PDA

View Full Version : Tool Height Setting Probe - Mach3 - solution



HiltonSteve
10-06-2012, 01:46 PM
I have been making a few different jobs over the last couple or 3 weeks and nearly every one of them involves manually changing tools. This was getting to be a pain in the arse so decided to make something to make life easier.

It took me about an hour to make using a bit of engineering plastic, a bit of steel which I had lying around and a spring, after using it I realized I should have made one a long time ago. Changing tools now is a piece of p**s.! I put the spring in to give the probe a little bit of movement in case the machine overtravels slightly, this way it does not damage the tool when setting.

I have attached the drawing, photo of it and the script which I took from the Mach3 website and modified the code to suit my machine. The code is not 100% compatible with everyone's machine as each machine is different so be warned.. the reason why I had to edit it was when running the original code the machine wanted to come down and touch on the probe, stop and then rapid down into the table, nice... This was mainly down to the fact that I do not have any home switch's on my machine which is one of the jobs I will get round to one day, not really needed them but can definitely see the advantage in having them. Anyway, I changed the code to get round this and now it works fine.

The probe is wired into the controller using a single core wire, any size wire within reason will do, I used a length of 0.75mm. Once you wire it in setup mach so that the input you have wired it to is associated with the digitize function. The input configuration can be found in the can be found in the 'Config', 'Ports and Pins', 'Input signals' section in Mach3. You may have to play with the active low setting to get it to work, just depends how your inputs are wired. Mine is set to active low ON, the default is off.

The method for using the probe is as follows -


1 - Set your x and y offsets on the job.
2 - Set tool to tool 0 - this is where the Z0 offset for the job is stored
3 - Jog the tool (any tool) over the job.
4 - Jog the z axis down to where you want Z0 to be, this will vary depending on how you have programmed the job.
5 - Hit the 'Zero Z' button just in the same way that you would normally set the z offset.
6 - Put the tool height setting probe (THSP) on the bed of the machine (NOT on the top of the job), it could be fixed to the bed in a specific position if required.
7 - Jog the machine over the THSP and jog down so that the tool is about 20mm away from the THSP.
8 - Double check that mach3 is set to tool 0 and hit the 'Auto tool zero' button (once you have put the script in which I have attached!)
9 - The tool will feed down until it touch's the probe, it will then rapid up away from the probe. Mach now knows where the top of the job is in relation to the table and stores the offset.
10 - Run the first tool for the job.
11 - Tool change - Manually change the tool to the next one in the program and jog the machine so that it is over the THSP and around 20mm above it.
12 - Make sure that Mach3 is now NOT set to tool 0, at this stage it needs to be T1, T2, T3 etc ** Important note - make sure that all of your tool offsets are set to 0, the script does not use the tool offset values but if your program uses them and you have a value of anything other than 0 in then it will probably end up either scrapping the job or crashing the machine. Just set them all to 0...!
13 - Hit the 'Auto tool zero' button in Mach, the machine now jogs down and touch's the new tool on the THSP then rapids away.
14 - What the script does is now look at the difference between the first tool which you used and the current one, it then adjusts the z offset height on the machine.
15 - Change tools as many times as you like using the same method.

I did try to write the script and make it store the values in the tool offset table but this proved too complicated and is not required, when manually changing tools then all you are interested in is the difference in height between the first tool and the current one and this is what the script does.

Best thing I have made in a while...

6117
6118
6119
6120

JAZZCNC
10-06-2012, 04:49 PM
Hi Steve,

Long time no speak (Remember me, Hemsworthlad.!!)

If you think this is good addition Get the home switch's ASAP they really are one of the best and simplist things you can add to a machine.!

If you want to expand on this script and and basicly make it full autotool setting checkout Bigtex's screenset then mod the code to suit your screen or machine if like me you don't like the MachBlue screen.
I modded my own screen and probe scripts, in the early days of tex's scripts I adapted(along with others) tweaked them so they worked with metric or imperial units checking which was being used. I also altered the code to double tap the probe differantly for some reason but can't remember why.? All I know is it wouldn't work how I wanted it.!! . . Initial fast probe then a small retract then slow accurate one. I found it far more accurate and you didn't need to mess about positioning the tool 20-30mm above the pad as the first fast probe was quick enough to probe from highup and not seem like for waiting for ever.!!

In the past I wrote(or Hacked others) and used probe scripts all the time by MDI calling macros, top of material, material edge, corner, circle centre, circle outer, parallel edge etc and they are so usefull I wouldn't have been without them thou I never took the time to fully build a custom screen to make best use of them. Then Gerry(Ger21) came along with his 2010 screen which had pritty much the same probe routines so now I just use gerry's screen.! . . . It's Mega.

The probes have saved me hours and hours in setup time and got my arse out of so much trouble it's unreal. Between the home switchs and these probes they must have literialy saved me hundreds and hundreds of pounds in lost material and lost work when shit happens. ..!! (often)
With probes and home switchs I can be back in absolute position in less than a minute, no loss of position, Either start code from beggining or use "run from here" if half way thru a job say after a tool break or something.!!
Job setup time is reduced to less than a minute, imagine having to manualy align accurately the metrial edge parallel to an Axis or the spindle or find centre of hole or centre of circler boss.?
Normally this would involve setting up dial indicator and either indicating off the axis or putting in the spindle then indicating along the edge. .:thumbdown:
With the parallel edge probe script I just tell it the distance between 2 points along the edge to probe the distance to retract off the edge and away it goes and reports back the angle, difference distance positive or negative so a quick tap here and there and I have a perfectly parallel edge all done in seconds and perfectly accurate no guess work. .!! . . Same with centre of circle.!! Stick tool some where near centre click and watch it find centre in seconds :yahoo:

To be honest Playing with screens and scripts is good run and quite rewarding but honestly for 20 I'd just buy Gerry's screen because it does everything.!!

HiltonSteve
10-06-2012, 06:12 PM
I did see gerrys screen and nearly bought it but decided to have a go at writing my own scripts as it did seem that without a z axis homing switch gerrys screen would not work.

Do like the look of the screen compared to the std mach layout and thinking about it now it would have probably been quicker to get that and fit a home switch.

Ok, just talked myself into it, with a bit of help from you.... Just off to the workshop to fit a homing switch. Will order gerrys screen now.

HiltonSteve
10-06-2012, 06:22 PM
Just bought Gerrys screen, it is $20 not 20 which worked out to 13.36.

No brainer really....

Will let you know how I get on with it.

Ger21
10-06-2012, 07:51 PM
If it were 20, I'd have to pay Dean a commission. :beer:
Thanks for the purchase :thumsup:

JAZZCNC
10-06-2012, 08:20 PM
If it were 20, I'd have to pay Dean a commission. :beer:
Thanks for the purchase :thumsup:

Gerry I'll be your sole UK distributor then it will be 20. .:pirate: . . . . . Well UK Gecko distributors get away with it as do lots of others.!! . . It seems like some UK folks like getting ripped off.???

HiltonSteve
10-06-2012, 11:45 PM
Well got the Gerrys 2010 screenset, installed it as per the manual, and got to say that it looks much nicer than the original Mach screen. A lot easier to navigate around, took me about 5 mins to get my head round it.

Still not bothered with the homing switch's and I have got the auto tool length setting working just fine without them, I will be putting them on at some time soon though. Set up and tested my soft limits and they should give me enough protection at this stage.

Quick question - In the Auto Zero settings, can I set the tool using my height probe on the bed of the machine, put the height of the probe into the plate thickness box (41mm in my case) and then put the distance from the bed to the top of the job (Z0) in the material offset. This is more or less the same method that I have used on larger CNC machines in the past, only difference is the G54 Z offset is not used and the figure in the material offset box is used in its place. The simple auto zero button seems to achieve this but not played enough yet to see if the material offset workaround will work or not.

Theory behind this is quite simple, if i tell the machine how far the top of the work is from the bed by measuring it then the machine only needs to know where the tool is in relation to the bed. For a lot of my jobs I tend to be cutting rough sawn hardwoods which first need facing to give me a flat surface to work on and I usually set my z0 lower than the top surface as it is so uneven. This means setting zero on the top is no good to me.

JAZZ, let me know where you want the 6.64 sending and I will sort it tomorrow.....

JAZZCNC
11-06-2012, 12:09 AM
Quick question - In the Auto Zero settings, can I set the tool using my height probe on the bed of the machine, put the height of the probe into the plate thickness box (41mm in my case) and then put the distance from the bed to the top of the job (Z0) in the material offset. This is more or less the same method that I have used on larger CNC machines in the past, only difference is the G54 Z offset is not used and the figure in the material offset box is used in its place. The simple auto zero button seems to achieve this but not played enough yet to see if the material offset workaround will work or not.

You know these four letters. . . RTFM.!! . . . . But here's a snippit.! (Example 2 )

" Material Offset: Use the Material Offset option to zero the Z axis to a position offset from the plate
bottom. Check the box to enable this option. If unchecked, the offset value is ignored.
Example: Say that you have g-code that cuts profiles .74” deep into a .75” thick panel, and you'd like to use
the same code on thinner material, say .50”. There are two ways to use the offset.
1) Set the offset to the difference between the material originally coded for (.75”) and the material your
using (.5”). You'd set the offset to .25”, and zero with the plate on the material. Z zero will be set
.25” above the material.
2) Set the offset to the thickness of the original material, .75”, and zero to the bed of the machine. Z
zero will be set .75” above the bed. This will allow you to cut the profiles from any material
thickness not greater than the original.
Note: Negative values are allowed for the material offset. If a negative value is used, a message will be
displayed to notify the user, followed by a 3 second pause, before the probing operation begins."

Send the 6.64 along with my consultencey fee's to RSPCA for chimps.!!

HiltonSteve
11-06-2012, 11:18 AM
So basically what your saying is yes!

I did read that part of the manual but with not using this screen set before I was still unsure if it would work. Will give it a go later.

As for the 6.64, I will put it back in my pocket and go buy myself some banana's.

JAZZCNC
11-06-2012, 03:56 PM
Opp's just re -read my reply and it comes over like was being OFF doesn't it which wasn't the case honest. . Soz if ya took it that way.!!

Yep dont do it personally but it reads has thou it's do-able. Easy to check thou without risking damage by Zeroing off the top of something soft has thou it was the bed, Then entering probe thickness and offset settings.!

Buy green Banana's they last longer.:encouragement:

HiltonSteve
11-06-2012, 09:57 PM
Takes a lot more for me to take offense ..... anyway ... non taken!

Tried it, and it works perfectly.. Just what I was after :tears_of_joy:.

Gerrys screenset is very good, looks nicer than the original, the functions on it are very impressive, only thing that niggles me is that it runs in a window and not full screen on my 1280 x 1024 monitor but I will get used to it.

JAZZCNC
11-06-2012, 10:07 PM
Takes a lot more for me to take offense ..... anyway ... non taken!

Ok I'll try harder next time. .:beguiled:

Ger21
12-06-2012, 02:41 AM
Still not bothered with the homing switch's and I have got the auto tool length setting working just fine without them, I will be putting them on at some time soon though. Set up and tested my soft limits and they should give me enough protection at this stage.


If you don't have Home switches, just Ref the Z at the top of travel. This will allow the macros to keep from crashing the Z axis into the top of travel if you enter some settings that won't work. In order to use the toolchange position, park position, and tool change auto zero, you need a repeatable home position. Switches make everything easier.





Quick question - In the Auto Zero settings, can I set the tool using my height probe on the bed of the machine, put the height of the probe into the plate thickness box (41mm in my case) and then put the distance from the bed to the top of the job (Z0) in the material offset. This is more or less the same method that I have used on larger CNC machines in the past, only difference is the G54 Z offset is not used and the figure in the material offset box is used in its place. The simple auto zero button seems to achieve this but not played enough yet to see if the material offset workaround will work or not.

Theory behind this is quite simple, if i tell the machine how far the top of the work is from the bed by measuring it then the machine only needs to know where the tool is in relation to the bed. For a lot of my jobs I tend to be cutting rough sawn hardwoods which first need facing to give me a flat surface to work on and I usually set my z0 lower than the top surface as it is so uneven. This means setting zero on the top is no good to me.


The short answer is yes. The G54 ofset is still used, bbut the zero position is offset by the Material Offset amount.

I use the material offset so that I don't need to worry about the actual thickness when I program my parts. I just program to cut .75" deep, and it doesn't matter if the part is .78 or .68, it always cuts right to the bottom. I zero to the spoilboard and use a material offset of .75".

Of course, if doing V-Carving you need to zero to the top, but if you're just cutting out parts, the material offset can make things much easier.

riche543
20-06-2012, 04:13 AM
Subscribed ( notification )


Sent from my iPhone using Tapatalk

Leadhead
12-11-2013, 12:32 PM
Just about to make up some plates for my tool height setting. I am using a mill and remain nervous about the programme (2010) dropping my tooling onto a solid plate. Is it best practise to laminate either the fixed and/or movable plates to give some "sprung" resilience at touchoff?

JAZZCNC
12-11-2013, 04:25 PM
Just about to make up some plates for my tool height setting. I am using a mill and remain nervous about the programme (2010) dropping my tooling onto a solid plate. Is it best practise to laminate either the fixed and/or movable plates to give some "sprung" resilience at touchoff?

Don't worry about it just keep the touch speed sensible and you won't have a problem. Think I have mine set to 300mm/min initial touch then 50mm/min for final touch.

Always best when first setup to place something soft under plate for testing. Ie sponge then after that always touch probe to earth and check light comes on before each use.!. . . . After that you won't have any trouble I use mine everyday with tool direct to aluminium with no plate used at all (Ie zero thickness for plate) just a wire touching material and doesn't even mark the material.

Bazzer
12-11-2013, 05:11 PM
Always best when first setup to place something soft under plate for testing. Ie sponge

Thanks Jazz, another new product for me to sell "Touch Plate Testing Sponge" :hysterical::hysterical::hysterical::hysterical::h ysterical::tongue:

JAZZCNC
12-11-2013, 06:06 PM
Thanks Jazz, another new product for me to sell "Touch Plate Testing Sponge" :hysterical::hysterical::hysterical::hysterical::h ysterical::tongue:

Actually not a bad idea that Stick some PCB to that hard foam you have Si and would work treat.!!

Bazzer
12-11-2013, 06:23 PM
It's ok for testing, but I tried it with very firm foam and it must have flexed slightly on touch off giving a bad result.
Still u live and learn...well hopefully live to learn :hysterical::hysterical::hysterical::hysterical: