1. This site uses cookies. By continuing to use this site, you are agreeing to our use of cookies. Learn More.
  2. PLEASE: Read the FORUM RULES BEFORE registering!

    Dismiss Notice

Some Ideas for Ease of Use

Discussion in 'CNC IN THE HOME SHOP' started by MontanaAardvark, Apr 25, 2017.

  1. MontanaAardvark

    MontanaAardvark United States H-M Supporter - Premium Content H-M Supporter-Premium

    Likes Received:
    61
    Trophy Points:
    28
    Location:
    Just South of the Kennedy Space Center
    City:
    Melbourne
    State:
    Florida

    -Return to Top-

    Now that I have my CNC G0704 running, I've been thinking of ways to make living with it easier and do things faster. I thought I'd put out a couple of ideas running in my head and ask you gurus what you think.

    I'm not doing this for money, but a lot of time spent indicating the edges of a part for every part just seems like a waste of time. It's not hard, it's just tedious. Industry uses tooling plates or homing switches that always are (0,0) and I'm thinking of doing something like that. I've assigned a fixture (0,0) for several parts on a little project I'm building, making the front left hand corner of the fixed jaw on my vise into (0,0). All I have to do is put a piece in the vise, press it against the stop and it's ready to machine. Yeah, all my Y numbers are negative, but no big deal.

    The issue is that the vise only holds a small range of sizes without changes. Something like this Sherline-sized tooling plate from eBay looks like the trick to do (no relation to the seller, don't know if it's any good, and all disclaimers). Set one corner as the reference point and go from there. Making or getting one for the G0704 might be a good exercise, although I think the clamping screw holes would have to be bigger due to the (much) higher power of the Grizzly over the Sherline.

    Do any of you guys do anything like this?

    The other thing I'm trying to improve is tool changing. I'd love a Tormach changer and the whole TTS, but they're like $4000 so that ain't happening (I am a retiree, after all). So I was thinking of getting a bunch of R8 end mill holders at $16 or $17, like this from LMS, and making a system of my own. Set the tools to all the same distance out of the holder (1" as example), and then when it's time to change tools, I'll still need to swap tools in the spindle, but they'll all be zeroed once the new end mill holder is in the spindle. I can replace the four sided nut on the G0704 with a regular hex head and stick a socket on a battery powered wrench to speed loosening/tightening. Or maybe a manual drawbar like Hoss shows on the DVD.

    Again, anybody done anything like this?


    Bob
     
  2. jbolt

    jbolt United States Active User H-M Supporter-Premium

    Likes Received:
    901
    Trophy Points:
    113
    City:
    Mountain View
    State:
    California

    -Return to Top-

    I have several tooling plates made from 1/2" aluminum plate or 1/2" mic 6 aluminum. I prefer to make my own since the pre-drilled hole locations may not line up well with a part. I also like to use dowel pins for locating stock. I machine the back edge and part of one side of the tooling plate for setup and reference. I keep a 3D CAD model of each plate and use them for creating the tool paths with the part on the plate. I also model the clamping fixtures so I can make sure I don't accidentally have a tool path go through a clamp. (learned the hard way)

    I generally keep two 4" vises on my mill so I can extend the clamping range or run multiple parts. I also made a tooling plate from 3/4" aluminum that is machined to clamp in the two vises if I have a part that is outside the vise clamping range but don't want to take the vises off.

    I use the TTS holders with a power draw bar. I like the TTS holders over the R8 end mill holders because they are faster to change plus they have drill chucks and ER collet holders etc..

    In Mach3 I have a master tool, tool zero. Once that tool is zeroed in Mach3 all the other tools are given a number (corresponding to the tool in the CAM program) and their offsets are entered into the tool table in Mach.
     
  3. JimDawson

    JimDawson Global Moderator Staff Member Director

    Likes Received:
    3,785
    Trophy Points:
    113
    City:
    Sandy
    State:
    Oregon

    -Return to Top-

    Your plan sounds fine for fixturing multiple parts. For one-off parts, most times it's better just to locate the working edge or a feature on the part. I don't have a vice on the table for most operations, that's what the T-slots are for. If I need the vice(s), it only takes a couple of minutes to mount and tram the vice. To tram a vice, snug up one of the bolts, then just bump the vice with your hand as you traverse with the indicator using the jog buttons. Once you have minimal movement on the indicator (don't worry about getting it to ''0'', you are just looking for relative movement), then snug up both mounting bolts. Normally this only takes abouts 2 passes to get it trammed. I don't like keys for tramming the vice. Plan the operations to minimize tooling and fixture changes.

    You can bolt a fixture plate to the table, then maybe use dowel pins to locate the part on the fixture plate. Use flat head screws to bolt the fixture plate to the table and countersink them extra deep to get them out of the way. If you need to mill the entire profile, then you can use shoulder screws to locate the part and then remove the shoulder screws after clamping. I normally try to design parts that have holes or some other area that facilitates clamping/bolting. MDF makes a great temporary fixture plate, you can also make a part shaped pocket to facilitate locating and holding. MDF is very resistant to petroleum based coolant, not so good with water based coolants.

    End mill holders are fine, but trying to get the tools all the same height is difficult at best. Normally you would locate the tool height from a fixed point, maybe the top of the vice, fixture, part, or table, then plug the offsets into the tool library.
     
  4. cs900

    cs900 United States maker of chips Active Member

    Likes Received:
    148
    Trophy Points:
    43
    City:
    binghamton
    State:
    New York

    -Return to Top-

    An alternative, and arguably better, way to set all your tool heights is to use a reference surface and a height gauge to measure the total tool height rather than having a master tool. This method would work with the TTS holders and could work with standard R8 holders as well.

    In addition to using the corner of your vice as a work offset, I take that a bit farther. I have a step machined into some soft jaws for thin work holding. So one of my work offsets is to the corner of the step on the left (G54), another for the left corner of the inside of the jaw (G56) and I also have the same for the right side (G55 and G57). so depending on what side I need to machine I just change the work offset and go. Unless I'm trying to do something very accurately, it's very rarely that I indicate a part. Of course doing this you will need repeatable home switches which I think are a good idea any way.
     
  5. jbolt

    jbolt United States Active User H-M Supporter-Premium

    Likes Received:
    901
    Trophy Points:
    113
    City:
    Mountain View
    State:
    California

    -Return to Top-

    The TTS tool holders register to the face of the spindle. All tools heights are measured (with a height guage) from the spindle mating surface to the tool tip and entered into a tool table. The master tool sets the zero to the spindle face. Each tool has a number (t#) and height offset (h#). Without a master tool (unless you zero the face of the spindle which is not always practical) there will be no offset tool height reference for any other tool unless you zero each tool individually as you use it.

    An R8 holder registers to the taper so it would be difficult to measure the tool height out of the spindle.
     
  6. MontanaAardvark

    MontanaAardvark United States H-M Supporter - Premium Content H-M Supporter-Premium

    Likes Received:
    61
    Trophy Points:
    28
    Location:
    Just South of the Kennedy Space Center
    City:
    Melbourne
    State:
    Florida

    -Return to Top-

    That's exactly the kind of thing I was thinking of. Setting the tool "stick out" of the EM holder is easy. Stand the edge of the holder on the edge of a 1-2-3 block, put the end of the cutter on the surface the block is setting on and tighten the setscrew. The question becomes is that surface in any way locked to the where the R8 taper sits in the spindle.

    Thinking of it another way, there figures to be a reason that EM holders are 17 bucks and TTS holders are more like $80. I spent part of my career assuring repeatability in a totally different field (radio interference levels) and it left me with respect for how much money repeatability really costs.

    <edit to add> The thing is, though, that setting Z heights is very easy compared to setting X and Y zero. As long as the center of the cutter is referenced to the center of the spindle, I'm not sure I care about setting Z heights.
     
  7. cs900

    cs900 United States maker of chips Active Member

    Likes Received:
    148
    Trophy Points:
    43
    City:
    binghamton
    State:
    New York

    -Return to Top-

    maybe we are just confusing terminology. I think of a master tool as a tool that never changes (ie a pin gauge mounted in a holder). Using the method you just described (which is exactly what I was referring to and is the method I use every day) you do not need a master tool, you just need to make sure that height offset is called up in MAch3 before touching the corresponding tool off. You can use any tool to set the Z work offset, and as such you do not need a "master" tool, nor do you need to touch every tool off after that.
     
  8. jbolt

    jbolt United States Active User H-M Supporter-Premium

    Likes Received:
    901
    Trophy Points:
    113
    City:
    Mountain View
    State:
    California

    -Return to Top-

  9. jbolt

    jbolt United States Active User H-M Supporter-Premium

    Likes Received:
    901
    Trophy Points:
    113
    City:
    Mountain View
    State:
    California

    -Return to Top-

    I think were talking along the same lines. Sure there many ways to accomplish the same thing. I prefer the master tool because that value never changes. I don't use a touch-off pad on my mill (I do on my router). I use a dial indicator in a TTS holder. When the indicator is zeroed to the part or fixture reference point the pre-measured value is already set in Mach 3 so I only have to pres the set z button. During startup Mach3 defaults to tool zero so that is the master tool.

    Just my $ .02
     
  10. cs900

    cs900 United States maker of chips Active Member

    Likes Received:
    148
    Trophy Points:
    43
    City:
    binghamton
    State:
    New York

    -Return to Top-

    I think we are as well. I do the very same thing on my lathe with a master tool as I'm too lazy to make a reference fixture to hold the tools so I can measure them.

    My only concern is if you ever crash the indicator, you'll have to adjust all your tools to the new master. Not the end of the world, but annoying for sure, lol.
     
  11. RJSakowski

    RJSakowski H-M Supporter - Premium Content H-M Supporter-Premium

    Likes Received:
    2,418
    Trophy Points:
    113
    City:
    Barneveld
    State:
    Wisconsin

    -Return to Top-

    Take a look at the Tormach TTS system. You don't need the ATC to gain the benefits of the TTS system. The TTS system can be adapted to any mill with R8 tooling. The principle is that the ER20 collet chuck is mounted in a 3/4 R8 collet and as the R8 collet is tightened, it pulls the ER20 collet chuck tight to the spindle face, ensuring a reproducible tool offset. This allows the chuck with tool to be removed and remounted without losing accuracy.The ER collet chucks can be purchased for as little as $25 and other options such as TTS Jacobs taper adapters or end mill holder for Weldon shanks are available. ER32 and ER16 collet chucks are available as well

    You still have to manually load the tooling but it removes the necessity of re-referencing your tooling each time you mount it. I use the Tormach system in both my Tormach 770 and my old mill drill. I believe that Tormach has a white paper describing the process for converting a mill to the TTS system. It basically requires checking your spindle face for runout and truing if necessary. Tormach sells a special R8 collet for use with the TTS system but you can make your own easily by grinding the face of a 3/4" R* collet for clearance.
     
  12. MontanaAardvark

    MontanaAardvark United States H-M Supporter - Premium Content H-M Supporter-Premium

    Likes Received:
    61
    Trophy Points:
    28
    Location:
    Just South of the Kennedy Space Center
    City:
    Melbourne
    State:
    Florida

    -Return to Top-

  13. spumco

    spumco United States Active Member Active Member

    Likes Received:
    35
    Trophy Points:
    18
    City:
    Ashtabula
    State:
    Ohio

    -Return to Top-

    Second the vote to switch to the TTS system. The only similar alternative short of swapping to a BT30 spindle would be a Royal quick-change collet system, and those are very expensive.

    You can even make TTS-compatible tool holders for very little money, especially if you have a lathe. Get some 3/4" ground stock and put a groove in it for a C-clip. Drill and ream for your tool shank. Get some 1-1/2" or 1-5/8" stock and bore it for a light press fit on the 3/4" stock. Cut off some 1/2" thick doughnuts and press them on the 3/4" tool holder using the C-clip as a stop - there's your flange that registers against the mill spindle nose. Use loctite if you're paranoid. Put the assembly back in the lathe and clean up the back side of the new flange.

    Side-drill for a set screw and you now have a $3-$4 tool holder. If you don't trust the runout or set screw holding power, at least you can use it for indicators, taps, whatever doesn't spin at high RPM. And you haven't spent all day turning 1-1/2" stock in to chips just so you can get a 3/4" shank out of it.

    You can build or buy power drawbars pretty cheaply that are based on a cordless or pneumatic impact gun. If you're motivated, an air or hydraulic cylinder-type power draw bar with belleville washers isn't very hard to do.

    As for tool heights, I assuming you're running Mach3, Mach4, LinuxCNC, or some other PC-based control software. All of these controllers have software add-ins available for touch-plate Z-height setters. Whether you choose to use the TTS system or not, setting up (or buying and installing) a touch-plate macro is quite easy. Once set up and you have the touch-plates connected, the macro/software will automatically touch off on the touch-plate after a tool change and set the appropriate Z-height. You tool table will be set to zero for all tools, and the Z-offset will be written directly each time you change tools within the program. The systems that use two plates are pretty slick: one plate of known thickness goes on top of your part at the beginning of the job to set part height zero, and then all subsequent tool changes are done on the other plate that's out of the way on your table.

    This method is slower (during machining) than entering the tool length in the tool table and calling it up mid-program, but it also means you don't have to stop and re-measure if you break an endmill. More frequently, if you have 3 or 4 drills to use during a program you don't need separate drill chucks for each size with the lengths pre-measured. When the tool change sub-program (macro) pauses for a tool change, just put the different drill in the chuck and it'll touch off and write the new Z-height. Again slower, but you don't need a separate holder for each tool.

    In fact, you don't even need the TTS system to take advantage of the touch-plate. Stick with R8 collets for your tools, get a cordless drill, and let the tool change macro worry about the tool length. The reason I prefer the TTS system AND the tool change macro is that it's much faster to change a TTS holder than take the whole R8 collet out for different tool shanks - as well as being shorter (gaining me extra room on tall parts).

    If you do go with the TTS system - and I obviously recommend it - you can buy TTS compatible ER11/16/20/25/32 collet chucks on ebay for about $15-$20 per including shipping. Suggest you visit the Tormach section on CNCZone and poke around.

    Finally, indicating corners is a pain. I hate it too. I'm not an expert, but it appears that in the absence of a tooling plate with known reference points either a high-quality touch-probe or a 3D taster-style indicator is the quickest thing. Even with a tooling plate, you may need to move the tooling plate or mount something on it in a non-standard location or orientation. To use a tooling plate you'll have to indicate it at the beginning of the session anyway, and then still figure out your offsets for the part edges for different jobs.

    Sub-$1k probes will probably get you with 0.002-0.003, perhaps better some of the time. This may be good enough for your work given other slop or tolerances in your machine (if any). A 3D taster (Haimer or similar) is about $400, is good to sub-0.001" and can be very, very fast to setup a part in all three axis. Watch some youtube videos on both probing and 3D tasters; you might find them to be worth your time.

    BTW, there's a guy on the Tormach CNCZone forum who is about to launch an 'impact-tolerant' touch probe that appears to be an order of magnitude more accurate than cheap probes and much more robust (crash resistant) for idiots like me than 3D tasters. I'll be sending him money the minute he makes them available.

    So... TTS system, power draw bar, touch-plates, and a probe or Haimer. If you get all that sorted out you'll spend more time planning the next part and less time dealing with the irritating setup part of CNC machining.

    Good luck...
    -S
     
    RJSakowski and brino like this.
  14. MontanaAardvark

    MontanaAardvark United States H-M Supporter - Premium Content H-M Supporter-Premium

    Likes Received:
    61
    Trophy Points:
    28
    Location:
    Just South of the Kennedy Space Center
    City:
    Melbourne
    State:
    Florida

    -Return to Top-

    Thanks, Spumco! Great stuff. Lots to digest in there, including terms I'd never heard (3D Tasters).

    (and I get the name)


    Bob
     
  15. spumco

    spumco United States Active Member Active Member

    Likes Received:
    35
    Trophy Points:
    18
    City:
    Ashtabula
    State:
    Ohio

    -Return to Top-

    I suspect "taster" is from a German word that doesn't translate quite right. I also suspect it's functionally accurate and amusing enough to English speakers that various manufacturers haven't changed the translation to something clumsy. Like ""3-axis mechanical indicator" or something else stupid.

    That, or "Machinist's Shiny Ball Dingus" was already taken.

    Or you were referring to my screen name, which of course comes from spending too much time watching TV in the early 90's...
     
  16. MontanaAardvark

    MontanaAardvark United States H-M Supporter - Premium Content H-M Supporter-Premium

    Likes Received:
    61
    Trophy Points:
    28
    Location:
    Just South of the Kennedy Space Center
    City:
    Melbourne
    State:
    Florida

    -Return to Top-

    Screen name. I stumbled across R&S toward the end of the first season, and quickly caught them all.
     
  17. spumco

    spumco United States Active Member Active Member

    Likes Received:
    35
    Trophy Points:
    18
    City:
    Ashtabula
    State:
    Ohio

    -Return to Top-

    You got it in one go.

    Give me a shout if you have other questions about TTS or anything else I mentioned. If I don't know the answer, I'll make something up and sound convincing.

    BTW, LMS or Tormach seem to be the only source of finished JT taper TTS holder for drill chucks. No ebay joy for those, but there are plenty of 3/4" shank insert tools (fly cutters, end mills, ect.) than can be converted to TTS. I'm about to try out a 5/8" 2-insert end mill I picked up for about $60 that includes 10 APKT polished inserts for aluminum. Sort of a poor-man's ShearHog.

    Google ShearHog if you don't know what it is and be prepared for a Holy Sh!t moment.
     
    MontanaAardvark likes this.
  18. TomS

    TomS Active User H-M Supporter-Premium

    Likes Received:
    415
    Trophy Points:
    83
    City:
    Redding
    State:
    California

    -Return to Top-

    This is the touch plate I made for finding and setting X, Y, Z zero. Set the touch plate on the corner you want to reference then start the script assigned to the Auto Tool Zero button. Using a rod or cutter of known diameter the script moves the table in the X axis until the rod/cutter comes in contact with the touch plate then backs off 1-1/2" then moves in the Y axis and does the same. The next move is in the -Z direction, contacts the touch plate and retracts 1". Done in about 60 seconds.

    Tom S.



    20170122_154905_resized.jpg
     
    MontanaAardvark and grumpygator like this.
  19. MontanaAardvark

    MontanaAardvark United States H-M Supporter - Premium Content H-M Supporter-Premium

    Likes Received:
    61
    Trophy Points:
    28
    Location:
    Just South of the Kennedy Space Center
    City:
    Melbourne
    State:
    Florida

    -Return to Top-

    It looks like plastic? Two plastic pieces on the sides - I guess to locate it? Is there plastic on the top?

    I don't think I see how it works, yet. Am I looking at the top or the bottom (that touches the piece you're setting zero on)? An outside corner you're going to want to be (0,0) goes in that plastic corner?


    Bob
     
  20. spumco

    spumco United States Active Member Active Member

    Likes Received:
    35
    Trophy Points:
    18
    City:
    Ashtabula
    State:
    Ohio

    -Return to Top-

    I'm pretty sure we're looking at the bottom. The inside metal corner edges are the 'known' X/Y surfaces, and the bottom and sides are plastic to insulate from the work piece. The metal plate is DC+, and the tool is DC- (perhaps through the spindle or another aligator clip. Flat head screws are recessed to maintain electrical insulation from part top surface. Damn clever.

    Similar to my Z touch plates. Mine are spring-loaded so I can rapid down at 50IPM without chipping the tool (it does a second probe at about 4IPM). However, mine doesn't do X/Y - that's pretty cool. It's kind of like an inflexible spindle-mounted touch probe.

    I don't see why you couldn't make a spring loaded probe that could do the same thing. Use a known diameter and you're in business. You could even make a spring-loaded button on the top instead of a telescoping probe thingie so you could do a two-pass fast-slow probe routine.

    I'm still trying to figure out how to touch off quickly on oddball shaped things or the top of round parts without resorting to the old 'creep up on the scrap of paper' trick.
     
    brino likes this.
  21. TomS

    TomS Active User H-M Supporter-Premium

    Likes Received:
    415
    Trophy Points:
    83
    City:
    Redding
    State:
    California

    -Return to Top-

    Your first paragraph is correct. I'll take more pictures and post them. DC- is through the spindle.

    Tom S.
     
  22. TomS

    TomS Active User H-M Supporter-Premium

    Likes Received:
    415
    Trophy Points:
    83
    City:
    Redding
    State:
    California

    -Return to Top-

    Here are more pictures of my X,Y,Z Zero setter. Hope this makes it a bit more clear on how it is used. I can provide the button script if you are interested.

    Originally this was a Z setter only. It was 2" square and 1" thick including the insulation material. I machined the notch so each leg is 1" wide and added the plastic
    ledges.
    20170427_093336_resized (1).jpg

    The groove in the right hand leg is the original hole I used to attach the DC+ wire.
    20170427_093409_resized.jpg

    Top view.
    20170427_093425_resized.jpg

    20170427_093515_resized.jpg
     
  23. MontanaAardvark

    MontanaAardvark United States H-M Supporter - Premium Content H-M Supporter-Premium

    Likes Received:
    61
    Trophy Points:
    28
    Location:
    Just South of the Kennedy Space Center
    City:
    Melbourne
    State:
    Florida

    -Return to Top-

    I think I see it better.

    So you put that piece on the corner of a piece of stock you want to be your reference, plastic side down, and you know that when your ohmmeter goes to zero on each axis in succession, you're at (-1, -1,+1)?

    Cool.
     
  24. spumco

    spumco United States Active Member Active Member

    Likes Received:
    35
    Trophy Points:
    18
    City:
    Ashtabula
    State:
    Ohio

    -Return to Top-

    MontanaAardvark,

    If it's like mine, and every other one I've seen on TV, the DC+ comes from an input pin on the breakout board to the tool setter plate. There's no ohmmeter; when it grounds through the tool & spindle the breakout board pin is driven high (or low? can't remember) and the controller sees the pin state change. When the probe routine is started, the macro/script moves the table and is continuously checking for a state change on that pin and registers the change. It then immediately writes the position to the DRO after compensating for the 1" offset and tool radius which was already entered in some screen field before the probing routine. After the DRO position is updated, the machine is commanded to move some distance off the setter (1-1/2" if I recall) and move to the Y-axis start position. Repeat, and do it again for Z.

    The first time you see the probing routine do it's thing it's like magic: creep-touch, creep-touch, creep-touch - then zoom to origin with the Z at some conveniently safe height above the part.

    That's why the probing routines are usually very slow and you need to jog pretty close to the start point before initiating the routine. You don't want to wait for it to creep at 4IPM when your table is over in the next county. It's done slowly - especially in this particular case when there's a rigid tool about to contact a rigid(ish) tool setter - because if you go fast the machine still has to decelerate after the pin state change and those few 'thou can ding something. It's also why I mentioned a spring-loaded probe or plate, because then you could zoom over to the setter and bang in to it at speed and nothing's bent. Of course, the macro then does it again at slow speed to get a very precise reading, but that time the macro just backs off 0.025" from the first contact location for the second (final, accurate) probe.

    The upside to this compared to a regular touch-probe is that there are no internal contacts to corrode like on a low-end probe. You don't have to worry about the probe stylus being bent from your last crash, or the internal contacts tripping at different distances based on orientation in the spindle and angle of approach. It's also free, more or less - just some wire and a few bits of scrap laying around.

    The downsides, and they aren't bad, are that this arrangement needs the part to have a square corner and be held in a trammed vise (or trammed to the table). Also needs a flat top for the Z to work, or at least a flat surface adjacent to the corner. Finally, I wouldn't trust some of my cheap drill bits to have low enough run-out at the tips to trigger the touch plate within 0.01" of the true spindle position. A 4-flute end mill or stubby carbide drill - yes. Most of my drill bits or a 2-flute end mill with big gullets - no way.

    I'm also betting that Mr. Clever here (TomS) has come up with some workarounds to address the downsides I've been speculating about.

    -S
     
    brino likes this.
  25. MontanaAardvark

    MontanaAardvark United States H-M Supporter - Premium Content H-M Supporter-Premium

    Likes Received:
    61
    Trophy Points:
    28
    Location:
    Just South of the Kennedy Space Center
    City:
    Melbourne
    State:
    Florida

    -Return to Top-

    Sorry - retired electrical engineer so to me, it's kind of an ohmmeter. When I get in a hurry, I write what's dumping out my head.

    I'm familiar with how it works and was looking at how to implement it on my mill and the controller box I built.

    On the other subject, I was looking at this starter set of TTS holders, but realized the drill chuck holder is the wrong size for my chuck, which is JT33. They make one, it's just not in the set.


    Bob
     
  26. TomS

    TomS Active User H-M Supporter-Premium

    Likes Received:
    415
    Trophy Points:
    83
    City:
    Redding
    State:
    California

    -Return to Top-

    In essence, yes. The script can be modified to put the tool where you want it. My current button script language moves the tool 1-1/2" in X and Y and resets the DRO to zero. In Z it moves 1" and sets the DRO to +1". I found the VB script on the internet. I'm not that familiar with script language so haven't tried changing the language so X and Y work like Z. Still it works great.

    Tom S.
     
  27. TomS

    TomS Active User H-M Supporter-Premium

    Likes Received:
    415
    Trophy Points:
    83
    City:
    Redding
    State:
    California

    -Return to Top-

    You got it! I use a 3/8" dowel pin in a dedicated holder to touch off X and Y. Then use the cutter/end mill for the job I'm running to set Z. I jog the table until my "probe" is about 1/2" from the touch off surfaces then run the routine.

    It does have it's limitations but for setting up square or rectangular stock it works. And, as you said, it cost me nothing to make.

    Tom S.
     
    brino likes this.
  28. spumco

    spumco United States Active Member Active Member

    Likes Received:
    35
    Trophy Points:
    18
    City:
    Ashtabula
    State:
    Ohio

    -Return to Top-

    If you want to try out the TTS, for similar money you can get this ER20 collet set.

    They also have ER11, 16, 25, and 32 available. Can also get them with the TTS ATC groove for a bit more money. They aren't all listed on the ebay site, so send them an email - they responded to me within 8 hours. Shipping is a little steep but it's FAST. I'm very, very pleased with the quality.

    Then pick up a JT33 drill arbor and maybe one of the 0-1/4" chuck &arbor combos from Little Machine Shop. Assuming you already have a 3/4" R8 collet, just grind the face down until it's flat so the TTS flanges bear against the spindle nose.

    If you have a DTI or some other measuring tool with a standard shank, you can make a holder like I mentioned earlier in the thread or buy the dedicated set-screw holders a la carte.

    Don't buy collet sets, just buy the sizes you need. I noticed after buying a couple of sets I really only use 1/2, 3/8, 1/4, 3/16, and 1/8. All the xx/64ths and 32nds are a waste.

    Being an electrical engineer I can't imagine you'd need much help, but if you want some help with the probe wiring just let me know what BOB you have and if you're running Mach3 or what.

    Photo of my plates below. Front plate is put on top of the part, and back plate is stationed at machine 0, 0. Jog over the moveable plate, hit the tool-zero initiate and it goes down at 50IPM and touches off. Repeat at 4IPM after a 0.025" backoff and it writes part Z 0 based on the thickness of the plate. It then moves to machine 0, 0 and does the same thing on the stationary plate and writes the difference between Z0 and the stationary plate to a register in the controller. Moveable plate is removed from part and you start machining (after setting X/Y off-sets). All tool changes in the program after the initial probe routine are touched off the stationary plate. The code pauses at M6, you switch tools and tell it go - it then probes, sets the new Z height based on the difference between the two plates, and gets on with machining.

    And with this setup you don't need TTS, because your tool offset is always 0. The Z off-set is changed, but there's no tool off-set applied so you can use regular R8 collets that don't repeat when you swap them out. I just prefer to use TTS because if's fast and I want to build an ATC eventually.

    Closest thing to an ATC I've ever seen. If you're running Mach3, Google & buy the "2010 Screenset" and make yourself some touch plates. The screenset is stupid cheap for all the features and you're not dependent on everything being TTS before you start using it.

    IMG_3400.JPG IMG_3399.JPG IMG_3396.JPG
     
    brino and TomS like this.
  29. MontanaAardvark

    MontanaAardvark United States H-M Supporter - Premium Content H-M Supporter-Premium

    Likes Received:
    61
    Trophy Points:
    28
    Location:
    Just South of the Kennedy Space Center
    City:
    Melbourne
    State:
    Florida

    -Return to Top-

    If you want to try out the TTS, for similar money you can get this ER20 collet set.

    On my end, when I click on that I get a Little Machine Shop page for their 33JT to TTS adapter. It's supposed to be someone on eBay?

    I was just pricing a "starter set" of TTS parts (not the starter kit Tormach sells) and I'm at $295 with a small ER-32 collet set and a few other holders. I need to seriously look at limiting the number of cutters I have, or that description of how to make some. I have a couple of 3/4" shaft cutters I want to use: a face cutter and an end mill. It looks like I'd need two TTS ER-32 collet holders and two 3/4" collets.


    Bob
     
  30. spumco

    spumco United States Active Member Active Member

    Likes Received:
    35
    Trophy Points:
    18
    City:
    Ashtabula
    State:
    Ohio

    -Return to Top-

    Crap. I suck at posting links. Try this one.

    For your 3/4" shank cutters you could just make a flange that registers against the spindle nose and stick the shank straight in the TTS spindle collet. If the end mill is too short for that, you'll need an ER32 as you mentioned.
     

Share This Page