I made a Tool length thingy

[Dave SParticipant @daves59043]

Not really sure what to call this. It’s sort of a tool length indicator. Knocked it up this evening from stuff lying around 🙂

I am about to run some programs on my CNC. The bulk of the work is done with a 3mm endmill, but then the details are finished off with 1mm square and 1mm ball nose tools.
I have a direct ER16 spindle, so changing tools will introduce a length change, no matter how careful I am.

With this I can gage the length of the first tool, then after swapping bring the Z back to the same overall height and reset the CNC Z coordinate.

The platen is press fitted into the end of a linear bearing, which then runs on its shaft. There is a light spring under it to take the weight so the indicator is just moved by the bearing, not holding it up.

Repeats really well, in the region of 1 or 2 microns, which is nice.

Dave

 

[Martin KyteParticipant @martinkyte99762]

The commercial ones are generally called Z Axis dial height gauges or at least mine is.

[John HaineParticipant @johnhaine32865]

Or generically touch plates or buttons.  Are you actually probing or just viewing deflection on the indicator? Probing is cool, simple routine using a “G31” command brings down the tool very slowly ’til it touches, then you apply a tool offset based on the touch plate height.

[Dave SParticipant @daves59043]

Manually bringing the tool down to the same zero point on the indicator, then setting the Z. That way I don’t have to think much about actual measurement, just about repeatability.

Proper probing is probably next on the list, but I think I’ll need to electrically isolate the tool and the probe plate, which is another set of things – not to mention the wiring it up to the controller.

I also want to solve the initial x and y zeroing, I’m currently using rizlas but there must be a better way.

 

[JasonBModerator @jasonb]

I use an edge finder for X&Y or a dti on the spindle for round work. Both are flexible enough that if you make a wrong move they tend to to get damaged.

Probing again is probably the ideal for X&Y

[HollowpointParticipant @hollowpoint]

What you have made is a “tool height setter”or “z axis height setter”. 🙂

[Julie AnnParticipant @julieann]

On the CNC mill I use a Haimer Zero Master for X/Y probing and a Haimer Centro for picking up round features. For Z probing I use a home made master tool (tool 0) and a fag paper.

For normal CNC milling I use the Tormach quick change system. I set tool heights using an electronic tool height setter that fills in the tool table for each tool prior to machining. The g-code file then uses the tool height table when changing tools.

However I also have a seperate high speed head using ER11 collets. I suspect this has the same problem as that highlighted by the OP. When changing tools height information is lost. The g-code programs using this spindle do not refer to the tool height table as the numbers are meaningless. I get round the loss of height information in two ways. I try and only use one tool for a job. In general I try and minimise tool changes anyway as otherwise it means I have to nursemaid the CNC mill rather than going and doing something else. If I absolutely need more than one tool on the high speed spindle I fixture the parts so that I can do all parts with one tool and then change tool and do the second operation on all parts. That way I only need to do one tool change and measurement per batch instead of doing it for every part.

Julie

[NealebParticipant @nealeb]

Everyone seems to develop their own techniques based on knowledge, competence, what’s available, and pocket depth!

I mainly use a CNC mill. For XY and centring I either use a cheap and cheerful 3D electronic probe that came with the machine or a more traditional mechanical probe – the kind with a spring-loaded disc on the end of a shaft. The electronic one is used in conjunction with probing macros in the software which work well and can automatically probe various different geometries. The downside is that it is a pain to calibrate if the probe is changed (no, nothing to do with the user, they just spontaneously bend every so often. Honest). But, it does have a 6mm shank which fits my smaller, favourite, drill chuck and the larger shank on the mechanical probe doesn’t.

For Z,  I can also use the probe or it’s the tool+fag paper as above. It’s the tool-and-paper approach if it’s a single-tool job, but with either I can then tell the machine to go off and measure tool length with the electronic tool-setter. I have rewritten the M6 tool-change macro so that on tool change, the new tool is measured by the tool-setter and the Z coordinate set accordingly. Using either a drill chuck or ER32 collet there is no repeatability so I can’t use a preprogrammed tool table so this measure-on-tool-change mechanism works for me.

Not sure the measure-only approach as per OP would work for me. Not until I can implement something like the TTS system, anyway!

[John HaineParticipant @johnhaine32865]

This is my tool height thingy.  Steel base with a ring magnet bonded in.  3 layers of 0.5″ epoxy-glass laminated.  Hole bored nearly through to the base but not quite in which sits a stainless steel slug.  On the top is a steel plate with aperture bolted to the GRP stack.  A large square TC tool is sprung against the underside of the plate as a “platen”, with the other end of the spring sitting on the slug.  Slug has a 4mm hole bored into its periphery aligned with the matching hole in the side into which a lead to the probe input is connected. Hardest part was accurately measuring the height of the platen above the base, as you can see it’s 38.44 mm.  In use the probe input (a/k/a digitise input) (which has a pullup in the controller) is isolated from the machine frame until the tool (which is grounded through the machine) touches it.  I used a height setting macro from the Mach 3 support forum with a few mods.  You jog the tool until just above the plate, hit the auto tool zero button, tool moves down @5mm/min until it touches, draws back a tad, then probes down much slower until it touches again, then lifts up to 50 mm above the table.

[John HaineParticipant @johnhaine32865]

This my edge finder, works on the same principle where the probe tip is grounded through the work.  To get dead concentricity, made as one piece from a 10mm ground stainless rod from an old HP printer.  Held in collet, drilled 8mm from one end leaving 20mm or so at the bottom of the hole.  The drilled 5mm for about 10mm further and threaded M6.  Length of M6 studding screwed tight into the threaded hole, so it’s coaxial with the body and the end slightly below the end. Then the space between the screw and the body filled with full-fat slow set araldite, with the assembly and the araldite warmed to get it runny.  Held in a warm place (top of the workshop storage heater) for a few hours to cure, then left for a couple of days more to fully harden. Then a narrow groove turned in the body just down to the resin so there is a length of the body isolated at the tip.  A split brass block clamps to this and has a 4mm hole for the probe lead.  This time there are 4 Mach3 button macros to find the 4 edges of a part and another one to find the centre of a hole, activated by the buttons on the offsets screen.

 

[John HaineParticipant @johnhaine32865]

I also probe on the lathe to find the periphery and end of the stock, and populate tool table, but that’s a different kettle of fish entirely.

The only time I do manual height setting or edge finding on the CNC now is when executing an “inch” program – you can send the machine a G20 command to tell it that the Gcode is in inch moves, but this doesn’t apply to the macros.  Useful for PCB milling and recently for doing a replacement component for a clock made with inch measurements.

[Dave SParticipant @daves59043]

Took a quick video of it in action:

Dave

[DiogenesParticipant @diogenes]

Neat & quick. Can see how something like that would make life easier on my manual mill when swapping multiple tools.

 

[Author]

Posts