# Some Ideas for Ease of Use



## MontanaAardvark

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


----------



## jbolt

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.


----------



## JimDawson

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.


----------



## cs900

jbolt said:


> 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.


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.


----------



## jbolt

cs900 said:


> 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.



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.


----------



## MontanaAardvark

jbolt said:


> 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.



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.


----------



## cs900

jbolt said:


> 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.



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.


----------



## jbolt

MontanaAardvark said:


> Thinking of it another way, there figures to be a reason that EM holders are 17 bucks and TTS holders are more like $80.  .



The standard TTS set screw holders are $22. ER collect holders are $35 https://www.tormach.com/store/index.php?app=ecom&ns=catshow&ref=TTS&portrelay=1


----------



## jbolt

cs900 said:


> 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.



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


----------



## cs900

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.


----------



## RJSakowski

MontanaAardvark said:


> 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


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.


----------



## MontanaAardvark

jbolt said:


> The standard TTS set screw holders are $22. ER collect holders are $35 https://www.tormach.com/store/index.php?app=ecom&ns=catshow&ref=TTS&portrelay=1



I was sure I'd seen TTS holders for quite a bit more at Little Machine Shop, but now I can't figure out what I was looking at.  The set screw style holders would be fine.  I think I'll go down this road.


----------



## spumco

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


----------



## MontanaAardvark

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

(and I get the name)


Bob


----------



## spumco

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...


----------



## MontanaAardvark

spumco said:


> 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...



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


----------



## spumco

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 **** moment.


----------



## TomS

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.


----------



## MontanaAardvark

TomS said:


> 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.
> 
> 
> 
> View attachment 232257



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


----------



## spumco

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.


----------



## TomS

spumco said:


> 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.



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

Tom S.


----------



## TomS

TomS said:


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



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.



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



Top view.


----------



## MontanaAardvark

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.


----------



## spumco

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


----------



## MontanaAardvark

spumco said:


> 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



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


----------



## TomS

MontanaAardvark said:


> 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.



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.


----------



## TomS

spumco said:


> 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



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.


----------



## spumco

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.


----------



## MontanaAardvark

_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


----------



## spumco

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.


----------



## MontanaAardvark

spumco said:


> 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.



Thanks.  I was just looking for a model at Grabcad to see if it had all the dimensions, but I haven't found one, yet.  I'd probably need to hold one of the TTS holders in my hand to understand what I have to do. 

The tool holders all seem to have a taper on the end that goes into their TTS holder.  If I can just take my 3/4" R8 taper EM holder and grind the face flat, that taper can't be an important dimension, right?  It has to be there just to help the tool changer pick it up and get it started easier (human or automatic changer).


----------



## MontanaAardvark

Back to the other topic, I "found" a piece of 1/2" aluminum plate in the shop (it was hidden under some stuff and I forgot I had it!)  so it seems natural to cut it to make a tooling plate.   It's 20x14.  

I don't know what size to make.  If I make it wider than the table, I'm sure it doesn't buy me anything.  My Y axis travel is a little low, like 6.65 instead of the factory 6.875, so if it's wider than that, I don't see the cutter can reach it.  The X travel is normal.  Other than supporting something unusually big, I don't see making the tooling plate bigger buys me anything.  

Making it smaller: the size of the middle part of the table makes a lot of sense.  The area between the outer T-nut channels is 4-1/2 wide, and between the channels on the ends it's 24 3/4 wide.  If I make it as long as I can and 4-1/2 wide, I can get clamps from the T slots all the way around the table.  I could put tapped holes and holes for 1/8" dowel pins in lots of places.   Since my Tee nuts and clamping set all use 3/8-16, that seems like the size to use.  As bonus, the middle of the plate would be on the center T-slot, so I can put some short bolts (3/8-16 x 3/4") in a couple of places to help mount it to the table

So it sounds to me like making it 20 long by 4-1/2 wide makes the most sense.   Comments?


Bob


----------



## spumco

The taper is just there to ease insertion as you surmised.  Probably also to keep a sharp corner from nicking the inside of the R8 collet if the shank is hardened.  Put a 30 degree chamfer on the shank and then round it a bit with a file and some sandpaper.

As for your tooling plate...  Something I've seen that might be useful to consider would be make it wider then your travels by a bit - maybe 1/2" or 3/4.  Then when you're done with drilling/tapping it use an engraver or V-bit and engrave a shallow groove all the way around that helps you visually indicate the machine limits.  You'll also need to drill & ream a hole in two corners for dowels that you might use to indicate the plate since the machine won't reach the outside.  That, or some other feature(s) for squaring the plate to the X-Y axis if you have to remove it and then re-mount it.

Also, if it's a bit wider than the table you can have threaded holes outside your limits for clamping bit stuff. The clamp holes don't need to be precision located - just a few for some strap clamps.

Something else clever I've seen is to space it up off the table with 1/2" or 1" standoffs.  If you use plenty of big diameter standoffs and mounting screws it won't flex that much and will make it WAY easier to clean the swarf out of the holes and the table slots.  You won't need to use a million plastic screws to fill the unused threaded holes - just leave them empty and blow them out.  The standoffs won't need to be super-precise in length because you'll bolt the plate down and use a fly cutter to deck the whole top a few 'thou with it's in place.  That's why I suggested making it a _bit_ bigger than the travels - but not bigger than a 2"-3" fly cutter can reach.  Just plan on re-decking it every time you have to re-mount it.

All of this assumes that you aren't using strap clamps to mount it.  1/2" is a little thin, but some 3/8-16 flat head screws countersunk straight in to the T-nuts would keep you from having to worry about clearance heights over clamps at the perimeter.  Just counterbore the holes 0.075" before you countersink and that'd give you plenty of extra fat to deck the plate a few times without running in to the screw heads.

If you have a big enough drop or drops from the plate, you could make a tooling plate that fits in your vise.  NYCCNC on youtube has a video about this that may give you some ideas.


----------



## spumco

MontanaAardvark said:


> Thanks.  I was just looking for a model at Grabcad to see if it had all the dimensions, but I haven't found one, yet.  I'd probably need to hold one of the TTS holders in my hand to understand what I have to do.
> 
> The tool holders all seem to have a taper on the end that goes into their TTS holder.  If I can just take my 3/4" R8 taper EM holder and grind the face flat, that taper can't be an important dimension, right?  It has to be there just to help the tool changer pick it up and get it started easier (human or automatic changer).



The idea is that any 3/4 shank tool can be modified to work with the TTS system.  The trick is that you need a flange on the tool to bear against the spindle.  The TTS shank is about 1-1/2" long, and the flanges are about 5/8" thick.  Because the flange has to be locked to the shank, you need some mechanical device to keep the flange from sliding down the shank when the collet tries to pull the shank & flange up against the spindle nose.

Method one is to use a tool with a shank larger than 3/4, and then turn the shank down.  The flange then bears against the shoulder.

Method two, which I plan to do, is start with 3/4" ground stock.  I'll then turn a groove for a C-clip 2-1/8" from the end of the shank.  The 5/8" flange is then pressed (or glued) on the shaft and the C-clip acts as a shoulder to keep the flange from sliding down the shank.  The flange is then faced off (on the spindle side) so the flange-to-spindle mating surface is true and the holder isn't pulled to one side when the drawbar yanks it in.  Keeps me from having to turn down a perfectly good 1" or 7/8" bar to 3/4" just so I can have a shoulder for the flange.


----------



## spumco

In the interest of full disclosure, I've just started using the TTS system - having finished my drawbar a few weeks ago.  I was having some problems setting up my 4th axis (also first 4th part) and noticed some runout on my edge finder when I was trying to touch off the side of the part.  Getting the DTI out I measured +/- 0.003" at the end of the wiggler.  0.006" runout is way, way wrong.

Long story short - the Chinese TTS holders, Tormach collet, and my spindle taper are fine - all within 0.0001" or so.  I measured "only" about 0.0015" of Z change on the face of the spindle nose, but figured maybe skimming the nose be the ticket.  I've seen videos of people taking a light cut on their spindle nose with a lathe tool held in the vise, and Tormach's TTS user manual even describes doing this.

Turns out it was, and that when the TTS tool holder flange gets pulled up against the spindle nose any issues get magnified in to angular misalignment and resulting tool runout.  Taking 0.005" off the nose in two passes and stoning the nose until the DTI read 0.00005" fixed everything.  I now have 0.00015" (or better) 3" from the spindle nose regardless of tool holder orientation.

Moral of the story - plan on skimming your spindle nose if you switch to TTS.  Carbide inset lathe tool run at 250RPM and manually jogged across the face at around 4IPM gave a good cut and 30 seconds with a very fine stone got the last few microns down and averaged the surface nicely.

-S


----------



## MontanaAardvark

spumco said:


> In the interest of full disclosure, I've just started using the TTS system - having finished my drawbar a few weeks ago.  I was having some problems setting up my 4th axis (also first 4th part) and noticed some runout on my edge finder when I was trying to touch off the side of the part.  Getting the DTI out I measured +/- 0.003" at the end of the wiggler.  0.006" runout is way, way wrong.
> 
> Long story short - the Chinese TTS holders, Tormach collet, and my spindle taper are fine - all within 0.0001" or so.  I measured "only" about 0.0015" of Z change on the face of the spindle nose, but figured maybe skimming the nose be the ticket.  I've seen videos of people taking a light cut on their spindle nose with a lathe tool held in the vise, and Tormach's TTS user manual even describes doing this.
> 
> Turns out it was, and that when the TTS tool holder flange gets pulled up against the spindle nose any issues get magnified in to angular misalignment and resulting tool runout.  Taking 0.005" off the nose in two passes and stoning the nose until the DTI read 0.00005" fixed everything.  I now have 0.00015" (or better) 3" from the spindle nose regardless of tool holder orientation.
> 
> Moral of the story - plan on skimming your spindle nose if you switch to TTS.  Carbide inset lathe tool run at 250RPM and manually jogged across the face at around 4IPM gave a good cut and 30 seconds with a very fine stone got the last few microns down and averaged the surface nicely.
> 
> -S



Very interesting.  For some reason, yesterday I was thinking about doing just that.  

I got the Mach3 2010.set going yesterday, and need to wire in the contact system.  The hardest part will be getting my control box out of it's corner and onto a workbench so I can get to the BOB.  Shouldn't take too long.   

I'm going to get the tooling plate done before I work on tool holding, but these suggestions are really helping me.  I sure hope they're useful to the HM community.  

The TTS system has a lot going for it.  I was thinking that I've got a tool box drawer full of cutters, and I just had to order a new size EM Friday.   Most of my cutters are 3/8 shank from my Sherline, but they're still different cutters, some 1/8 shank, one 1/2, plus a few larger ones.  The odd one is I have one of these sets which are all a different diameter - they will be harder to live with.  If I figure I need 10 holders, as long as there's one dedicated tool holder with a tool assigned to it, even with buying everything from Tormach/LMS, it's not that bad.  Even cheaper if I get some of those China.com holders to work.


----------



## spumco

Just for reference, I set up my 'starter kit' as follows:
10/ea ER16 Chinese TTS collet chucks
5/ea ER32 same source

1/ea 1/2" drill chuck + TTS arbor from LMS
2/ea 3/8 drill chuck +TTS arbor
2/ea 1/4" drill chuck + TTS arbor (the cheap package deal they offer)

Plus 1/ea 3/8" set screw holder I bought from Tormach a while ago as a guinea pig while I was building the drawbar.  Now the wiggler lives in it.

I will probably wind up with about 5-10 home made set screw holders for frequently used, lower-speed tools like 1/4-20 taps and such.


----------



## spumco

TTS update 2:

My new outboard spider chuck just came out of the mill.  The TTS system was stupid fast to change 5 tools (drill-mill to spot, Q drill, #7 drill, drill-mill for chamfer, 3/8-24 tap, 1/4-20 tap), and there was no wobble, run-out, misalignment or other issues with the tool holders. 

Running that 3/8 tap almost an inch deep would, I think, have revealed any slip or tool holder problems.  I'm sold.

Watching the 4th axis dance during the chamfer op was pretty magical.  I'd post a video but it's too big and needs some editing.


----------



## MontanaAardvark

BTW, do you have a G0704 or something else?  I've never tapped holes under power on the mill, but allowed my lathe to pull the tap in under power.  

A spider chuck is on my list of things to make for some possible gunsmithing projects.


----------



## spumco

I have a Mikini 1610L mill.  It's an orphan mill, company is out of business since about 2012.  Superb mechanical parts, ferociously crap electronics.  SumDood in California set up a company around 2006-7 to import the mill frames and he designed (or paid for design) & sourced all the electronics from backyard Chinese sweatshops rather than proven COTS components.  The result was utterly unreliable spindle operation and some incredibly cheap, failure-prone components.  The axis motors & drives he bought open-market; oddly enough those work fine and I've kept them.

Bought it last year knowing the reputation and I've spent the past 8 months gutting it and re-doing every eletrical component on the mill.  New computer, BOB, spindle motor, VFD, etc.  Price was right due to the known electrical issues, and it cut down on the time/effort of a manual to CNC conversion.

It's about the same size as a Tormach 1100, but has linear rails instead of turcite-coated dovetail ways.  So mine is probably a touch less rigid, but much, much faster rapids and no gibs to adjust.  The basic mill mechanicals are still being manufactured and sold under the brand SkyFireCNC, but with a few updates and far superior electronics.

As to tapping, I bought a big (too big, frankly) spindle motor with an encoder on the shaft and rigged up an index trigger on the spindle.  The controller software I'm using is UCCNC and it has the capability of rigid tapping out of the box.  Because everything is working well and the software isn't as (potentially) glitchy as Mach3, I can actually peck tap and not wipe out the threads.

Spindle speed goes up to 7400rpm, and I've set the rapids to 200IPM, but it can go a bit faster.  Cutting speeds up to 100IPM without losing steps (with low-pressure tool paths).  If I ever make some money with it I'll probably switch over to 750W servos just to bump the rapids and cut down on the irritating stepper noise.  It's plenty accurate now, but I fantasize about UCCNC upgrading their motion controller & software so I can use servo encoder output to close the loop back to the controller.

And yes, the spider chuck is for my G4016 14x40 lathe for exactly the same reason you want one.




The lathe mess.  I'm a slob.  Tablet is a home-made DRO.




The new spider chuck.  0.001" runout after tweaking the screws.  Woo!


----------



## jbolt

spumco said:


> The lathe mess.  I'm a slob.
> View attachment 232666



Tools are for using not displaying. I call that getting work done!


----------



## MontanaAardvark

Nice shop.  

The reason I asked was comparing spindles.  At the speed mine will dial down to, it says 50 RPM on the dial, I figured I could tap a full 3/8-16 hole in about 20 seconds.  I could stop it if the spindle started making odd sounds, but my experience with taps is that the first odd sound I hear is "snap!"  I think I felt something odd the last time one broke on me.  I know there are such things as tapping heads to attach to tools, they're just out of my price class.  

I'm not familiar with that brand of mill, though. 

My big lathe is the LMS 3540, which is sold as an 8.5 x 20, so "almost" a 9x20.     


There's enough room to stand comfortably between the mill enclosure and the lathe.

Turning to the left and backing up a little to get everything to fit.  


The G0704, controller box (lower middle - an orange plexiglass top) and the computer that runs it all.  You can't see the Ethernet Smooth Stepper that allows me to run three different CNC machines.  It's behind the PC on the left.  If you look on the right end of the table, you see rough cut Rev.1 of a tooling plate.  I need to pull the vise and work on that.  

Turn to the left a little more, and see the Sherlines.  



The mill is really a Sherline/A2ZCNC combo.  To its left are a fully manual Sherline 4400 lathe and a CNC-driven Sherline lathe.  I need to work on that; I'm going to replace the original wiring I made for it with an ethernet cable for the better flexibility.  Actually, the mill needs some maintenance, too. 



Bob


----------



## spumco

Bob,

Likewise on the nice shop.

As to tapping, you have a couple of options short of spending quite a bit of time and money on a closed-loop spindle system with different control software.

1. Tension-compression tap holder.  These apparently work quite well.  Tormach sells them for use on their 1100/700 mills, and they don't have an encoder or even an index signal.  Tapping a blind hole is dodgy unless you have plenty of over-run room, but it can be done.  Through-holes are a breeze.  You just can't peck-tap because the controller has no idea where in the rotation the spindle is and because of the fact that the compression feature means the thread doesn't start in exactly the same place every hole.

Shars sells a 3/4" shank ER20 floating tap holder for about $100.  There are a few from China on ebay for about $80.  Press a flange on it, grind the shank to length with a taper on the end, and you now have a TTS-compatible floating tap holder.  Or, for $135 you can buy a genuine Tormach TTS floating tap holder.

2. Thread-mill.  You've got a CNC mill, why not stretch it's legs?  Threadmills aren't cheap, but you could grab an old tap and grind off all the teeth except for one just to fool around with it.  Just be sure to grind the tip off so your new single-point thread mill has a full profile.  I believe there's a youtube video or two about using a homemade threadmill - have a look.

There are plenty of resources online to help with the code, but basically the thread mill goes down to the bottom of the hole, moves in to the hole side wall to cutting depth, and then does a helical interpolation up at the thread pitch.  Repeat at increasing depth of cut until the thread fit is to your preference.  You helix _up_ so that you're climb milling rather than conventional, BTW.

Zero spindle feedback needed, and the spindle speeds are probably in a range more suited to your G0704 than 50RPM.  If you like thread milling then you can go buy a swanky carbide one and you'll be able to cut a wide range of threads with one tool.  Another nice thing is that if you snap one, the shank and cutter are smaller than the hole so getting a broken one out isn't a big deal.

Down side is that the single-point thread mills are slower than a regular tap, and kind of pricey ($25-50 for a 1/4-20 to 56TPI). Big deal, right?


----------



## MontanaAardvark

Thanks for the info on that.  I essentially just know what thread milling is, but haven't looked at doing it.  Since the majority of things I thread are fairly small holes, I was just concerned with tapping by hand.  Right now, I have four holes to tap in 4-40 and two to tap 10-32in my tooling plate.  I thought all of those are too small for a thread mill.   The G0704 being limited to about 2300 RPM is a detriment, too.    

I had a rude surprise, yesterday.  I pulled my vise off the mill so I can set up to trim my Rev 1 tooling plate to size.  The bottom of the vise and the mill table were both rusty.   I think I've used my Fogbuster for only a few hours.  For sure, I'm still on the first quart and the whole system has only been working since Mid-April.  




I'm using the Kool-Mist brand fluid.  One of the reasons I bought it was they say it's non-corrosive and a few reviewers on MSC said that they didn't have any rust with it.   One reviewer said he adds a little alcohol to the mix to prevent growth of slime that encourages rust. 

I sprayed the vise bottom with WD-40 and rubbed it lightly with wet/dry sandpaper.  400 grit, I think.  Did the same to the table.  It seems deeper than pure surface stain.


----------



## jbolt

I have no experience with the Kool-mist fliuid. I have used a formula from Tormach, Rustlick 5050 and KoolRite 2290. Of the three the KoolRite 2290 is by far the best I have used for being operator friendly and machine friendly. The Tormach fluid  had a strong odor and irritated my skin, the Rustlick 5050 has a mild odor and was easy on my skin but stained every thing, had some light rust issues and was an excellent paint & adhesive remover. With the KoolRite 2290 I have had no rust issues, has a mild odor and does not remove paint or bother my skin.


----------



## MontanaAardvark

jbolt said:


> I have no experience with the Kool-mist fliuid. I have used a formula from Tormach, Rustlick 5050 and KoolRite 2290. Of the three the KoolRite 2290 is by far the best I have used for being operator friendly and machine friendly. The Tormach fluid  had a strong odor and irritated my skin, the Rustlick 5050 has a mild odor and was easy on my skin but stained every thing, had some light rust issues and was an excellent paint & adhesive remover. With the KoolRite 2290 I have had no rust issues, has a mild odor and does not remove paint or bother my skin.



I noticed a spot on my powder coated hardware yesterday, thought it was a drip of loctite and promptly pulled up a strip of paint when I rubbed it with a fingernail.  I didn't think it might be related to the Kool Mist spray.

I hadn't put 2+2 together about that.  

Thanks as always, Jay.


----------



## jbolt

The Rustlick 5050 attacked the paint and the body filler under it. It was quite amazing where that coolant would get into. On a machine with flood coolant I'm not too concerned how it looks as long as it functions properly. Rust isn't cool. Staining or darkening is okay but not pitting. 

I also wonder how the chemical makeup of the city water affects different coolants. I'm sure there are papers on this.


----------



## spumco

I find that wiping everything down with FluidFilm before installing a vise or whatever seems to help.  I have wicked condensation problems in my garage from time to time, and have spent 2-3 weekends with greenie-weenies getting all my lathe chucks and collets un-funked.

I'm using flood coolant at a pretty high concentration in the mill so I haven't seen any rust inside since I started using fluid film once in a while.

You can get threadmills down to #2; they look like expensive little needles with an itty-bitty head.  Frankly, I'd rather trust a threadmill that small than a tap.  http://www.lakeshorecarbide.com/singleprofileuncoatedthreadmills.aspx

-S


----------



## Boswell

I have used at CoolMist formula for at least a year (now in  fog buster setup) but have not had ANY rust or discoloration. I use rainwater to mix the concentrate with a neutral PH.


----------



## TomS

jbolt said:


> The Rustlick 5050 attacked the paint and the body filler under it. It was quite amazing where that coolant would get into. On a machine with flood coolant I'm not too concerned how it looks as long as it functions properly. Rust isn't cool. Staining or darkening is okay but not pitting.
> 
> I also wonder how the chemical makeup of the city water affects different coolants. I'm sure there are papers on this.



Jay - you raise a good point about the chemical differences of tap water.  I use Rustlick 5050 mixed at 30:1 and haven't experienced any issues with rust.  Removed my vise earlier this week that has been on the table for three or four months.  No rust and only minor discolorization on the table.  Must be the northern Cal water!

I use Kool-Mist in my Fog Buster and rust is a problem.  Removing the vise and wiping down the table with oil is what I do.  A real pain.

Tom S.


----------



## jbolt

TomS said:


> Jay - you raise a good point about the chemical differences of tap water.  I use Rustlick 5050 mixed at 30:1 and haven't experienced any issues with rust.  Removed my vise earlier this week that has been on the table for three or four months.  No rust and only minor discolorization on the table.  Must be the northern Cal water!
> 
> I use Kool-Mist in my Fog Buster and rust is a problem.  Removing the vise and wiping down the table with oil is what I do.  A real pain.
> 
> Tom S.



Our water comes from various sources so you never now what the makeup is. I ran the Rustlick as high as 5:1 and still had problems. Also left the machine sticky.

The Koolrite 2290 is mixed at 7.5:1 per manufacturer. They give no ranges just 7.5:1 for everything. Drys super fast with little residue.

Why not use the Rustlick in the fog Buster?


----------



## MontanaAardvark

spumco said:


> I find that wiping everything down with FluidFilm before installing a vise or whatever seems to help.  I have wicked condensation problems in my garage from time to time, and have spent 2-3 weekends with greenie-weenies getting all my lathe chucks and collets un-funked.
> 
> I'm using flood coolant at a pretty high concentration in the mill so I haven't seen any rust inside since I started using fluid film once in a while.
> 
> You can get threadmills down to #2; they look like expensive little needles with an itty-bitty head.  Frankly, I'd rather trust a threadmill that small than a tap.  http://www.lakeshorecarbide.com/singleprofileuncoatedthreadmills.aspx
> 
> -S



I'm a boater - in saltwater - so I have some corrosion sprays and things around the house, I just didn't use any because I didn't think I needed it.  I thought the coolant had anti-corrosion additives in it.  

The FluidFilm says it's lanolin-based, so compared to something like WD-40, I'd guess it's a thicker, waxy film.  That's like LPS3, but I just checked and don't see any.  I know I used to have a can, so I must have used it up.  I have some CRC Marine 6-26, which is more like WD-40 but a bit thicker and won't destroy electrical insulators.  (I had WD-40 eat through spark plug wires on an outboard years ago).  CRC 6-26 is really popular for boats, trailers, RVs and such, but I've never thought of trying it for this.  

Lanolin?  I could rub the vise with a Chap Stick.


----------



## TomS

jbolt said:


> Our water comes from various sources so you never now what the makeup is. I ran the Rustlick as high as 5:1 and still had problems. Also left the machine sticky.
> 
> The Koolrite 2290 is mixed at 7.5:1 per manufacturer. They give no ranges just 7.5:1 for everything. Drys super fast with little residue.
> 
> Why not use the Rustlick in the fog Buster?



My fog buster is on the manual mill and I use it very little.  Just haven't got around to changing it out.

Tom S.


----------



## spumco

MontanaAardvark said:


> I'm a boater - in saltwater - so I have some corrosion sprays and things around the house, I just didn't use any because I didn't think I needed it.  I thought the coolant had anti-corrosion additives in it.
> 
> The FluidFilm says it's lanolin-based, so compared to something like WD-40, I'd guess it's a thicker, waxy film.  That's like LPS3, but I just checked and don't see any.  I know I used to have a can, so I must have used it up.  I have some CRC Marine 6-26, which is more like WD-40 but a bit thicker and won't destroy electrical insulators.  (I had WD-40 eat through spark plug wires on an outboard years ago).  CRC 6-26 is really popular for boats, trailers, RVs and such, but I've never thought of trying it for this.
> 
> Lanolin?  I could rub the vise with a Chap Stick.



Fluid film is more like soupy sour cream in viscosity.  It doesn't dry like a wax.  Just wipe/brush or spray some on and smear it around.  Smells like sheep, which might be a bonus for some folks.  It wets out nicely and the capillary action is pretty helpful around screw heads and similar crevices.  Set your slimy rag aside when you're done and use it again from time to time to wipe everything down.  I suspect it may be like like other oils and if you have a pile of them then keep them in a fireproof steel rag bin if they're really juicy.

Crevice corrosion is the killer on these machines.  Anywhere you get oxygen exclusion you'll get a corrosion cell forming - especially if there's a helpful electrolyte like water or coolant.

Same thing for galvanic corrosion - that's why I mentioned using stand-offs on the aluminum fixture plate you were talking about earlier.  If you don't paint or anodize it and just bolt it to the iron table, you'll be very, very sorry if you leave it there for a while if you're using a water-based coolant or mister.  Fluid film and other barrier films/oils aren't as effective as an actual electrical insulator (aluminum oxide) against galvanic corrosion when the two materials are very far apart on the galvanic chart.

And unlike the zincs anodes in your boat, the iron will become the anode and your table will pit badly.


----------



## MontanaAardvark

spumco said:


> Fluid film is more like soupy sour cream in viscosity.  It doesn't dry like a wax.  Just wipe/brush or spray some on and smear it around.  Smells like sheep, which might be a bonus for some folks.  It wets out nicely and the capillary action is pretty helpful around screw heads and similar crevices.  Set your slimy rag aside when you're done and use it again from time to time to wipe everything down.  I suspect it may be like like other oils and if you have a pile of them then keep them in a fireproof steel rag bin if they're really juicy.
> 
> Crevice corrosion is the killer on these machines.  Anywhere you get oxygen exclusion you'll get a corrosion cell forming - especially if there's a helpful electrolyte like water or coolant.
> 
> Same thing for galvanic corrosion - that's why I mentioned using stand-offs on the aluminum fixture plate you were talking about earlier.  If you don't paint or anodize it and just bolt it to the iron table, you'll be very, very sorry if you leave it there for a while if you're using a water-based coolant or mister.  Fluid film and other barrier films/oils aren't as effective as an actual electrical insulator (aluminum oxide) against galvanic corrosion when the two materials are very far apart on the galvanic chart.
> 
> And unlike the zincs anodes in your boat, the iron will become the anode and your table will pit badly.



Thanks for that.  I have the aluminum plate mounted to the table now, and overnight.  The fog was never on, so it should be safe.  I was getting ready to make a test cut on aluminum with a different hold down method, but after working on setting up to do it yesterday, I'm having second thoughts now.   

I'm making a GB-22, a single shot 22 pistol that Mark Serbu posted to YouTube several months ago.   The frame is a 3/16" steel plate, and I'm going to hold the work down on the tooling plate with the two 10-32 screws in the grip.  I'm not sure if this is going to work, so I'm going to take a practice cut in a piece of aluminum.  It's only a 1/16" aluminum plate, so I can't really emulate cutting the whole thing and I'm having misgivings about trying it already.  Much of the cut is right near those two screws, but there's a cutout up where the 1/16 piece sticks over the end of the tooling plate.  I can visualize the 1/16" piece bending down with nothing to support it.  I'm afraid this cut might end up meaning nothing.     

If I make that cut, the Fogbuster will be on, so I'll take the big aluminum plate off the mill after that.   




Bob


----------



## MontanaAardvark

The test cut was uneventful.  At some point, I told myself, "this is a test piece - it doesn't matter if you add some more holes".  So I put in two new holes and used 1/8" spring pins to hold everything together, along with the three other screws that were already there.




I think it's time to move on to the real, steel work piece.  I'm not sure if I'm going to use the same tool plate, but I took it off the mill and wiped everything down with some oil.


----------



## Groundhog

I've used Trim C-350 coolant/lube in my cnc mill for years. When I lived in Idaho I just mixed it with tap water and did not have rust problems. Moved to Kansas and had immediate rust with tap water. Switch to distilled water (@ $1 a gallon) to mix with my C-350 and no more rust problems.


----------



## MontanaAardvark

Groundhog said:


> I've used Trim C-350 coolant/lube in my cnc mill for years. When I lived in Idaho I just mixed it with tap water and did not have rust problems. Moved to Kansas and had immediate rust with tap water. Switch to distilled water (@ $1 a gallon) to mix with my C-350 and no more rust problems.



That's a cheap experiment, which is my favorite kind.  I'll try that.  I'm still on my first quart, so I think a gallon will last a while.


----------



## spumco

When I wrote that you might get galvanic corrosion, I didn't mean overnight.  I meant leaving it on for weeks or months without any sort of insulator or barrier.

If the steel is less friendly than the aluminum, maybe a really sharp HSS endmill would be better than carbide.  Lower tool pressure would be a good thing here.  Something else could be to add some back-up blocks to the sides opposite the cuts.  Run the profile in two operations and remove the blocks when they're in the way.  Some mitee-bite clamps (or similar) would be pretty cool here to act as a stop if the screws start to flex from tool pressure.

Another thing...  once you have the steel main receiver/grip OD profiled, you could cut a matching profile in the aluminum plate about .125 deep and recess the frame  in it to keep it from moving around.  I foresee some chatter when you cut that long trigger spring section if the trigger/spring isn't held down with a little top clamp or something.  It'll vibrate like a tuning fork.  If it's not already in the $12 instructions, I'd suggest cutting the trigger free from the frame (at the front) as the very last operation.  Same thing for the frame cut-out for the barrel assembly.

Finally, is there some reason you can't up-size the 10-32 screws?  they don't ride on anything and it looks like you've got room for some 1/4-28's or even 5/16" screws to hold the slide sections together.  You could even use shoulder screws and ream the holes to get rid of any slop while you're holding them to the fixture plate.  If it were me, I'd make them out of thicker stock, hold them in the vise on tall parallels for the profile and top features, and then flip & face and do the back side spring groove.  No fixture plate needed for the slide sections.

If you're going to make more than one, mill some soft jaws for the slide sections and bang out 5 or 10 of each component in no time - no having to re-indicate between each section.

As for the GB-22...  this looks like an open bolt action.  For a single shot, won't the bolt sliding forward bugger the accuracy?  And what is the barrel/liner?

Please tell me you're going to thread the barrel and put a can on it.  That'd be a sweet little rat gun.


----------



## MontanaAardvark

I understand the galvanic corrosion.  I've had a couple of aluminum boats and had to learn about that (some of it the hard way).  

There's a lot in your comments.  The barrel is a rifled barrel that I got from an eBay seller, but not threaded for a can.  I've never gone down that road, and don't think I will here.  My plan is to finish this prototype and then build a nice looking one for my wife.  The GB-22's designer came up with a closed bolt version that's cooler - there's a video on YouTube.  Everyone is hoping he updates the plans, or offers them.  I'm on the mailing list and haven't heard anything.   If those plans come out sometime soon, I'm thinking I may end up building two of those, if I can't just modify the first two.  


I've always planned to cut that slot (3/32) between the trigger and rest of the frame last.  I have another large chunk of the aluminum (tooling plate) that is wider than my table and will allow me to put 1/8" pins in all four of the holes where the barrel goes.  I think that will keep that area from moving.  Those spring pins had to be hammered in and pulled out with Vise Grips, a fulcrum, and the same hammer.  Making the holes for the grip screws bigger seems possible, and with no penalty.  I need to look at what hardware I have.  

Right now, I have three CAM files: a rough cut that you can see the results of above.  That's just one pass, because the Al plate is thinner than the steel is.  I have a fine cut file that uses a 1/4" EM and cuts the main shapes to size.  And I figured I'd follow that with the trigger cut file, using a 1/8" EM.  It cuts around the trigger and that long slot to the left.  The last operation is to cut the 3/32 channel between the trigger and the rest of the frame.   Perhaps I should cut the 1/8" EM file first, since everything will be completely supported in that area while cutting.


Bob


----------



## spumco

Cool.  I think you're in business with the order of operations.

I'd just hate to see the cartridge walk out a little bit before the bolt slams forward and have an out of battery ignition.  If you're going to use it, and not just use it for buy-back bait, then keeping the chamber a little dirty might not be a bad thing.


----------



## MontanaAardvark

I think Mark's idea was to put together something that can be fired for $20 or so.  As a manufacturer, he has better source of materials than I do.  When you figure shipping, I had to buy enough to make four with minimum quantities, and pay shipping.  If you spread that out over four, I'm right around $50 each.  There has never been a buyback around here, so it's going to be a toy to play with a few times.  

The extra work on the mill and weeks of machining lessons are not included.


----------



## MontanaAardvark

Update, anyone?  The frame is cutout, all the pieces are done and I'm waiting on one part to put it all together and do a test.  It's the spring that makes the thing work.  




The whole piece was indexed from the screw holes in the test piece I cut.  

This is a new 20 x 7-1/4, half inch aluminum plate.   I'm thinking of options for making it semi-permanent, or my default plate.   Either drilling and tapping lots of 3/8-16 holes along with 1/8" tooling pins (because I have a box of them), or something else.  I'm not sure what.  

Now it's back to more mill update plans and projects.  I'm feeling the need to upgrade the motor and/or controller.  Higher RPMs for the same power would be really nice to have; CNC control of on/off and RPMs might even be better.  Higher RPMs might be different gears, but I don't know the options.


----------



## spumco

Sweet.

I figured we should start a new thread since this is straying off the 'ease of use' topic, but you keep posting cool stuff and I'm a sucker.

As for the mill, yes.  Do all of the above, you won't regret it.  CNC control of the spindle is pretty easy.  Does your BOB support/have a 0-10v PWM output?

While you're shopping for motors, do yourself a favor and plan on getting an encoder so you can rigid tap...  Or at least a spindle index sensor.  You can make an index trigger from an inductive sensor (limit switch) and a dumb old chunk of plastic pressed on the top of your spindle like a collar.  Use set screws to trigger the sensor, and use 2 or 4 of them for balance.  Mach3 can handle multiple index signals, and more is better for tapping.

Basic shopping list for nirvana:
*- 1-2HP Motor w/encoder.*  If you get a really good one that has a 1000:1 constant torque rating you won't need a two-speed belt drive to do low-speed hogging and high-speed small end mills.  You can fit an encoder that's WAY cheaper than the one that comes on the BlackMax motor.  Really, you can fit a 56C sized motor on top.  I managed to get a 182 on mine, but mine's bigger than yours....

If you're worried about 1HP being undersized, don't.  Good-quality motors are way under-rated, compared to the grossly-overrated cheap motors.  I 'only' have 2HP, but I'd have no problem snapping a 1/2" tap in steel at 500RPM, or running a 3/8 3-flute in aluminum at 7k.  Piles of chips, no gear or belt changes.

Here's a peach: https://www.automationdirect.com/ad...0HP)/Marathon_Black_Max_(0.25HP_to_30HP)/Y535

And another, WITH an encoder already on it: http://www.ebay.com/itm/Marathon-1h...616518?hash=item282e7cb4c6:g:TRUAAOSw4CFYytt9

*- Belt drive.*  Figure out your top speed, based on your bearings and smallest intended end mill speed.  I can go to about 7400RPM before I chicken out, but I expect my bearing to die sooner rather than later, and then I'll replace them with really good ones.  If you get an 1800RPM motor, and run it up to 5400RPM with the VFD (max safe RPM on that BlackMax), then a 1:1.3 or 1.4 belt drive should work well to get you to 7500RPM.  A single-speed belt drive is way easy to sort out, and the cogged sheaves are pretty cheap and easy to get.  You won't regret ditching the gear system, and you might even sell the gear set to someone as a replacement or backup.

*- VFD.*  I got a Hitachi WJ200 and love it.  However, the Automation Direct GS-3 VFD's have an optional encoder input card  - for a bit more money - that is superb.  Takes 3-24VDC complimentary inputs and can work with very high speed encoders.  Not something I realized when I bought my Hitachi was that the WJ200 is very limited in the encoder inputs.  It's superb otherwise, and can even do positioning (servo-ish).  Doing it again, I'd spend the extra $50-100 for the GS-3 VFD just to avoid the encoder input compatibility issues I had to work out.

Even if you don't get an encoder, buy the best-quality motor you can and make sure it has the capability of accepting an encoder later on.

The other option, of course, is to throw down on a servo spindle.

DMM's 1HP, 5kRPM servo: https://store.dmm-tech.com/products/dst-0-75kw-ac-servo-motor

And the matching drive: https://store.dmm-tech.com/products/dyn4-h01a2-00-dyn4-ac-servo-drive?variant=20982430342

That combo would be rally, really sweet.  Unfortunately, their "big" servos just don't have the top speed I wanted without gearing them up too much and lose low-end torque for big drills and tapping.  For you, a 1HP servo would be pretty nice, and you might be able to find one on Fleabay.

Gold Standard: http://www.ebay.com/itm/Parker-J092...469419?hash=item33ce00786b:g:zfoAAOSw7GRZC3FQ

If you start a new thread "In Search Of the Ultimate G0704 Spindle"  I promise I'll chime in.


By the way, I successfully milled Grade 5 titanium for the first time today.  I'm still new at this, so it was pretty awesome watching the mill make something round in to a hex.  2750RPM, .625DOC, .025WOC (adaptive), 5.5ipm, .250" 4F.  Chips looked good, excuse the never-seize goo.

And yes, I've got an approved Form 1 for those who may be unable to control their urge to chime in about such things.

-S


----------



## MontanaAardvark

spumco said:


> Sweet.
> 
> I figured we should start a new thread since this is straying off the 'ease of use' topic, but you keep posting cool stuff and I'm a sucker.
> 
> As for the mill, yes.  Do all of the above, you won't regret it.  CNC control of the spindle is pretty easy.  Does your BOB support/have a 0-10v PWM output?
> 
> While you're shopping for motors, do yourself a favor and plan on getting an encoder so you can rigid tap...  Or at least a spindle index sensor.  You can make an index trigger from an inductive sensor (limit switch) and a dumb old chunk of plastic pressed on the top of your spindle like a collar.  Use set screws to trigger the sensor, and use 2 or 4 of them for balance.  Mach3 can handle multiple index signals, and more is better for tapping.
> 
> Basic shopping list for nirvana:
> *- 1-2HP Motor w/encoder.*  If you get a really good one that has a 1000:1 constant torque rating you won't need a two-speed belt drive to do low-speed hogging and high-speed small end mills.  You can fit an encoder that's WAY cheaper than the one that comes on the BlackMax motor.  Really, you can fit a 56C sized motor on top.  I managed to get a 182 on mine, but mine's bigger than yours....
> 
> If you're worried about 1HP being undersized, don't.  Good-quality motors are way under-rated, compared to the grossly-overrated cheap motors.  I 'only' have 2HP, but I'd have no problem snapping a 1/2" tap in steel at 500RPM, or running a 3/8 3-flute in aluminum at 7k.  Piles of chips, no gear or belt changes.
> 
> Here's a peach: https://www.automationdirect.com/ad...0HP)/Marathon_Black_Max_(0.25HP_to_30HP)/Y535
> 
> And another, WITH an encoder already on it: http://www.ebay.com/itm/Marathon-1h...616518?hash=item282e7cb4c6:g:TRUAAOSw4CFYytt9
> 
> *- Belt drive.*  Figure out your top speed, based on your bearings and smallest intended end mill speed.  I can go to about 7400RPM before I chicken out, but I expect my bearing to die sooner rather than later, and then I'll replace them with really good ones.  If you get an 1800RPM motor, and run it up to 5400RPM with the VFD (max safe RPM on that BlackMax), then a 1:1.3 or 1.4 belt drive should work well to get you to 7500RPM.  A single-speed belt drive is way easy to sort out, and the cogged sheaves are pretty cheap and easy to get.  You won't regret ditching the gear system, and you might even sell the gear set to someone as a replacement or backup.
> 
> *- VFD.*  I got a Hitachi WJ200 and love it.  However, the Automation Direct GS-3 VFD's have an optional encoder input card  - for a bit more money - that is superb.  Takes 3-24VDC complimentary inputs and can work with very high speed encoders.  Not something I realized when I bought my Hitachi was that the WJ200 is very limited in the encoder inputs.  It's superb otherwise, and can even do positioning (servo-ish).  Doing it again, I'd spend the extra $50-100 for the GS-3 VFD just to avoid the encoder input compatibility issues I had to work out.
> 
> Even if you don't get an encoder, buy the best-quality motor you can and make sure it has the capability of accepting an encoder later on.
> 
> The other option, of course, is to throw down on a servo spindle.
> 
> DMM's 1HP, 5kRPM servo: https://store.dmm-tech.com/products/dst-0-75kw-ac-servo-motor
> 
> And the matching drive: https://store.dmm-tech.com/products/dyn4-h01a2-00-dyn4-ac-servo-drive?variant=20982430342
> 
> That combo would be rally, really sweet.  Unfortunately, their "big" servos just don't have the top speed I wanted without gearing them up too much and lose low-end torque for big drills and tapping.  For you, a 1HP servo would be pretty nice, and you might be able to find one on Fleabay.
> 
> Gold Standard: http://www.ebay.com/itm/Parker-J092...469419?hash=item33ce00786b:g:zfoAAOSw7GRZC3FQ
> 
> If you start a new thread "In Search Of the Ultimate G0704 Spindle"  I promise I'll chime in.
> 
> 
> By the way, I successfully milled Grade 5 titanium for the first time today.  I'm still new at this, so it was pretty awesome watching the mill make something round in to a hex.  2750RPM, .625DOC, .025WOC (adaptive), 5.5ipm, .250" 4F.  Chips looked good, excuse the never-seize goo.
> 
> And yes, I've got an approved Form 1 for those who may be unable to control their urge to chime in about such things.
> 
> -S
> View attachment 233519




Let me get this straight: that hex head on the cap was once solid round titanium bar and you cut it to final size hex bolt head?  That's very cool.  Especially 5/8" DOC, skinning off .025 at a time.  

I've cut titanium on my Sherline mill and lathe: 1/8 HP.  Much lighter cuts.  OTOH, I thought it machined a lot like the couple of pieces of stainless I had cut by then (long ago).

The rest of this is encyclopedic!  I really should start an "Ultimate G0704 Update" thread, although I'm sure other people want things I don't.  I was looking at Hoss' DVD again, at the supplemental projects and in particular the manual drawbar, which is probably going to be a high priority project so I can start on the TTS.  He's using this motor, which is 5000 RPM, 120VAC and 1200 W input (1HP output), but has no encoder.  

I think my goal would be what the Tormach PCNC 770 says it's using: 1HP, 10,000 RPM.   I'd settle for 7500 RPM, for sure.  Those machines are in the same work envelope class as the G0704 and are rated for a 120V 15A outlet.  I don't consider 1HP underpowered and will be happy to live with that.  Putting a 2HP motor on a machine in place of a 1 HP motor doesn't make it a 2HP mill - at least in my mind.  The mill is a system and has to be rigid enough to handle the motor that size, and that extends to every part, including the ballscrews I just put in.  

I have a 220 VAC outlet near the mill, but I think it's conventional 220 not three phase.  

My BoB has digital outputs and inputs but not a PWM encoded output.  



Bob


----------



## spumco

The chunk started as 1.25"OD  bar stock.  I turned the OD and ID threads and turned a .750 spigot.  I then milled the spigot in to the 5/8" hex on the mill.  Held it in a step collet that I bored to hold the threaded section - the little flange registered against the collet face and helped keep it rigid.  It was only a couple of .025" passes since I wasn't going from 1.25 to .625.  It turns out that getting the RPM and chipload correct for that material is the key - not that I figured anything out.  I just pressed the "I Believe" button on the F&S calculator.



MontanaAardvark said:


> I have a 220 VAC outlet near the mill, but I think it's conventional 220 not three phase.



The VFD's in the HP range you'll need convert 220V 1P to 220V 3P.  They're like magical little computers with million page instruction manuals.

What BOB do you have?  If you've got a part number or model number I can check the specs and see what we can do with it.

And I think 'encoded output' may be a misnomer or a term I'm not familiar with.  Some BOB's can take a digital PWM signal from Mach3 parallel port or your ESS and convert it to a 0-10vdc output.  VFD's usually require one of three input types to set the speed:
1. 0-10vdc (common hobby method)
2. 4-20mA (common industrial method, more RFI/noise resistant than 0-10vdc)
3. Pulse + direction signals (rare in hobby world.  You would use the output from an encoder - maybe on a conveyor belt roller - to drive a different VFD/motor combination probably at some speed ratio to the primary device).

If your BOB really doesn't have a 0-10vdc output capability, there are spindle control sub-boards available to connect your ESS/BOB to the VFD.  Or you could also get a new BOB that has a built-in PWM output and it would probably be an upgrade to your existing BOB with more inputs/outputs for your future auto tool changer, power drawbar, glass scale feedback for full closed loop operation, servo drive encoder signals, coolant, mister, auto oiler, and the kitchen sink timer.

You can NEVER have enough inputs/outputs.


----------



## MontanaAardvark

I have the C35S from CNC4PC.com.  I have the manual .pdf and searched for PWM, motor control, and a few other terms. 

I'd rather not go down the road of the VFD unless I have to, though.  Like I say, I'm OK with 1 HP and that size plugs into the 115V typical wall socket just fine.


----------



## spumco

You're right: the C35S doesn't have onboard spindle control.  You have two options for computer control - simple on/off and you set the speed manually, or full control.  If you're going to upgrade, I wouldn't bother with the simple relays-to-the-motor setup.  Having the computer set the speed and direction isn't hard or expensive.

For full control, you could get a C41 or C69 board from CNC4PC and mount it as a daughter-board on your C35S, but you'll still need to figure out what motor/controller combo (OEM or otherwise) you want and whether the OEM can use a PWM input.

As for the VFD, they're available - and cheaper for lower power - in whatever HP rating you need for your motor choice.  You need one if you switch to a 220-3P motor, regardless of HP.  The nice thing about moving to 220-3P  is that the motors are quieter, generally better built, and use fewer amps per horsepower (smaller wire, less heating) than the equivalent 110-1P.

If you prefer to stick with the OEM motor, there are a ton of resources available to help you set it up under CNC control.  Smarter folks than me have written tons about upgrading your mill.  Poke around on the Mach3 forum and CNCZone and you'll find what you need.  If you followed Hoss' plans for your conversion, you should go straight to his site and just copy whatever he did for spindle control.  That guy is frikkin' clever.

If you want to move to a non-stock 3P motor & VFD combo, I can help a bit.  Also, if you want to upgrade your BOB to something with on-board spindle control, I have an unused C23 available at a steep discount.


----------



## MontanaAardvark

I spent a few hours in the last couple of days getting my fourth axis running.  I'd wanted to add a rotary table since the start of the project and have added parts along the way.  Pretty much every time I bought needed parts, I got extras for the fourth axis.  I picked up the 6" rotary table itself last November on a Black Friday sale at Wholesale Tool, and everything has been sitting in a corner while I finished CNC converting the mill.  

I had a leftover NEMA23 motor mount from when I started out doing Hoss' Phase 1 conversion, and two sets of standoffs.  I had both too long and too short.  All I had to do was figure out how to get the hand crank off the table, then drill and tap two holes in it and two clearance holes in the motor mount.  And cut four standoffs down to size.  



Tweaked the Mach3 Motor Tunings in and it works fine.  I can't actually use it yet, because I don't have any Tee nuts that fit the slots on it.  A 7/16 nut from my mill is too big, so I'd guess a 3/8" Tee nut would fit it.  There's probably a complete clamping set for that size slot out there somewhere.   Minor annoyance in Mach3: it interprets the IPM numbers in feed as degrees per minute.  If I'm running 1.3 IPM, like I was for the small slot in steel, then told the table to go 90 degrees, that move would take an hour and a half.  When I was testing this, I ended up at 3600 degrees/minute to run 90 degrees in a "reasonable" time - about 5 seconds including acceleration and deceleration 

My only gripe with the motor on the G0704 is the speed, although it also seems kind of noisy to me.  The spindle runs smoothly and while I measured the runout when it was new, I don't recall anything bad.  The part that sticks out of the top of the headstock and has the bolt for the collets or EM holders has a very pronounced wobble to it, though.  I assume noise translates into losses (friction) in the bearings.  A quieter, smoother motor would be nice.  I don't know that the motor is too noisy.  It's not like I feel I need hearing protection, and I'd be pretty sure it's quieter than a lot of other tools like my table saw.

Time to do more reading and research.


----------



## spumco

1.  Awesome.  Figuring out - sort of - 4th axis CAM has been challenging for me.  Manual indexing is easy, but getting the integration between operations has been fussy (my post processor is wonky and I don't know how to edit it very well).

2. I'm in the same boat for speeds since mine is also based on a worm-drive table.  Mine was CNC from the get-go, but is also slow.  I suggest you bump the max speed after ensuring you have good lube in the gearbox.  I ended up at about 15RPM before it becomes unreliable.  Another good tweak to increase the rotation speed is to bump the max feed rate but cut way back on acceleration.  This allows the backlash to be taken up from a standstill (or direction change) without binding the gears and losing steps.   I have also a 90:1 ratio and can get 15RPM - whatever that is in steps/degree/second.  This setting will, of course, depend on your microstepping and gear ratio, but I suspect you can go a bit faster if you cut back and not slam the gears.  The nice thing is that while you're fiddling around with the speed settings if you top out and stall the stepper - no harm done.  That NEMA 23 won't strip the gears.  Just make sure you adjust the backlash as close as you can without binding and keep an eye on it from time to time.

T-nuts - this is a Chinese rotary table so you probably have metric T-slots.  My guess is a M8x12 T-slot, but set your caliper to metric and measure the height, width, and side slots.  I just bought some from J.W. Winco - they were considerably cheaper than anywhere else online.  An alternative is to mill down a 3/8 if it doesn't quite fit right-  but it should go in there a little sloppy.

3. 





MontanaAardvark said:


> My only gripe with the motor on the G0704 is the speed, although it also seems kind of noisy to me.



Told you so.  Single phase motors are noisy, and you've got that gear set in there screaming away.  Your table saw is even louder because it's probably a 3600RPM thing, and your mill motor is turning at half that.  Belt-drive and 3 phase motor or brushless DC would be your friend here.

4. 





MontanaAardvark said:


> The part that sticks out of the top of the headstock and has the bolt for the collets or EM holders



That doo-dad is called a drawbar.  And at the max RPM you have available, the wobble isn't going to roach your bearings any time soon.  It will drive you crazy watching it, however; mine did the same thing.

What you do is make a new drawbar.  McMaster sells 7/16-20 grade 8/9 all-thread and extra-heavy nuts.  Pin and lock-tite the nut on the end, and make a big-old pair of bearing plates that are a close fit on the all-thread.  Bottom bearing plate gets a shoulder turned to fit inside your spindle with a little clearance so it runs true.  Top one is same size as the bottom one OD (spindle OD).  Polish the contact faces, harden them with a torch & oil, and re-polish.  Add some never-seize to the threads, bearing plates, and collet taper and you'll never have to look at the cheap wobbly drawbar again.  And you'll have enough all-thread left over to make a second one when you wear out the first.  And use a torque wrench to tighten the drawbar - not a cheater.  Or get a cordless impact that can't go higher than about 15ft-lbs if you want a poor-man's power DB.

-S


----------



## MontanaAardvark

The thing about the rotary table that puzzles me is that I wrote down both decimal inches, and mm, and it doesn't strictly match anything. 




The width of the slot is 11.0 mm, the bottom width is 17.3mm, wide section height is 7.64mm and the narrow section height is 9.4mm. 

The dimensions look like a 3/8 slot except for the width of the bottom part (0.68).  Engineers' references say that should be bigger: 0.719 at minimum.   In metric, that slot with of 11 mm is halfway between M8 and M10 at 10 and 12mm, respectively.   Otherwise it looks like it would be M8, like you say.  Either way, one dimension messes up the match. 



The slot is just a bit tight on 7/16 (.438)  which is what I have for the 0704.  I can slide one of those nuts in the slot if the nut's upside down, but the bottom slot is too narrow and the bottom section height is too short for the 7/16 Tee-nut.  

I tried some hardware I have and found a 3/8-16 "hardware store" nut fits in width but is too tall for the slot.  A 3/8 bolt will fit in the slot, so I'd have threads sticking out instead of a nut in the slot. 

Not that there's anything wrong with that.  

Hoss has a video where he makes an adapter to mount a 6" four-jaw chuck on the table.  He made his own Tee nuts.   A four jaw might be a good thing to have on the rotary table for almost everything.


----------



## JimDawson

I just made T-nuts for mine.  A nice couple hour project.


----------



## spumco

That sounds like sloppy M8 slot.  The metric T-nuts are so cheap at JW Winco you should just buy some instead of making them.  If you try to kludge something in there that isn't an actual T-nut, you could put an angular strain on the slot and possibly crack the slot lip.  

Unless you want to put miles on an end mill just for fun.  I actually have to skim about .025" off the bottom of some of my table T-nuts, but that's just a single skim pass off the bottom.  You're talking about facing the stock, profiling the shoulders, flipping and facing again, then drilling and tapping before finally cutting to length and deburring.  (all that x2 if you want a couple of spares)  That's quite bit of work for some stupid nuts that are $2.42 each and can be in your hands in a couple of days.

As for the chuck - you can fit a 6" chuck on it, but I'd recommend thinking about a 4" or 5" instead.  Check your jaw clearance to the table with the proposed 6" chuck and see if it's even possible to hold something that big with the jaws spread out on the OD.  In addition, the further you get away from the A axis centerline the less rigid your setup will be.  You don't have a brake on your 4th spindle.  Ok, you do have two brakes, but what happens when you forget to loosen them before the next move?  Or if you're doing 3D contouring with continuous rotation?  Any machining offset from the A centerline will have gobs of torque on the 4th axis  - and a 3" off-set (6" part) may be a bit much for a rigid setup.

Finally, how would you even mount the 6" chuck to the backing plate and then mount the backer to the faceplate?  At that point you just get a front-mount chuck and be done with it.

Another thing to consider - get two-piece jaws.  That way you can swap between OD and ID without having to rotate the chuck to get clearance for the bottom ones to come out.  Another benefit of a smaller chuck is that you may have clearance to pull the bottom jaws without rotating.

If you want to do something big, make a trunnion table that bolts to the faceplate and is stabilized outboard by a tailstock or something.  This will get the part closer to the centerline.

I'm now seriously considering making another adapter and adding a 3-jaw chuck to the collection. That, or a front-mount chuck.   Because of the mounting system it'd be fairly easy to dial it in very concentric (vs. on a lathe where you're sort-of screwed if it isn't true).  I got the 4-jaw to hold square stuff, and I like it, but dialing in a part is painful.  With only 15RPM available it takes FOREVER to get something running true.  My 4th doesn't have the ability to unlock the worm, unlike the expensive grown-up HAAS or other commercial ones.  For quicky jobs that don't have to be dead-perfect, a 3-jaw would be an order of magnitude faster.

I mounted mine using flat head socket screws with conical bearing washers (also from JW Winco) so they sit flush but have a nice big holding surface. Every little bit helps with clearance.

Backing plate was 7"x7" .875" stock, and I did all the ops from the top side holding on to about .125" of the stock.  Flipped it over and ran a profile around the outside before facing off the back parallel to the front.  Profile was to avoid having the facemill plow through a bunch of unsupported stock and chatter like mad on the last .010".  Counter-sunk the chuck mounting screws (M8 flat head) by hand on the work bench - easier than taking forever to indicate the holes after the flip.

Things to consider based on my mistakes and having used it a few times now:
- give yourself enough slop on the backing plate to face plate mounting holes to nudge it true.
- pick a chuck and bore the mounting plate center hole larger than the chuck hole.  Gives you access to the 2 or 3 MT taper in the spindle for all sorts of good reasons.  Also think about boring it to some known exact diameter to use as an indicating surface.  It doesn't have to be bored with a boring bar - drill a starter hole and hog out the hole with an end mill.
- keep it as thin as you can without any flex.  More clearance is better and less overhang is very nice.

-S


----------



## spumco

As for your spindle motor - read this, please.

http://www.cnczone.com/forums/benchtop-machines/290706-g0704-vfd-ac-motor-upgrade-information.html


----------



## MontanaAardvark

spumco said:


> That sounds like sloppy M8 slot.  The metric T-nuts are so cheap at JW Winco you should just buy some instead of making them.  If you try to kludge something in there that isn't an actual T-nut, you could put an angular strain on the slot and possibly crack the slot lip.
> 
> Unless you want to put miles on an end mill just for fun.  I actually have to skim about .025" off the bottom of some of my table T-nuts, but that's just a single skim pass off the bottom.  You're talking about facing the stock, profiling the shoulders, flipping and facing again, then drilling and tapping before finally cutting to length and deburring.  (all that x2 if you want a couple of spares)  That's quite bit of work for some stupid nuts that are $2.42 each and can be in your hands in a couple of days.
> 
> As for the chuck - you can fit a 6" chuck on it, but I'd recommend thinking about a 4" or 5" instead.  Check your jaw clearance to the table with the proposed 6" chuck and see if it's even possible to hold something that big with the jaws spread out on the OD.  In addition, the further you get away from the A axis centerline the less rigid your setup will be.  You don't have a brake on your 4th spindle.  Ok, you do have two brakes, but what happens when you forget to loosen them before the next move?  Or if you're doing 3D contouring with continuous rotation?  Any machining offset from the A centerline will have gobs of torque on the 4th axis  - and a 3" off-set (6" part) may be a bit much for a rigid setup.
> 
> Finally, how would you even mount the 6" chuck to the backing plate and then mount the backer to the faceplate?  At that point you just get a front-mount chuck and be done with it.
> 
> Another thing to consider - get two-piece jaws.  That way you can swap between OD and ID without having to rotate the chuck to get clearance for the bottom ones to come out.  Another benefit of a smaller chuck is that you may have clearance to pull the bottom jaws without rotating.
> 
> If you want to do something big, make a trunnion table that bolts to the faceplate and is stabilized outboard by a tailstock or something.  This will get the part closer to the centerline.
> 
> I'm now seriously considering making another adapter and adding a 3-jaw chuck to the collection. That, or a front-mount chuck.   Because of the mounting system it'd be fairly easy to dial it in very concentric (vs. on a lathe where you're sort-of screwed if it isn't true).  I got the 4-jaw to hold square stuff, and I like it, but dialing in a part is painful.  With only 15RPM available it takes FOREVER to get something running true.  My 4th doesn't have the ability to unlock the worm, unlike the expensive grown-up HAAS or other commercial ones.  For quicky jobs that don't have to be dead-perfect, a 3-jaw would be an order of magnitude faster.
> 
> I mounted mine using flat head socket screws with conical bearing washers (also from JW Winco) so they sit flush but have a nice big holding surface. Every little bit helps with clearance.
> 
> Backing plate was 7"x7" .875" stock, and I did all the ops from the top side holding on to about .125" of the stock.  Flipped it over and ran a profile around the outside before facing off the back parallel to the front.  Profile was to avoid having the facemill plow through a bunch of unsupported stock and chatter like mad on the last .010".  Counter-sunk the chuck mounting screws (M8 flat head) by hand on the work bench - easier than taking forever to indicate the holes after the flip.
> 
> Things to consider based on my mistakes and having used it a few times now:
> - give yourself enough slop on the backing plate to face plate mounting holes to nudge it true.
> - pick a chuck and bore the mounting plate center hole larger than the chuck hole.  Gives you access to the 2 or 3 MT taper in the spindle for all sorts of good reasons.  Also think about boring it to some known exact diameter to use as an indicating surface.  It doesn't have to be bored with a boring bar - drill a starter hole and hog out the hole with an end mill.
> - keep it as thin as you can without any flex.  More clearance is better and less overhang is very nice.
> 
> -S
> 
> View attachment 233650



As usual, lots to absorb here - and thanks for that.   I'm not decided on how to setup the rotary table.  Not by far.   I haven't even verified I'm getting the right number of degrees in a movement or checked it for backlash.  To to that, I need to attach something to the table. 

I have both three and four jaw chucks for my LMS lathe, but don't want to tie one up on the rotary table as they're both very useful on the lathe.  OTOH, Shars has several nice chucks in the 4" size class, and I could dedicate one of those.  I'm sure the same goes for other suppliers.  The table has an MT2 taper in it, so that's an option for mounting a chuck. It seems like clamps and Tee nuts are probably the most direct, secure method.  

On my Sherline's rotary table, I have both independent and scrolling four jaw chucks.  The scrolling 4-jaw isn't as accurate as the independent jaw, as you'd think, but it's pretty good.  Now that I say that, I don't recall the numbers.  These are 3" chucks.  It's a 4" rotary table.   

Thankfully, I have lots of options.  I occurs to me I could upgrade my big lathe to a 5" chuck and use the 4" chuck on the A-axis.  

I'm still working on the bulk of this thread: the tooling plate and tool changer questions.  Thanks for the motor/VFD reading on the CNCZone forum to go read.  

I'm also working on a problem on the Sherline mill, so I've been out in the shop trying to shim a gib.  It's 10 years old, and the gib is a plastic or composite, so it's probably worth it to just go get a few spares to have around the house.  If one is wearing out, there's bound to be another behind it.  


Bob


----------



## MontanaAardvark

I know it has been six months since anything was posted to this thread, but I wanted to add a followup in case anyone found it or was even still following the thread.  

I found that the slots on the Wholesale Tool 6" Rotary Table are 3/8".  While searching for parts, I found someone selling T-nuts that offered free cad files, and I could put the cad file of the T-nut in the cad file of the slot (see post #71).  

I searched a few tool places (Wholesale Tool, MSC Direct, Travers), and could only find a 3/8 clamping set at Little Machine Shop.  The quality is nothing to brag about.  I had to run a tap through the Tee nuts to clean up the excess coating on them, and had to hold onto the studs with big pliers and thread a nut onto them with a 3/8 drive ratchet to get them to thread on.  But it's a bunch of parts in one place for a clamping set.  It'll be OK now that I've finished the cleanup.  

So onto a project.  This is almost done.  




I drilled 3/8" holes in the flywheel for the little wobbler steam engine I built a few weeks ago.  I had this in mind from the moment I got it, so it's nice to have it done.  Needs a little finish work now to debur the holes and clean up the edges of the wheel, but I'll get that done as soon as I can.  

So, for anyone who cares, or has the RDX Rotary Table (or one like it) this the answer to some of the things I left hanging.  Now I want to measure the backlash and rotational accuracy of the table.


----------



## Bob Korves

MontanaAardvark said:


> Now I want to measure the backlash and rotational accuracy of the table.














All you wanted, and more!


----------



## MontanaAardvark

Bob Korves said:


> All you wanted, and more!



You're miles ahead of me, but I'll be saving those (only watched the first).  The way I think of it, I can hold something horizontally with my dial indicator and tell it to move 0.1 degree.  At 3 inches from the center (it's a 6" table), the end should move 3 sine(.1) or .0052".  If backlash is more than 1/10 of that (5 tenths) I think I'll see it.  I could always make the distance longer by bouncing a laser off a mirror several feet onto a wall.


----------



## MontanaAardvark

MontanaAardvark said:


> You're miles ahead of me, but I'll be saving those (only watched the first).  The way I think of it, I can hold something horizontally with my dial indicator and tell it to move 0.1 degree.  At 3 inches from the center (it's a 6" table), the end should move 3 sine(.1) or .0052".  If backlash is more than 1/10 of that (5 tenths) I think I'll see it.  I could always make the distance longer by bouncing a laser off a mirror several feet onto a wall.



Backlash is easily measured with a 6" steel bar clamped to the table and a dial indicator.  (The bar is longer than 6", but the indicator is set to measure movement there.  1 degree works out to .1047" and that was repeatable.) 




I measured .038 degrees backlash.  The table is 4 degrees per rotation of the shaft.  I have the typical 200 step motors, so 4/200 is .02 degrees per step, indicating two steps of the motor taken up in backlash.  I entered .038 in Mach3's backlash compensation and it seems to work repeatedly.  

Onward...


----------

