Someone on here mentioned that the Shop bot comes with a Z axis zeroing tool made up of a plate that you set on your material. You run some kind of "Zeroing routine" and the tool comes down an touches the plate and calculates the material top of stock location and sets the tool zero to be at the top of stock.

Well I made my own, and it's so simple it's silly.

I made a small .125" thick plate from aluminum. I took the +5 volt wire off my Z axis home switch, extended it and tied it to the plate. I set my z home switch in turbocnc.ini file to normally open and the home offset to .124". My router has an aluminum body so it is grounded.

To set the tool height, I chuck in the tool, set the little plate on my material, under the tool, then I home the axis. The z axis slowly moves down towards the plate. When it touches the plate, it stops, thinking it hit a NO switch, and sets the z height to .124". The 1 thou difference seems to be the time it takes for the tool to stop. I raise the tool, remove the plate, and if I send the z to 0" it stops perfectly on the top of the materail every time. I han just barely slide the material out from under the tool, it leaves just the slightest mark. I love it.

I will make a plastic pocket, attached to the z axis to hold the little plate so it can ride along and be insulated from things while not in use.

Here is a picture

Eric

Way Cool! Have to use this idea.
Bill

Definitely cool!

I one of those things where you say "Doh, why didn't I think of that!"

Good work Eric.

I'm probably stating the obvious but for those with insulated routers, you could rig up an aligator clip to attach to the bit.

Or would this be electrically harmful to something?

That would work fine.

Eric

Great Idea !!!
I will have to do this

Great idea Eric.
If the tool overtraveled into the plate, you could design a spring loaded the plate to allow for that.
Bill.

Eric would you mind me showing my tool set switch here? I will have to get it photographed. I tried one photo and the light was not good enough? My switch is a different animal completely so it will at least give a variety, .....just say the word.
Mike

I've also done something like this with my 'nearly completed' machine. I've done a permenant
system, where I've constructed a spring loaded touch sensor just to the side of the table. This
sensor is exactly the same height as the spoilboard, so after I've flycut I can adjust the sensor
accordingly. The feed is to pin 11 of Mach 2 and ground is through the frame (the spindle is double insulated). I'm about to run a macro the moves the tool to the sensor. The only thing I haven't worked out yet, is how the automatically set the height when it touches. Apparently I should use the 'digitise' method. Has anybody done this in Mach 2?

I'll post some pictures of the machine in a few days or so. I'm rather proud of it.

Turmite, go ahead.

Krsykes, I would like to see some pictures

Eric

Nice idea Eric


as for my impatience and related promised pics...
It's been an hour now and no pics posted yet!;)

Very nice simple implementation. What Feedrate do you use when probing the tool? I would imagine that with this system, the slower you run it down the more accurate it will be.

A little spring loaded system like they use on the big machines would be nice to keep from breaking bits in case they touched down a bit hard, but you're not making this for Joe Schmo, you made it to make your life easier. You know, the more I look at this system, I am in love with it's simplicity. :D

Great job on a very useful tool!

It aproaches the plate at around 10" per minute. It does not hit hard, and stops instantly. It will not break a bit unless something is very wrong(wire broken off the little plate, software settings messed up).

Eric

krsykes my system is Mach2. I have the macro already done. I will try to email it to you or post it in the files section over on the y Mach2 forum.

Eric I will try to get the pics today. It is basically a micro switch mounted to the table that I machined some add on parts for. It sounds like exactly what krsykes has done, except I used a shotgun barrel!:D

Mike

That is fantastic. I had wondered if it could be done like that, that is how the CNC machines I have used in the past worked.
I am going to check the Mach2 forum to see if you have put up the macro yet. With a spring loaded switch, do you have it set to plunge quickly, then retract a bit when it hits the switch then plunge slowly and stop again when it hits the switch? This is how the tool probe's I am familiar with work. Very accurate because the second plunge is slower.
co

yukonho I had to use my brother's digital camera and then he had to email the jpeg to me for the pics. I have been waiting for over three hrs for the email and he lives 1/4 mile away. I will go to the shop and get the macro and will put it up by 2:00pm central time.

Mike

Great, thanks.
If you cant post it, could you e-mail it to me? That would be great. It is so cool to add a feature like this to a home made machine. Just approaches "real machine" status with every addition.The spindle on off and Estop are my latest additions and I love em.
cant wait to do this one
co

yukonho believe it or not I couldn't see on my computer at the shop. :o No...seriously I forgot my glasses and couldn't see it.:D

I did find it in my email folder I have dedicated to Mach2.

You will have to edit it to fit your needs and the feed rate needs to be about what has been posted so far of 10" min.

Here tis!

code "g31 z-10 f10"
While IsMoving()
Wend
code "G92 Z0"
code "G0Z3"
While IsMoving()
Wend
code "g92z0"

I have a deep z so I put in the z-10. This script restes the z axis to zero in the last line. If you will notice the fifth line down is a z3" move up. You can edit that for whatever you would like. I don't have to have a know distance from my table height but from the centerline of my a axis. I hope this helps. I will post the pics as soon as they get here from cyber mail.

Mike

edited to add ( make sure you write it exactly as shown as in Caps spaces etc. I made the mistake of having 1 space in between ( and) like before the a in and, and it wouldn't work.)

Sweet concept Eric. I love it when simplicity reigns. Now we need to think of a similar device which will work on conductive stock like steel or aluminum. I suppose one could insulate the touch pad with a piece of teflon, or better yet, how about a phenolic block, with an inset of brass, machined to an exact height? The phenolic would be oil resistant and dimensionally stable to boot. You could have different shapes for other than flat stock, such as a v-block for round stock, a rod probe for recesses, etc.

Just thinking out loud, here. Thanks for sharing this with us!

how about a peice of PCB?
Bill

If you use the fixed probe idea you dont need to worry about top of stock on the machine, you take it into account when you are programming.
Thanks for the macro. I have never heard of those commands, so I have some learning to do.
Any suggestions on resources for this info?
Really cool guys.
After this, my next thing on the list is a pendant of some sort. Even just an x, y, z jog pendant and maybe a cycle start and estop added in. But why not a zero axis button as well......
Anyone done any work on a pendant?
co

Anyone done any work on a pendant?

I believe there is a lot of recent info on the Mach2 group.

my two little additions to this idea are....

what kind of spark gap is there? granted it will probably be pretty miniscule but still might be worth paying attention to with higher tolerance stuff if you wanted to make this for a big machine

and also instead of just using this for the x, could some sort of probe be built to do this in all three dimensions, either to determine the starting size location and orientation of a piece of stock and then adjust the toolpaths to fit, or for doing secondaries on parts that have already been begun and have the part orientation be cued up by the system

There is no spark gap. The axis moves until it touches the plate.

Eric

does it move until the plate and tool touch or until the connection and circuit between the tool and plate are closed? not trying to second guess its a great idea just curious as to how to apply this and possibly make it into something that could for example auto zero on the edge of a workpiece

ger21, didn't find anything on pendants in mach2 forum.
I think the best thing about this idea is its simplicity. Going to all kinds of probes and moving parts takes away its best feature.
co

Check out this site, they use a slightly modified version to also zero out the X and Y axis. There are quite a few other interesting things to look at on this website, a manual indexer, horizontal router, etc.

http://www.lb-innovation.dk/CNC%20TOUCH%20SENSOR%20en.htm

what alame product! $60 us aprox. for a lightbulb, a magnet, a wire, an alligator clip, a project box, and a piece of copper tape. and what sup with that storage box? wierd.. is that renshape?

BTW, this idea seems pretty simple, and i recall seeing a special option for it in some CNC control program a while back. anyways - just setup an extra axis and use its limit switch or home switch for this. its easy to use a bare copper strip and an electrode on your machine to do this. it just assumes your machine has a path from any metal point to the spindle tool..

dunno about that...

Originally posted by avsfan733
does it move until the plate and tool touch or until the connection and circuit between the tool and plate are closed?

These two are one in the same, so the answer to these two questions is yes...:)

Eric

Originally posted by buscht
Check out this site, they use a slightly modified version to also zero out the X and Y axis. There are quite a few other interesting things to look at on this website, a manual indexer, horizontal router, etc.

http://www.lb-innovation.dk/CNC%20TOUCH%20SENSOR%20en.htm

It seems to me this just lights up when contact is made. It doesn't stop the axis, or zero the axis. You still need to manually stop "jogging" when you see it light up, then manually set the axis to zero...

Eric

Great idea Balsaman! I will use something like this on my router, although I will probably tweak the design a bit. What about using a small piece of 1/4 inch steel plate and cutting a recessed pocket into the table top? You could run the wires under the table in a permanent position. If you get everything right, it should find the Z 0 perfectly.

Just a thought.

A good thought.

BUT, I always set my 0" at top of stock, not top of table. With this one you set the 0 on top of stock no matter how thick the stock is by placing the pad on the material after it's clamped down. If I do want to set my zero at the table, I just put the pad on the table.

I had thought of doing it as you have suggested, but this way works better for me. Also this way I can zero the z anywhere, so I don't need to jog to a corner first, then jog back to the material.

Eric

For people that want to use the copper tape setup you can get it from anybody thay sells stained glass supplies, and it's fairly cheap.

Turmite...

Sorry for the delay in posting the picture. I just need help with the coding now. I have mounted a sensor at spoilboard level that is connected to pin 11 and 'digitise'. This physically works fine. Art suggested looking at the Set Tool option in the latest version. I did this, and I now need to adapt it to give the 'daylight' for the tool (from the top of spoilboard to tooltip). Basically, I want to do the same as a 'manual' Touch Tool but incorporated into the automatic Set Tool facility. I've adapted the code...


if IsSuchSignal (22) Then

code "g0 x10 y1"
code "g0 z-30"
code "g31 z-62 f100"
While IsMoving()
Wend
....
....
etc. etc.

so that it rapids to X10 Y1 and down 30. Then slows for the G31
until it touches. It's here I need the help !

Touch Tool works great, I do a manual Touch on the senor then Ref the Z. I then insert a G43 into the NC code and it comps for the length. How can I adapt the code to do the same as 'Touch Tool'.

Many thanks. Keith

krsykes my z reference 0 is at the top of my z axis. I use the posted script that Art of the Mach2 fame and Jim Cullins of the Campbell breakout board fame.....well they're famous to me, help me to refine.

code "g31 z-10 f50" ++++this lowers the z head+++++


While IsMoving() +++if memory is correct don't do anything else while the first move is taking place++++


Wend ++++this ends the first move++++


code "G92 Z0" ++++this sets the switch position at 0+++



code "G0Z3" ++++this moves the z up 3"+++++

While IsMoving() +++again don't do anything while doing the above command+++++

Wend +++again ends above command+++


code "g92z0" +++sets the z axis to 0 once again and this happens to be 1.451" above the centerline of my a axis. I could move it up by as little as I want or till I hit the upper limit again.

I also wrote a screen for Mach2 that has this as a button that is very easy to use. Ok so Art help em again but once you do it, it is really easy.

I needed this feature due to the many tools required in a given program and I don't have an auto tool changer. This has speeded up the tool change process quite a bit. I will eventually include programed tool changes into a master program that is stiched together from many seperate programs.

I hope this helps. If not shoot me an email offline and we'll get it worked out for you.
Mike

Ihatespam2guzakaka@earthlink.net Just remove the obvious. This one does not have the blocker so you should be able to get through ok. Oh yeah, start the address with g;)

krsykes you will have to forgive me. I have had kinda a badk couple of weeks and my head is maybe not where it normally is
and by that I mean I have been kinda preoccupied:D .

I re-read your post and think I need to grab all the info I can off of my shop pc for you. It really does work well. I will try to get it for you tonight.

Mike

Originally posted by gopackgo
For people that want to use the copper tape setup you can get it from anybody thay sells stained glass supplies, and it's fairly cheap.

You can also use aluminum duct tape, not the 200 mph kind but the aluminum foil type available at all heating and air supply houses. It is only .002" thin after backing is removed. Just apply a small piece to your object surface and leave a corner turned up to clip an alligator clip to.

Tom

Balsaman,
Thanks for the inspiration as always. Here is my version of your idea. I can do X,Y, and Z with it to center the bit on the lower left corner of the stock. My Z axis plate is machined to 0.375 though and I can't place it anywhere on the stock like yours.

Marv

Cool....:)

Eric

I need some clarification on this. I want one. I am have a xylotex 3 axis board and turbo CnC. I plan to set the switches according to the diagram i got from the xylotex website. do i connect the switches for the x and y axis like the diagram and use the plate and ground wire on the z axis? Can i hook it up like that? telling turbo Cnc that the x and y axis has normally closed switches and the z axis has a normally open switch.

Has anyone set this up with a Soundlogic Mach 2 Breakout board?

I am interested in how it is attached to the input on the board and what settings they are using in Mach 2?

I would like to add a Z -axis touch probe to my router but I am abit confused how to do it properly. Ok... I am alot confused. LOL :confused:

The way my system is setup now I am using all 'NC' micro-switches for the homing of my axises and wired up in parallel according to the diagram found on the Xylotex website. Each switch is connected to it's own input pin on the parallel port. I want to keep my Z- Axis home switch at the top of the axis the way it is since I like to use the "Home All" feature in Mach2, so I can't connect to that circuit for the touch probe. At least I don't see how it would work if I did. I also like to zero my tools from the top of the stock so I was planning to just use a piece of flat aluminum stock .100" thick with a wire lead attached to it. Now I do have one input pin left on my parallel port which I was originally going to use for a A-Axis home switch but I doubt I will need a home switch on my rotary axis, so I could use this last input pin for a touch probe.
The question is how do I go about connecting it properly and setting up Mach2 to know what to do when it gets a signal? I'm guessing it would need to be set as if I was using a 'NO' switch but are there any other setting I need to set in Mach2 for me to be able to use some of the macro scripts I have seen posted, such as the digitize setting? I have already created a button in Mach2 for activating a "Z -Touch Probe" sequence and I used the macro that "termite" posted. The Z -axis goes down slowly as it should but without a proper circuit for the probe it will not do what it is suppose to.

So basically what I want to be able to do is click a button on the Mach2 screen that triggers the Z to move down slowly till the cutter comes into contact with the aluminum touch plate. Once contact has been made Mach2 resets the Z - axis DRO to +.100 or +.101 then moves back up a set distance, say 3 inches. But most important I would still like to tell my Z-axis to go home and it moves up to the home switch.

Is it possible or am I asking too much? If it is possible how do I go about doing it? I have no programing experience so I don't know how to create my own macros.

Thanks in advance for any advise. :wave:

Carl

Well I have finally gotten it to work properly. I ended up using the spare LPT input pin that I was saving for the A-axis home switch. I just ran a long enough wire from the +5V end of that circuit to the aluminum touch plate. I then went into- Mach2 - "Config" > "Ports and Pins" > "Input Signals" and turned on 'digitize. Clicked on Apply.
Then went into the "Input Pins" tab, set 'Digitize/Skip' to Active Low and entered the corresponding pin number. Clicked on Apply.

To double check the plate was triggering properly I went into the "Diagnostics" screen. When I touch the aluminum plate to the end of the cutter the Digitize led came on.

Now when I click the "Z - Touch Probe" button I created in Mach2, the Z axis moves down slowly till the tool touches the plate, resets the Z- DRO to (+.100) then rapids back up 2". I am using the same macro that "termite" posted earlier except with a few value changes. It really works nicely. Thanks termite. ;)


Carl

how bout machining a corner plate to home all.. this will also allow you to set the matierial location as well.

In post #38 marvinstov did that for his machine.

The only issue I see with that is going to depend on the cutter you are using.
Cutters like router bits tend to have their flutes straight up and down so you would have to make sure that your cutter is rotated at the correct position so the furtherst most point of the cutting edge is what touches your corner plate first. Four flute endmills have more more cutting edges so you have a better chance that one of the edges is going to line up properly. The easiest solution to this is to use a piece of 1/4" diam. ground drill rod in the router instead of a cutter. Probe to the corner locations of your stock, set your offsets then install your cutter then probe down to set the Z to the bottom of your cutter. Abit more time consuming but more accurate. I know most of the time I will be cutting something completely out of a piece of material so having the exact edges of my material is not important. I can set the tool to the corner by eye and that will be good enough.

krsykes my z reference 0 is at the top of my z axis. I use the posted script that Art of the Mach2 fame and Jim Cullins of the Campbell breakout board fame.....well they're famous to me, help me to refine.

code "g31 z-10 f50" ++++this lowers the z head+++++


While IsMoving() +++if memory is correct don't do anything else while the first move is taking place++++


Wend ++++this ends the first move++++


code "G92 Z0" ++++this sets the switch position at 0+++



code "G0Z3" ++++this moves the z up 3"+++++

While IsMoving() +++again don't do anything while doing the above command+++++

Wend +++again ends above command+++


code "g92z0" +++sets the z axis to 0 once again and this happens to be 1.451" above the centerline of my a axis. I could move it up by as little as I want or till I hit the upper limit again.


Just wondering why not set it to "G92 Z-3." instead of "G92 Z0" the first
time it hits.
This would be shorter and you would not have to reset this again later.
To move 3." up you could then tell it to "G0 Z0" and be done with it.

In post #38 marvinstov did that for his machine.

The only issue I see with that is going to depend on the cutter you are using.
Cutters like router bits tend to have their flutes straight up and down so you would have to make sure that your cutter is rotated at the correct position so the furtherst most point of the cutting edge is what touches your corner plate first. Four flute endmills have more more cutting edges so you have a better chance that one of the edges is going to line up properly. The easiest solution to this is to use a piece of 1/4" diam. ground drill rod in the router instead of a cutter. Probe to the corner locations of your stock, set your offsets then install your cutter then probe down to set the Z to the bottom of your cutter. Abit more time consuming but more accurate. I know most of the time I will be cutting something completely out of a piece of material so having the exact edges of my material is not important. I can set the tool to the corner by eye and that will be good enough.


how bout a set up rings made from say brass??

I cannot view you attached file...why is that? I'm new to CNC Zone and I can't figure out why I cannot view attached thumbnails.

Vince

Any idea guys if that will work with PMDX-122 Braking board?
Manual is here: http://www.pmdx.com/PMDX-122/PMDX-122_Manual_15.pdf

My router is under construction, but I am using 4 stepper motors 8,5Nm 6A, (2 for X)and PMDX-122 breakingboard.

I am going to use mach2/3 or turbocnc.


Thank you for any help

This is neat. If I ever get a working machine together, this is a must.


Vince - you probably havent setup your email address? You need to follow the registration email they send you.

In Mach3, can the z axis be homed independently to the x & y.

it works great >>>>>>>>>>so easy thank you :)

What a great solution to a pain in the a%% problem.

I built one of these and installed it on my CNC router.

I have a WinCNC controller and software.

I created a SETZ G code file that includes the following two lines.

G31 Z-300 f100
G92 Z9.835

The file aborts do to hitting the limit plate and never runs line two.

Help?

I have emailed both WinCNC and PracticalCNC and have not received a reply yet.

Thanks in advance.

Sam

It needs to be connected to the z - home input, not the z - limit input.

Eric

It needs to be connected to the z - home input, not the z - limit input.

Eric


Eric,

I meant to say home input. I am still having trouble with the software seting the Z to odd values after the file runs.

Still can't seem to make it work correctly.

Sam