of the ones that we've had around our shop are the import version we haven't noticed a problem with them whatsoever we rarely use high speed steel these days instead preferring carbide in this case I don't need the stiffness that comes with carbide and a lot of times I don't need the longevity of the tool life or edge life so there isn't a drawback exact same feeds and speeds as the lakeshore tool ten K at twenty inches a minute mm cut and as you can see it does a really nice job with the engraving where I would definitely consider using this tool is if you've got a piece of mystery metal you're not sure what it is and you don't want risk chipping or breaking a more expensive carbide version give it a test with the high speed steel next up 360 force ball end mil until we found the lakeshore tool this was my favorite way to engrave we're using a 2 flute version here single-ended for 10 bucks they make a for flute version as well which will let you go twice as fast and maintain the same chip load per tooth for only a few bucks more the biggest drawback to this tool is just that it's a larger diameter end the 360 force is over twice as large and that matters when you're trying to engrave things that are quite small or even small features on larger engravings with a 1/8 inch shank we have to use an ER collet and when you're looking to maximize tool life as well as get a good engraving you're going to want to check that tools run out again same recipe 10 K 20 inches a minute if you had the forefeet version you should have no problem stepping that up to 40 inches a minute blast the oddball in the group the tormach diamond at drag engraver I love this tool it has some drawbacks but number one you can go incredibly fast with it and number two it lasts forever third benefit is that when you're engraving materials like aluminum the way it cuts really causes that aluminum to pop even more so if you're engraving after the part has been powder-coated or anodized the fourth benefit to this tool is the spring-loaded nature of that tip means it's relatively immune to Z variations in your part height as a quick demo I faced off this piece of scrap aluminum and then put paper between the parallel and the workpiece on the left edge most printer paper or notepad paper or somewhere between three and four thousandths of an inch thick now the face that part is no longer a perpendicular to our spindle as we go from right to left and graving gets deeper because of the angle in that part and it's very noticeable whereas the diamond drag tool is able to float to the surface there's one other way to solve this problem which is a spring-loaded engraving tool I actually used to own this one from 2l ink we couldn't get it dialed in but that was quite a few years ago and I've learned quite a few things about machining since then so I almost wonder if it would be worth giving a try again the spring action allows it to accommodate variations in the Z face or height but according to their fees and speeds your feed rates will double if not triple when you move a rigid tool over to a spring-loaded holder two big drawbacks number one it raises a burr I prefer to machine that burrow way just deck your part off with the superfly bust a half a thousandth of an inch above your part this obviously requires that your part be perfectly flat for that to work though tumbling your part sanding or scotch-brite can also knock that burr off but the downside there is you're affecting the finish of the whole part not just removing the burr the second drawback the tool does have a small amount of run-out or radial slot it's only an issue for really fine details but nevertheless noteworthy the way we program it again a trace tool path the axial offset here of ten thousandths of an inch causes that tool to be compressed we measure it the same way we measure any other tool on our tormach setup where we bring it over to a granite block and just bring that height gauge down to touch the top of the tool you don't need to compress it it's also worth noting I am neither a gunsmith nor an attorney but I don't believe this tool does ATF compliant engraving in terms of the required depth speeds and feeds totally different fusion now supports zero rpms as a spindle speed which is great you do get a warning but we're okay with that and I'm running this at 100 inches a minute you're effectively not limited though and that's a big difference if you've got a lot of engraving to do yes you're probably gonna want to come back again with the face mill to clean off the top of the part to knock that burr down but you're able to move multiple times faster with this tool if you have to engrave deeper I would recommend starting with shallower depths of cut keep them to two or three thousand seven inch of max then as you build confidence in that tool you can start to experiment with perhaps taking it all in one pass I've also found that even solid carbide tools can start raising a bird especially as they start to doll out you want to squeeze one last run out of that tool before you replace it you can either run a spring pass with the same tool sometimes that will knock it off or you can use your graving tools in a roughing and finishing strategy use that slightly older tool to quote-unquote rough out the engraving bring back the sharper one just to finish up the last little bit here's a close up of those for the top left with the 20 degree lakeshore and the top right with the high speed steel center drill almost indistinguishable the ball envel on the bottom left looks a little bit rough and the scoring on the aluminum one looks totally different but keep in mind we're zoomed in quite a bit here which really highlights the look of those features one tool I wouldn't recommend is a mill drill I used to love these tools but I found that it's just so easy to break the tip they seem to be more fragile than the four tools we just showed in this video because once you break that tip off the Z height of that tool isn't going to measure correctly so if you try to use that tool to do say chamfers your chamfer Heights most likely going to be wrong you could compensate for this by using a tool preset or an optical comparator to find out how much of the tip you broke off but that's a pain and I just don't recommend that for engraving or even spot drilling one last tip folks just because you're working with small tools or small numbers on things like feed rates doesn't make changes less significant in other words if you're cutting in a slow feed rate and you increase that maybe say from 4/10 to 6/10 of an inch feed per tooth that's still a relatively large increase as a percentage so keep that in mind otherwise well hope you learn something hope you enjoyed take care see you soon [Music] you [Music]

Channel: NYC CNC

Views: 71,550

Keywords: tormach, fusion 360, how to, cnc, machine shop, nyc cnc, DIY, machining, milling, CAD, cnc machining, cnc milling, engraving, lakeshore carbide, tools, end mill, speeds, feeds, tips, tricks, education, diamond drag, high speed center drill, ball end mill, 0 rpm

Id: 4Le6AxorcZI

Length: 8min 36sec (516 seconds)

Published: Wed Feb 13 2019