How to use Tool Length Offsets in Fusion 360 and MACH3

today we're going to talk about tool length offset in virtually every video you've seen where I make parts with my CNC mill you've also watched me swap tools in and out of the spindle with impunity without resuming the z-axis today we're going to talk about how that works I'm going to show how to set up the tool tables in fusion 360 and Mach 3 we'll look at what Mach 3 is actually doing with that information and then we'll make a sample part so stay tuned [Music] welcome back to cloud 42 I'm James this video is in response to a viewer comment terrence Kersey left a comment asking if I would do a video on tool length offset that's something I've been planning to do for a while but I hadn't gotten around to it so let's go ahead and tackle that today you know some of the videos that have been the most popular on this channel are the ones where I set up a VFD and programmed it for my lathe and I didn't see that coming those videos have generated more views than literally anything else on the channel by a longshot so let's take the same approach here walking through all the details of setting up the tool length offset sand making them work on the mill let me get the mill lubricated and booted up and let's get started I'm sure everybody's aware of how tools mount in a typical mill spindle this is an r8 spindle nose and so it uses re kaulitz to hold tools so the call it goes in the spindle and then the tool goes into collet we cinch that down and then we're ready to mill now in order to do CNC machining if I were just doing manual machining I'd bring this down I'd touch off the surface of the part and then I know where my Z height is at zero it and then I can dial this up and down and then anytime I come back later and put a different tool in here then I'll have to touch off I'll still have the X&Y on my Dro but I'll have to touch off the Z height cuz the tool can't be replaced repeatedly in the collet so if I pull this tool out if this is a certain length and I have my zero set and then I pull the tool out and then I come back with another tool and put it in there's no way to get it positioned at exactly the same Z height so anytime I swap out the tool I'm gonna have to Reiser the C even if it's literally the same tool I'm not going to be able to put it back in the same position so the solution to this when your CNC milling touching off the Z height and the surface of the part or using shims or whatever but remeasuring and Reiser ohing in the middle of a CNC program when you do a tool change is really inconvenient in fact it's generally not support it's difficult to say okay pause the program now let's move the mill to a different location get the Z zero and then put it back or put it back somewhere and trust that the program's gonna pick up and it's not going to crash into anything when it starts moving again so you really need is a way to put the tool back in exactly the same position every time now for mills that have other spindle styles like dual contact or tapered spindles you can have tool holders that hold the tool that go back in in the same position but with our eight kaulitz you can't really do that there really is no kind of stop all the call it really does is squeeze the tool there's no z stop on it and this is the purpose of the TTS tool holders that you've probably seen develop my tormach or at least sold bite or lock so there's two parts to the tormach tool holding system one is this shortened collet you can see compared to an ordinary three-quarter inch epaulet which I'll grab here you can see that on an ordinary call it there's some crown on the end but the TTS call it has been shortened and the reason for that is so that when it goes in here and draws up to you know the tight where the the position where it'll actually tighten down on a three-quarter inch shank which all the tool holders have it's actually above flush with the end of the spindle nose so the thing that sticks out the furthest is actually this face on the end of the spindle nose and then all TTS tool holders like this is one with a drill chuck holding a drill have this second register they have the three-quarter inch shank that is actually gripped by that collet but then they have this additional flat ground surface the registers directly against the end of the spindle nose and the reason they have that is so now every time I put this tool in it registers back into exactly the same position and then as the call it grips it both grips the outside in order to hold this in place and keep it from moving in this direction but because the collet is is pulling up as it grips it also sucks this ground surface against the end of the spindle nose and the result is a zero clearance fit and it sucks up to exactly the same position every time within a tenth or two at least I've done a little bit of testing with a dial indicator and as far as I can tell it sucks it up to exactly the same position every time as long as the face of your spindle nose is nice and clean so what this then allows me to do is swap tools at any time and have the new tool go into exactly the same position so if I'm done with this drill I can pull that out I can grab an end mill in this case a 3/8 inch aluminum and mill I can put that in and it will register in exactly a predictable location every single time that I put it in now this solves the issue of getting it into the same position every time this doesn't necessarily solve the issue getting all of the tools to have the same z0 because as you can see this tool comes to here this tool is much much longer and so if I hold those side by side you can see one tool is much much longer than the other and so the meal is going to have to know pretty much no matter what which tool is in there so that it knows how long it is and it can compensate but at least with these hook tool holders every time I put it in it goes to exactly the same position so I get repeatable predictable position now virtually any tool that can go in the mill can have TTS style tool holder I already showed the drill chucks and I've got multiple drilled Chuck's so I can have multiple drills sometimes they'll have a clearance drill and a tap drill both in tools so I can swap those out easily as a part of the program in Mills of course this is a this style of tool holder has an ER 20 collet in it so I've got in this case a quarter inch three flute end mill in this one I've got 3/8 inch end mill in another I've got spotting drill in this one and this will become very important later I actually have a an edge finder and a tool holder this is tool number one and we'll talk more about that in a little bit there's really no limit to what you can put in these this is a for flute carbide face mill in a TTS tool holder and this face mill Arbor is actually one that I made I just turned this out of 1144 stress proof steel and cut it in and made keys and so now I have a TTS tool holder for my face mill of course if you buy any of the tormach tools like the superfly it has the TTS tool geometry built into it so the fly cutter is of course available in that I even made a tool holder for my boring head so if I have very precise round holes I can get this all set up and then I can use this as a CNC tool to come through and bore out the center of a well like a bearing bore something that needs to be very precise and has to be very very round and again I just made this just turned this out of 1144 steel I even have a TTS style Harbor for my slitting sauce so again this is just turned out of 1144 steel I put the slitting saws in here and then once I've measured the length of this as we'll show it here in a minute I can put this into the spindle repeatedly it has that same TTS geometry so really there's there's no limit to the tools and in fact pretty much every tool that I have here I have a TTS tool holder for there are a couple of exceptions there are only a couple of tools that I generally don't want to use these forms talk about why so if I have an end mill in this case this is a 3/8 inch 3 flute carbide end mill for aluminum it has a certain length and so if I put this directly in the spindle nose then you'll have the inch inch and a half of stick out here then you're directly into the spindle nose and then the spindle bearings are above that where if I put it in a tool holder like this I've added probably an additional two inches of stick out now these are pretty rigid so I'm not too worried about the tool holder flexing but overall the spindle bearings are now up here someplace and I've added a whole bunch of extra lengths and so this is now 2 inches further away from the spindle bearings than it would have been if I just put it in the mill directly and so if I've got something where I've got a really heavy cutting load like in particular this tool which is a roughing end mill for steel this generates a lot of side load and a lot of forces and if I just do my roughing with this I'll have a set up is a separate program so I can put this directly in an r/a call it in the spindle nose and just machine with that with just an inch of stick out it's much more rigid makes a lot less noise a lot less risk of tool breakage and overall the mills a lot happier sometimes when I have something that's really heavy I will forego the additional length of the tool holder and I'll actually just go right in and re call it but when I do that I forego the opportunity to change tools in the middle of the program so this is how the tool holders work and you know having them all organized in the drawer is very very handy you can see that I generally have a piece of tape on here and I'm just right the tool numbers this is tool number one tool number two tool number 15 I started out writing these on the side of the tool holder but after a while I realized I have more tools than tool holders so for any given program I'm gonna load up the ones I want and it's much easier just to lay down a piece of masking tape so that when the tool change occurs and the call comes for a particular tool I can just look down here and I have all the ones that I'm gonna use in my particular program right at hand and I can put one back and grab the next without making mistakes because it because the tools are all different lengths you make a mistake you're gonna crash the mill or you're just gonna cut the air hopefully you cut the air because crashing the mill really sucks so that's the tool holders in order to make all this work though the tracking of the tool number starts in the cam program this is fusion 360 and I have a very simple part modeled up in here this is just a block of metal with a sketch on the surface with my logo and we're going to engrave this logo into the surface so there are three operations we're gonna face it off first then we're gonna engrave and the engraving always leaves a burr so then I want to come back with the facing tool and just shave a thigh or two off just to take that burr off so if I simulate this this is the model this is model as a face mail but I'm actually going to use the superfly so this is gonna come in take a couple passes just to smooth the surface then the next operation is the engrave and using a 90 degree tool single lip cutter to come in and actually engrave the logo and then of course since the logo leaves the burr will come back and face it off again with with the face mail I have this modified mod as a face mill because that's what you have available here in fusion 360 but in reality this is the superfly cutter that I'll be using so let's take a look at the tools easiest way to do that is just going to be going here and look at the tool library and within this particular model within this particular cam program I only have two tools I have my number 20 tool which is the chamfer mill that I'm going to be using to actually do the bee engraving and then I've got my face mill which is you know actually the TTS superfly now if you go in and edit these tools the thing that's most important is the tool has to have a number so that fusion 360 cam can put tool numbers into the g-code so it can tell Mach 3 which tool you're using so that Mach 3 can then apply the appropriate tool offset and that's done over here in the post processor tab in the post processor tab when I'm editing the tool we have the number right here NC stands for numerical control as in CNC computer numerical control and you can just edit the tool number in this case I've put in 20 if I change this you know something else you'll note that it's editing two other fields the length offset and the diameter offset now the thing that's important to remember here is this is not the actual length offset of the tool this is not the actual diameter offset of the tool in any kind of dimensional measurement this is the number of the slot in the table that should be used for this so this is tool number 20 so it'll do a call up for tool change to tool 20 and it should use the length offset that is in table slot number 20 and it should use diameter offset number 20 those are actually set in the machine tool itself in this case in Mach 3 so all you're doing in here is putting in the number so as you edit your tool library and set up your cutter setup you know the shaft and holder if you have holders and you want to model those those are mostly good so that fusion during the simulation can tell if the tool holder is gonna collide with anything got your feeds and speeds and you have to set up the tool number so this one's tool 20 if I go look at my face mail here I have that one set to tool number 28 and that's just the number that I've assigned to that tool there's nothing magical about these numbers you just make them up and you maintain your own library of how you want to track your tools now you'll note in here you have this document tool library and that's what I'm looking at here and in fact you can go down and actually manage them by setup there's only one set up in this document and then I also have my cloud libraries so I have a library of my tools set up that I use in aluminum and so when I'm adding a brand-new tool that I've never seen before that never had before rather than just putting it in here on the individual document I instead click over here to my TTS tools aluminum or TTS tool steel it's essentially the same tools in most cases but the feeds and speeds are set up different for lumen impedes and speeds versus steel speeds and feeds so what I'll do is I'll come to my aluminum here I'll click the new tool and then I'll choose the type of tool set it all up set the feeds and speeds that I want to use and then give it a number and when I hit OK it will put it here in my cloud library of aluminum TTS tools it'll also make a copy of it into the document so I can use it in this particular document but then later when I'm working on another document in the future I can come back here to my TTS tools aluminum and it will be in this table and I can pick it so here's tool 20 which is my 45 degree engraving tool or 45 degree chamfer mil which is a 90 degree included angle engraving tool and then here's 28 the superfly so when I set this document up I didn't enter those I just came and picked them out of my library and they already have the tool numbers set okay let's generate the g-code I'll just select the setup I want to use and come up here and click post-process this brings up the post process dialog now I am using all of the defaults I've selected Mach 3 mill as the post processor that I want to use because I'm generating this for a meal that's being controlled by Mach 3 and then I'm just taking all of the defaults it's possible to change things about how the retracts work whether you want to use certain G codes but I'm just taking the defaults for everything I'll click post and we'll save this 1001 that's the S the program number by default so if you go into the setup here and edit the setup itself over on the post process tab you actually set the program number and this is only really important if you're gonna have a library of them but generally if I have a bunch of setups I give each one a separate program number so it'll have a different file name though you can also edit the file name and change that ok let's take a look at the G code that it generated up here at the top there are some comments that just tell you which tools are in this file and this is really handy to look at we're using tool 20 and tool 28 which you know I already knew that but if I'm looking at this G code later trying to remember exactly what it does I can see this the other thing that's really handy at the top here to look at is the Z minimum so this is the minimum Z height at which it's going to attempt to make a cut with each one of these tools so in this case the Z minimum of T 20 which is the chamfer meal is going to go eighty nine thousandths deep below the zero point and the face mill is going to go 50 mm steep so from the point we set on the zero on the top of the part the face meal is going to take off about 50 thousandths and then the mill is going to plunge in or the chamfer mill that we're using for the engraving is going to go in about another forty thousands this is a great sanity check I can just look at this and see if anything looks weird if one of these said negative 3 inches I'd have to go back and try to figure out what I did wrong because clearly I'm about to plow a part or plow a tool down into my vise or into the meal bed so that's a good sanity check so then each of the operations has a comment followed by the code for that operation so here's the face 1 here's the engrave 1 which is a second as a bunch with the grave and then here's face 3 which is the last operation so if you look at each one of these you can see is a couple things that are interesting here t28 is the tool change call-out so this is going to tell Mach 3 to change to tool number 28 now if I had an auto tool changer that might actually cause my machine to do the tool change but I don't have a tool change or I'm going to be doing it by hand and so T 28 calls out the tool m6 tells it to execute the tool change and again in this case it's gonna be a manual tool change so what's gonna happen is it's just going to wait and then I'll change the tool and I'll hit continue and the program will continue the next thing it's interesting we've got some things here setting the spindle speed controlling coolant some other stuff here G zero is a rapid so it's going to go to these coordinates and then G 43 is the other interesting thing it's in here that tells Mach 3 that you want to use the tool offsets and so you'll note that that tool length offset call-out is right before the first z height so we tell it as tool 28 then before we go to Z any Z height we tell it G 43 which means apply the current tool length offset so it knows it's tool 28 so it's going to apply the tool length offset for tool 28 and then when it drives to this Z height of 0.6 it's going to take the tool offset into account and then you'll see exactly the same pattern if we go down and look at these others here's the engrave and there's the tool call out the tool change and then here's the G 43 again before it makes a si height move and here's the last one 2 twenty-eight tool change and then here's that g43 again before it drives to an initial Z height and then you know it continues driving around in Z after that now the important thing to remember out of all of this with the cam is that the only thing you see here is identifying which tool is in use or more importantly which tool table slot number to use for the offset the offsets are not in this file at all those offsets are managed in mock three okay now we've got the numbers in the cam program we also now have to tell Mach three the lengths of all of the tools so if I come up here and say config and pull down and select the tool table this opens up the tool table in Mach three now this has a bunch of different things down the left or all the tool numbers one through how many are there 253 tools and it gives you a place you can put in a description it doesn't do anything with the description the description is really just there as a convenience so that you can remember what it is you can see the tool number one here is my edge finder now it has diameter information that you'd use for diameter offset it's got diameter where information height information but what we care about in this case since we're only doing tool length offset is the height so in this case I have a height for tool number one my edge finder set to three point four to four inches if I scroll down a little further I have tool 20 which is my 90-degree engraving tool which we'll be using and the height that's in there is 3.0 eight three inches and a little bit further down the list I have tool number 28 the superfly and it's currently the tool height in here is one point eight seven four now of course if you mess with the tool at all you take it in out of the tool holder yet where's you know anything gets touched at all and these numbers change and you have to remesh put the number in here now a good question is where do you measure the height from right so this is superfly is one point eight seven four inches 1.8 7 4 inches from where to where and ultimately what we care about is the register on the tool so if I have this register and then I'm going to measure from that register to the tip of the actual cutting edge of the tool or in a case of an end mill it's going to be from the register to the tip of the end mill now in reality it doesn't matter as long as I'm measuring something that's consistent with the position of this register then it as long as I measure all the tools in the same way it won't matter because as long as if the tool is half an inch longer then the height in here is a half an inch longer it doesn't really matter where you measure it from as long as all the tools relative to one another are the same we'll talk about more of that in a minute so how do you measure tools let's go over to the surface plate so the way we measure the tool length is with a height gauge and this is a dial height gauge so I've got readings up the side here plus down to a thousandth of an inch with the dial now I'm using a special small surface plate made by tormach for exactly this purpose and this surface plate has a hole in it to accept the three-quarter inch shank of the tool so this is my edge finder and I can just drop it in there so now the register face of the TTS tool holder is on the surface of this surface plate so then I can put my height gauge on here and I can take a measurement of the length of the tool so this looks like I am at three point four to four inches I write that down edge finder three point four to four and it's just that simple let me grab the other tools this is the 90 degree engraving tool I'm just wiping off this register surface and wiping off a surface plate make sure it's clean drop it in there and then I can take my measurement and in this case we're looking at about 3.08 three and finally the superfly again I'm just measuring straight to the highest point here 1.90 for these furnace plates are not that expensive they're 30 or 40 dollars and I finally broke down and bought one because they're really handy and it makes this job a lot easier but you don't have to have one if all you have is a surface plate which I happen to have right here you can actually take these measurements directly on the surface plate using one two three blocks so if you take a couple of one to three blocks like this then you can set your tool so that the register is sitting on the one two three blocks and then you can come in and take your height measurements like this now one of the things you'll note if you do this is that the base of the height gauge which we're using to actually measure the tool and the register the tool are not coplanar if you were using this then you would have the height gauge sitting on the same surface that this is registering so in this case there's two inch there's a two inch difference here because these are accurately ground one two three blocks there's two ways of handle this one would be just subtract the two inches so instead of getting three point four two four on my edge finder I should be getting let's see what am I getting I am getting five point four two four which is exactly what you would expect because we've got two inches of one two three block underneath this so I could either just subtract the two inches knowing that instead of five point four to four it's actually three point four two four and I could just enter that smaller number in to mach3 but in the end it really doesn't matter because we're going to use this tool tool number one which is the edge finder to zero the Z height and zero the Dro s in Mach three and then when we switch to other tools the only thing that really matters is the difference in length between those other tools and the one that we used for zeroing so if every tool is in there with two inches longer in the tool table than it actually is that's chromatic Li suspect the way I said that but if every tool is 2 inches longer in the tool table then everything will work out and it's fine now if I were actually zeroing the mill based on the spindle nose or something you know exotic like that it would matter but as long as I'm going to zero with one tool and then switch to other tools it doesn't matter if I measure all the tools and they're all two inches too long it's fine so let's go over and put these numbers into Mach 3 and let's look at how the mill behaves when we look at Mach 3 here what we're seeing here in the Dro is the current coordinates in the current work offset system and the current work offset system is set to G 54 which is you know fixture number one we're not going to worry about that today but what's important is that what we're looking at here is not the raw machine coordinates what we're seeing here is actually the coordinates of the actual current working coordinates if I click the machine coordinates button here it shows you that the actual Machine Z is zero and that's exactly what you'd expect because the mill is all the way at the top of its travel against the limit switch because I press the ref all home button and zeroed it that way but it doesn't do me a lot of good having zero up there because I need zero to match the zero that I'm using in my in my CNC program so I'm gonna need to set that zero someplace else yet the mill still needs to know that the zero of the Machine coordinates is at the top so it can decelerate and not crash into it so me turn off the machine coordinates we're gonna work in the reference current working coordinates so I can actually zero this and now they'll match so if I go back and forth you can see it's zero on both because I have zero the z-axis in the working coordinate system now the tools right now I have tools 0 selected and this is what happens by default when you just bring up Mach 3 tool 0 is selected and it's not going to apply any kind of work offset I'm actually going to do my zeroing with tool number 1 which is the edge finder let me go put that in the mill now you I have not selected the tool yet so if you look here I have tools 0 I don't have any tools selected so the actual working Z coordinate is 0 now if I come here and I select tool number 1 1 enter you'll see that this immediately changes so now the coordinate is minus 3 point 4 2 4 and that makes sense because we that's the link that we put in the tool table for that tool is 3 point 4 to 4 inches and in fact that tool sticks down 3 point 4 to 4 inches from this face so it makes sense that if we had the 0 if we considered the actual working coordinate system 0 or in this case also the Machine 0 with it all the way up being the face of that spindle nose our Z position now we've selected tool 1 the mill thinks oh my goodness it's actually lower than that it's actually down here at minus 3 point 4 to 4 which is exactly right because we've added a tool of that length now let me run this down I have placed a ruler a six-inch scale here in the mill just so that we have a point of reference for the length so let me run this down and roughly 0 on that now this is just gonna be a visual thing we're not actually gonna machine this scale so I'm just gonna get it so that it looks about right by eye that look about right yeah that looks pretty close now I'm gonna come over here I have tool one selected that's important and now I will zero the Z height so now we go back to the machine coordinates machine corden is still minus one point three three four it's something else because we're actually one point three three four inches down from the top but in terms of the actual working coordinate system for my selected tool tool number one we're now at zero and you can see the end of the tool is right there next to the top of the scale yeah you can see that okay so now I go ahead and run this up and I lost my Z so I'm gonna have to do that again sorry about that I had a little problem with the mill and I lost the Z coordinate system because I lost some steps it's a lot colder in the shop today than the last time I tuned it and I got some lubrication issues you don't want to hear about it anyway so I'm back to the same position I was at where I have the end the edge finder in here I have tool one which is my edge finder selected and I have it zeroed right at the top of the scale so let me take the mail up and let me swap this tool out for the engraving tool okay now I've got the engraving tool in the mill let me just tell the mill to go to Z zero so G 0 Z 0 and the mill will wrap it down to G 0 now if you take a look at that that doesn't look quite zeroed because it's actually higher than the end of my scale here I went back to 0 but this tool is not as long it's actually shorter now I have not told mach3 that I changed that tool if I go down here on the tool and switch to tool 22 0 enter you can see that my Z coordinate has now changed 0.341 so it's 340 1000s positive and in fact if you look at the tool here that looks about right I'd say that's about 1/3 of an inch too high now that I've actually selected tool 20 now if I go back and tell it to drive to GZ 2 z 0 now it's going to come back down and you can see the tip of that tool is now even with the top of the of the scale now so it's driven this same tool to the same physical height with the same g-code coordinate because I switched to a different tool number here so it knows to apply that offset and this is really all there is to it now instead of during the CNC program instead of me swapping the tool and then coming in here and telling Mach 3 which tool number it is the program will be telling me to swap the tool I physically change it and then it already knows which tool number I'm going to because the CNC program has that in it so let me stick a piece of stock in here let's zero up on it and let's go through the steps and make a part I've got a piece of stock here in the mill vice and I've got tool number one my edge in it first thing I need to do is find the center of this okay so we found the X&Y Center now we just need to find the z height now I always find the Z height with a shim I have a piece of copper here that I know is ten thousandths thick and I put it under here and I'll come down till I can feel the grip and I know I'm at a Z height of ten thousand thing and I cannot emphasize this enough and you will thank me if you remember this and it saves you some broken tools right now what I have selected here is tool 20 because that's the last tool I was working with that tool that I'm about to zero with is tool number one if I leave this set to tool 20 and 0 I will get the wrong offset because it will be applying the wrong tool length offset you must must must select the correct tool when you do this when you first power up Mach 3 usually tool zero is selected which has no offset and so you'll get nothing and so then when you zero at that height and then put in then switch to tools for machine that have actual length you end up cutting the air up above that's your best case scenario worst-case scenario well we can all imagine worse scenarios but a much worse scenario is if you have a shorter tool selected and you zero it and then you come in and try to run with other tools the mill will have no idea where it is it'll actually start ploughing into the workpiece into the vise jaws all kinds of bad things happen so us click here enter one press the Enter key now I have tool one selected now I can zero the mill so I use my dial here and I will just run this down until it just grips this part if it just grips this 10,000 there and it's just gripped it so over here in my offsets I have already entered Oh point zero one into the gauge block height that I'm using and so I just click here and click set Z and so now it's set Z to ten thousand of this tool which is 201 which I have entered here is ten thousand ow I'm all zeroed up and I'm ready to do some machining now it can be a little bit confusing because while the program is running it's not actually going to change this number but if I look down the program I can see T 28 28 which is the superfly is the first tool that's going to be called up so the first tool change in the program just gets skipped it just assumes you already put the right tool in so I'm gonna do that now I'm going to put the superfly in the mill okay so he put lies in the mill air compressors all charged up I got air I've got coolant let's let her run [Music] [Applause] [Music] [Music] there we go nice and clean just like the superfly always does so now if we go back here and look at the program you can see that it has stopped and it's waiting for a tool change the status line down here says engrave one which was the you know that the the name that I gave to it that's the comment and the program engrave one but you can see it's sitting on a line the next line here says T 20 I don't know if you can see that so it's waiting for me to put in tool 20 so let me put in tool 20 now tool 20 is actually shorter so if it just started engraving without having without knowing about the tool table difference it would just end up turning up in the air and not actually cutting anything now you can see here that even though we just finished with tool 28 and we're going to 20 this still says tool 1 here and still has the height offset of tool 1 Mach 3 is really applying the tool offset even though it's not showing it here so we've got this in here get the coolant going get this spun up and then we'll check it continue on the program and it will do the engraving and assuming we set up our tool table correctly and it switched to the right tool and LU the engraving in the top of the part [Music] [Music] that's the engraving complete now we've gone from a longer tool to a shorter tool now we're going to go back to the longer tool the superfly and shave this off now fortunately it did do the right thing and it cut to the right depth unfortunately the burr I promised you really didn't materialize the tool was sharp enough that I didn't get much of a burr but we'll come back with the superfly and assuming all the tool lengths are correct this should just shave a couple of thousand leave a nice clean finish then we just hit cycle start to continue there it is barely dusting the top there is the finished part that is really all there is to using tool offsets in fusion 360 and Mach 3 if you're joining these videos or find them useful please give me a thumbs up feel free to subscribe to the channel and leave me a comment I'd like to know what you think thank you for watching you [Music]

Channel: Clough42

Views: 23,419

Keywords: Machine Shop, Machining, CNC, Milling, MACH3, Fusion 360, Tool Length, Tool Length Offsets, Tool Table, Tormach, TTS

Id: yE2NWeIzuXA

Length: 43min 26sec (2606 seconds)

Published: Thu Nov 08 2018