[Swede]

The latest Flashcut 2.XX series software has a number of tool-change friendly features, one of which is tool length sensing, something I've been desperate for. Within Setup, all you have to do is enter the tool-sensor location, a few other bits of Z data, and whatever formula you'd like to use to generate a G43 for the given tool.

After staring at the docs for a while, I decided to whip together a test rig. I bolted a microswitch onto a piece of aluminum, and did a few test tool swaps. Since all of my input lines were occupied, I "borrowed" one from the Servo Z axis position error line.

The first test was to determine the machine Z height of the spindle nose. Next, the spindle nose was used to set Program 0 on a chunk of aluminum. Using the spindle nose to touch-off program 0 allows any subsequent G43 offset to "raise" the Z, bringing the tip of the tool to the original program 0.

The formula to obtain G43 for a given tool is simply (X + #Machine.Z), where X is the known height in absolute Z of the switch relative to the spindle nose, and #Machine.Z is the absolute Z when the tool tip touches the switch.

For example, if the sensor/spindle nose contact (and this remains unchanged for all tools) is at -5, and the tool tip senses at -4.5, the formula is (5 + -4.5), yielding a G43 for that particular tool of 0.5.

Thus, tool swap is as simple as this: The G-code asks for "Tool #3". Select Tool #3 from the drop-down tool list, click the Tool Length... button, and after sensing, the G43 is automatically applied to Tool #3. It works great!!

This is a boon for my KaVo 4041 spindle which doesn't use fixed tooling, and allows me to experiment freely with ER16 spindles, etc, and not have to sweat numerous tool swaps.

Thanks FC for this nice addition to the software. All I need to do now is make a decent fixture.

[Swede]

Follow up: Sensing works great, BUT (and that's a capital BUT) executing one IN THE MIDDLE OF A G-CODE, DOING A NORMAL TOOL SWAP, WILL RESET THE G-CODE FILE! So TL sensing, as it stands now, still requires fixed tooling. TL sensing simply fills in the G43 offset in the tooling.... dialogue. FC says that TL sensing DURING a tool change will happen in the next version, so when that happens, hopefully all of our non-fixed tooling changes will be easy and effective.

[cncadmin]

How do you like Flashcut? I downloaded the demo looks very professional.

[ger21]

Swede, Mach2 can do the tool swap sensing thing. I think it just requires a macro.

[Bubba]

Swede,
I have been doing it in Turbocam since V3.25:})

Right now, I have my tool sensing switch which is an optical and it works fantastic. I just stick the tool in at a M06 and the quill runs over to the switch, measures the offset and then waits for me to turn on the spindle and coolant (don't have that automated YET!) and does its thing.

To me this is much better than worrying about setting up a table and being sure I insert the tool to just the right postion.

[ynneb]

Swede, Mach2 can do the tool swap sensing thing. I think it just requires a macro.

Hey Gerry, I have been thinking to try and implement this on my machine. Do you know where to get this macro from? Could you please upload it if you have it? Tanx

Right now, I have my tool sensing switch which is an optical and it works fantastic.

Did you make this yourself ? Do you have the plans or a description so that others could make it too? How well does it work with a V bit ? Does it see the tip well or only kicks in slightly up the V ?

Swede, thanks for sharing your experiment with us. You have started me thinking about that again.

[Bubba]

Yes, made it made myself. Most of my projects are "DIY" and fit to my needs

My switch senses the TIP and when doing a "home", sometimes I manually twist the quill to make sure one of the cutting edges hits the sensor.

Here is my web site of one of my versions of the limit switch. I have a better one now, but have not gotten around to making pictures and updating the web site.

Nope, no plans as you need to make the system fit YOUR needs. Maybe this weekend, I can update my web page of this version. Am also planning on making a simular setup for my X axis so I can have an "accurate" repeatable home switch for my setups. Then maybe another one for the Y so it will also be "repeatable"

In my setups, I use the homes as G53 and then G54 for my part and G59 is my tool change place. Thus I use G28 to home the X and Y (G53), then set my part X0, Y0 in G54. In my G-code file I home the quill (no tool) DOWN as 0 and then when the tool is in place, do a G53 and go to the location of the aux. Z switch (which has previously been set to the part Z=0 and sets the tool to Z=0. Then it pauses and waits for me to turn on the spindle and coolant. Then it will process the code for that tool. Repeat as necessary. NOTE: all of this is done in my modification of TurboCnc to handle homing on a single axis in G-code.

Version 3 of my aux. Z homing switch can be seen at:

http://bellsouthpwp.net/A/r/Arts_hom...limitswitches/

Let me know if I can help

[JRoque]

Hi. Mach2 certainly works for this. I do it a bit differently. I have a 'sensor' which is a piece of copper attached to a wire on a parallel port input. I place the sensor on top of the workpiece and run a macro. The macro lowers Z until it makes contact with the sensor, subtracts the sensor's thickness and backs out to a set height, 1" in my case.

The advantage I see with this method is that different material heights are accounted for and cutting always starts at Z=0. Here's a link to my machine log and an early video on how it works: http://www.cnczone.com/forums/showthread.php?t=5302 (3rd post down)

Thanks,
JR

[Bubba]

Jr,
Yes, I can see an advantage to your system also, but in my case; there is only one setup for the gage and I handle the "offset" say by doing a facing first in my Cam program. EG. If I face off .020, I simply start each new operation as necessary at -.020 and go on. (To be honest, if it is a drilling operation, I just let it cut air for that extra .020

[Swede]

Paul, I like FC very much. I wanted a system which was pretty much turn-key, as I wanted to focus my efforts on the hardware rather than the software and amplifier setup. They've been updating the software continuously, and the current version has some very nice features. It's Windows based, but no timing problems as the command stream is fed serially (115kBaud) into their signal generator box. Overall, I like it and it has grown along with my own ability to use it. Support seems excellent.

The FC servo "box" is really a Logosol product:
http://www.logosolinc.com/

I spent a day flogging this tool length sensing thing, and was unable to write a macro to accomplish it. So for now it's fixed tooling and G43, using the current tool length sensing to update the tooling list. The latest version also has automatic tool change capability for those with nice machines.

unfixed tooling can still be used, of course, just need to touch it off. Bubba, I couldn't access your site... how repeatable is the optical sensor? For now I'm happy with my mechanical sensor which repeats to 0.0002" or so. But I'm a sucker for the type of setup you describe!

[Bubba]

Swede,
I can't find the spreadsheet that I did on the last iteration of my optical, but what I did, was to repeatably hit the switch and record the difference between T0 (G53) and the tool T1
As I remember on a run of 10 iterations, I got a repeatability of .0004" This was done in a series of measurements over a period of say 45 seconds.
But what I found that if I did this over a period of say 5 minutes, the repeatibility improved by a factor of about 10!

This makes me think there may be some sort of thermal (?) problem or maybe something else. My system is a servo system using geckos on the micro feed of my Mill/Drill and the encoder is on the worm shaft of the feed.

PS: I do not understand why you could not access the site I posted as I copied the url when I pulled that page up.

If you cannot get in in a reasonable time, let me know and I will mail you the pictures etc.

[Su Boka]

Swede,

Any idea on how I can tell if a couple of Kavo 4041s are in possible working condition without applying power yet? For example no bearing noise, measuring winding resistances. I have 2 I stripped out of some production equipment but was not able to find a controller. I would like to start using one of them but dont want to invest in a controller untill I have some idea if one has a chance of working. I also have a Freqrol U100, but have not had time to research if it is compatable.

Thanks
Rick

[lerman]

Bubba, Swede,

Which commercial mechanical switches did you use?

Bubba,

What optical sensor are you using?

Thanks,

Ken

[Bubba]

lerman,
For the mechanical switches, I used Automation Direct http://www.automationdirect.com AAP2T51A11 mini din switches. As I remember, I paid about UD$12.5 each for them and at 1,000,000 operations they are rated at .0003" repeatability.
For the optical, I used a GP1A05 that I salvaged out of a defunct copy machine.

[ger21]

Try this number AAP2T51Z11

[Bubba]

OOPs, sorry bout that! :{(

[centaur91]

How do you determine the tools offsets for each turning tools? The manual does not give single example how to do it.

I have a lathe with 5 tools in a gang. I would like to use them all but not sure how to enter the tool offsets

Has anyone done it successfully?

[Leoo5van]

I would like to use them all but not sure how to enter the tool offsets

[davidtye23]

So far, so good.

[datac]

I'm retro-ing a Denford right now and it has the tool changer. I never spent any time with a CNC lathe, so its going to be a bit of a learning curve. I can't imagine it being any different than setting up tooling for a mill,... just that different axis are used.

I've been working on building an automated, swing out tool sensor switch that can be called to automatically measure the tools. Not sure when It will actually operate, but its at least started and in the plans !

I'm sure I will spend a great deal of time cutting AIR, then move to wood or plastic until it all makes sense.

Good luck !