Measuring Tool Lengths in MACH3 Without a Presetter

today we're going to try to demystify running tool length offsets in mach 3 without a tool presetter welcome back to cloud42 i'm james well if you're a friend of the channel then you know i just put a new spindle on my grizzly geo 704 cnc mill back here now previously i was using the stock r8 spindle so i was able to use the tormach tooling system and with tts you're able to measure the lengths of the tools on the bench with a height gauge and then enter that data manually into mach3 so it can compensate for the different lengths of the different tools when you swap them out during a cnc program now this spindle has a taper and with taper tooling there's not really an easy way to measure on the bench unless you want to spend thousands of dollars on a tapered tooling presetter and spoiler alert i don't so i'm going to switch over and instead touch the tools off in the spindle to establish their links and it turns out mach3 makes that really easy to touch off tools and automatically update the tool table but it's something that wasn't very well explained when i was trying to learn it so today i'm going to make the video that i wish i'd been able to find here's a sampling of the tooling that i have for my new spindle and these just have you know a taper that locks into the mill spindle and facility for holding a tool in this case this is an er 32 collet this one's a drill chuck and and i've got some er20s and of course i've got the hymer which is just held in an end mill tool holder so that again it can be mounted in the spindle at a repeatable height to measure the position of the work piece now if you're not familiar with using tool length offsets in a cnc mill i did a video on that and i will put a link up here in the corner and you can go check that out if you would like today we're just going to assume you're familiar with the process but as a short refresher essentially what's going on is as we're running a cnc program we're going to use this taper tooling and these tool holders to swap different tools in i've got a quarter inch end mill here i've got a spotting drill i've got an eighth inch end mill and one of the things you'll note is that of course these different tools stick out a different length from the face of the tool holder so if i'm going to run a program and swap from one tool to another then the controller in this case mach3 has to know the relative lengths of the tool so it can compensate so that the tools will cut at the same height and i can make a part now the system that i was using previously is designed to work in an r8 collet this is these are actually clone tool holders but it's called the tormach tool system or tts and the way it works is a three-quarter inch shank and this fits into a shortened ra collet and as that collet tightens up there's a register here that presses against the face of the r8 spindle nose and so this tool always goes in and ends up at a repeatable height so all we have to know is the distance between that register and the tip of the tool put that into mach 3 and it's able to then compensate for tools of different lengths and the way tormach generally does this is they sell this which is a small granite surface plate with a hole in it and you can just set the tool through that hole so the register is on the surface plate and you can come along and measure the tool with a height gauge and enter that number in the tool table in mach 3. so i grab a shorter tool measure that one enter this height into mach3 so now when i switch between those two tools mach3 can automatically compensate but how do we do that with a taper tool now there is a flat face here but this flat face is not a consistent distance from the spindle nose what's really going on is this taper is going in and locking against the taper in the spill in the spindle and that's what actually determines the z position of the tool so we can't measure off of this face because two different tools there actually is a different amount of space between the spindle nose and that flat surface so what we need to do instead is use normally what you do is use a tool presetter with a taper in it that this drops into locks into place and then you come over the top and measure it or it has an optical comparator system but those systems for taper tooling are very expensive i thought about trying to make one trying to figure out well could i just mill just interpolate the right taper in a block and set it in the block under its own weight but then i wasn't sure if the tension on the pull stud is going to affect different tools differently and get me inconsistent results and then i realized i don't need to do any of that i already have a something that will hold this and it's the mill spindle itself so what we're going to do is we're going to just put these in the mill spindle touch the tip of the tool off and use that to measure the length now i thought this was going to be really complicated but as i looked into it i realized mach3 has features in it to automatically do this and automatically update the tool table i didn't really find good videos or instructional material on the web that i thought explained it clearly so today i'm going to make the video that i wish i had been able to find let's go over the mill and take a look at the process this is mach3 i will apologize for the poor quality of this video i don't actually have a screen capture on this machine just because it doesn't have the horsepower to run it i do have a new computer coming that is going to have that so in mach 3 we have our dros up here that show the work coordinate system that we're currently working in with the mill and we have a table of tools if i go to config tool table we have a list of all the tools and their diameters links and information about where height and diameter wear which we're not going to be worried about today we're mostly just going to be concerned with the height so this is a list with a with a every tool has a number and every tool has a height there's some descriptive information in there but that's just for the humans so that we don't make a mistake and i have gone through and set the heights of all the tools to zero so that we have a clean starting point i had these heights all set originally for my tts tools but since i'm switching over i don't want to have any old data in here that causes me to crash the mill at some point so if we go all the way down the only one that has a height in here is tool 99 and that's the hymer and i have a height in here and we'll talk about where i got that number here in just a minute so the first thing we need to do is actually establish a position that we can reliably know where the mill is now i've already set the length for the hymer tool so i'm going to set the heimer as my active tool by entering 99 in the tool here and hitting enter and you can see it does have a height 4.869 inches and this really isn't that important we'll talk in a minute about where i got that and let's go over to the tool offsets and actually zero the mill on something here's the hymer i'm going to put that in my foot on the pedal down here suck that into the mill and for the purposes today i'm just going to use the anvil here on the movable jaw of the vice as my flat surface so the first thing we need to do is locate zero on this now i'm going to go past the zero and then i'm going to come up to it and in fact i happen to hit it exactly okay so now we are exactly on zero now we have to have some kind of a starting reference to a length now the hymer is a hard one to measure because you have to measure it when it's actually under tension and you actually have it resting on a part because the plunger length changes so we've got this right now set to exactly zero and we have to choose a reference for the length now i could just declare that the heimer tool length is zero and that's fine because all mach3 really cares about is the relative length of the tools but if we just declare that this is zero then what will happen is tools that are longer and shorter are going to have different lengths the sum will be positive and some will be negative and that introduces the possibility of dropping a minus sign and causing a crash so i'm going to run this the same way we would with the tormach tooling system and that is we'll establish zero on the face of the spindle now the exact face of the turning part of the spindle is hard to get at but i can easily get at this surface so what i did is i brought it down set it on zero just like this and i brought in a set of gauge blocks and slid them under here and just measured this length and that's how i got that length that i have in the tool table for tool 99 and that tool again is 4.869 that's the length that i established so what we're going to do is we're going to zero our work coordinate system using that tool and using that known length now it doesn't actually matter if that length is correct or not as long as it's sufficient that we aren't going to have any negative linked tools i'm happy again because it's only the relative lengths that matter and since we're going to measure off of our work coordinate system they'll all be relative to whatever we have on this tool so to zero the work offset which i have work offset one which is g54 and i have set this up you can enter a gauge block height and then set the z based on the current position of the mill i'm not using a gauge block with the hymer i'm directly on the surface so i've got zero entered here and i will just click set z and so you can see that my z coordinate here in my current working system is zero and i do have tool 99 selected with that offset so now that i have actually zeroed my work offset based on the one tool that i do know the length of i'm now ready to measure the length of other tools that i don't know the length of so let's make sure i'm going up so i don't break another hammer tip okay [Music] and let's bring in the first tool we want to measure and the first tool that i'm going to measure is this one this is a carbide spotting drill this is tool number two so i'll put that in the spindle now i need to bring this down and touch this surface but that's the last thing i want to do is actually bring this down and actually ram a carbide tool into a hardened surface so there are a couple of ways you could do it i have previously used brass shims and brought it down and just moved it until it just clamped it but that's really not very precise because these get beat up and it's hard to tell when you're exactly on it instead i'm going to use a gauge pin now this is a three-quarter inch diameter gauge pin you can just buy these individually if you don't have a set of gauge pins i just picked this up off of amazon for a few bucks and what we're going to do is we're going to bring this down until we can just roll this under the tip so what i'm going to do is i'm going to bring it down so it's low enough that it will not fit under so it will not go under the tool and then i will slowly bring the tool up until it just passes under i'm going to do this i've got dialed down so i'm incrementing by 10 thousandths of an inch and i'm dialing in the up direction only you do not want to dial down and there we go it just goes under but i can actually feel it touch so we are with this tool we have confidence that it is now exactly three quarters of an inch off of this surface now because i'm moving in the upward direction this mill actually has a little bit of backlash in the z-axis between a thou and two-thou backlash and the z-axis and so i want to make sure that when i'm using it for measurements that backlash is always taken out in the same direction so since i'm moving upward in order to move this pin underneath i am the i wanted to move upward on the heimer as well that's why i went past zero and then came up to zero so now we have this now so it is exactly three quarters of an inch above the movable jaw here on the vise which is where we zeroed the work coordinate system so now i'll come in here make sure that i have tool two selected so enter two hit enter now you can see my z offset currently is zero for that i touched it off based on a three quarter inch pin so i have 0.7500 in here and then i will just click set tool offset and what it's done is it's figured out that the z offset of this tool is 3.354 inches now that makes sense because the heimer was over four inches this tool is a little shorter and so that makes sense as a z offset so i can just say save tool offsets and that will make it permanent so if i come in here and that opens the tool table here's tool number two my quarter inch spot drill and it has put in a height of 3.353867 inches automatically click apply click ok and now the tool length for that tool has now been set and i can move on to my next tool [Music] next tool is tool 15 which is a quarter inch three flute end mill for aluminum now here is the beauty of this taper tooling system one tool out one tool in done now we'll do exactly the same thing to set the height of this [Music] and there we are there's the zero point this is tool 15 so i'll come in here make sure i have tool 15 selected enter set tool offset and i could wait and save these all at the end but i'm going to go ahead and save it now just to make sure and there it is 3.319787 apply okay now all i have to do is run through and set the links of all the rest of my tools and it is that simple okay so we've got our tool table populated if i go in here and look i've got a length for tool two i've just got putting the tools i'm planning on using on a part i'm going to make here i've got tool 15 i've got tool 25 and i've got tool 31 in addition to the heimer so i've got links on all of those let's do a little test so let's start with the carbide spotting drill tool number two put it in the mill and let's make sure we have tool number two selected and then let's go over here to our mdi and let's just wrap it down to a height of one inch so g zero z one and the spindle should wrap it down to one inch above and stop and there we are and this isn't exactly an inch wide but you can see we are about an inch above the two above the surface there in fact i have a one two three block you can see we're about an inch above the surface and i'll just leave that there it's actually behind the tool from where from your angle so you can just see the height but it's not going to hit it hopefully okay so that was good let's switch to a different tool it's a different length and do the same thing [Music] so this is a much shorter tool this is tool 25 my eighth inch end mill put that in the spindle come back over here make sure we have tool 25 selected and i'm going to do a sanity check and make sure that yes we do have a height for tool 25 and it's shorter which is what i was expecting and let's do exactly the same thing g zero g zero z one and we should wrap it down to the same one inch height at the end of the tool and there we are right at one inch and that is really all there is to it now that we've got the numbers in the tool table for these particular tools we can swap them in and out all day and get repeatable z heights well i hope this was helpful if you enjoyed this video 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 and if you have ideas for other kind of quick tip or technique videos like this go ahead and drop those down in the comments too thank you for watching [Music] you

Channel: Clough42

Views: 16,362

Keywords: Tool Table, Tool Lengths, Tool Length Offsets, MACH3, ISO30, Taper Tooling, Tool Presetter, Tool Setter, Haimer

Id: um75P9vmoK4

Length: 18min 30sec (1110 seconds)

Published: Sat Sep 05 2020