Work Horse Rebuild - Lac-Brome, Quebec, CA

[Robert M]

Salut Norm....

"wondering if you got 3 phase going straight in your shop"....

Your truly a funny guy .....cheers mate

[normand blais]

not wanting to be funny Bob some old shop have 3 phases .well I guess you would have know .
But want to hear a good one , your nice dust foot skirt wont be any good for you any more.ah ah
I could recycle it if you want,I use same router

[Robert M]

Not always obvious how to ask question in regards to what your seeking / hopping for ??...right, or…....right !!
So, hoping this is comprehensible !

Say when your programming a toolpath from a CAM, whatever the one, and say you’re selecting a ½’’ endmill for the cutting of the selected vectors out in the file on your CAM software!
Say, you have more then a few pieces to cut with this ½’’ EM, but, say…while not completed done ( qty wise) you must change End mill since the initial one has dulled !
So fare, nothing irregular to most!!
But here come ( or goes) my question / catch !!
How to go about when you changing tools ( end mill in this case) to new re-sharpened one that is a smaller diam, say, .480 vs .500 new….

Is there a way, in Mach3 ( the controller I’m using) to change tool with some “miracle” tool diam compensation ( or call it different diam) from the NC file ( witch has / had been initially programmed with a 0.500 E.M ) ??

Bottom line, in a nut shell ( or 2 version) to my question is:
Is there a mean ( or way, not to say miracle way !!) when one has a NC file with a tool diam of xxx, and must change tool size to a diff tool diam, to change that directly in the controller ( say Mach3 or CNCC) IE: from end mill .0500 to a replaced EM of 0.480 ( .020” less diam)….with out reprogramming the tool back in the CAM ??

Wishing I’m ….clear @_# !!

Thanks, Robert

[ger21]

G41/G42.
This is how we do it in our shop, where most of our tools have been sharpened, and are all different sizes.

[Robert M]

Great Gerry, thanks for your input....
Not playing enough ( practically never) with G-codes, that option your steering me to has never cough my attention !
SUPER...I've learned another new thing !!

LOVE what this machine and all it's surrounding effects, .....fun isn't it ,,,@-#

just a thought.....although, strange to me as none of these "popular" controller offers a "kwik" CRC vs going in the nc file and taper/change this G41 & G42 !!

How it goes......they "must" be a better way
Till then, I'll pay with this G41 & G42

Thanks Ger, R.

[ger21]

When you use G41/G42, you just need to enter the tool diameter in the tool table, and Mach3 will handle the compensation.

You'll need CAM software that supports G41/G42, and can provide the required lead-in and lead-out moves.

[Robert M]

Thks again Gerry,

Great, so basically, right in Mach3, it can be that simple through this "tool table" config !
Problem I'm having this past hr++....is I can't find in this "darn" mach user guide (latest V1.84) how to learn to use this tool table ??

A simple picture example would been so simple from this so called "user manual".
Tool table_resize.jpg
Now I remember why this past 10yr I can stand Mach user manual......to me, mostly not user friendly ?....again, must be me @-# !!

As for CAM, I'm mostly using MasterCam or Aspire , so not a problem from what I can understand at this point !!

So in a simple approach, when you say "you just need to enter the tool diameter in the tool table"....may I ask you to show me a simple tool compensation say from 0.500 to new at 0.480" ?....or what page / pages in mach user to learn on this ??

Thks much....

[ger21]

I'll show you this evening when I get home from work.

[pblackburn]

I was going to refer you to a post on cnczone that Gerry answered. Glad to see he is still here for help.

[ger21]

OK, enter the tool diameter for tool #1 in the tool table, then load this code:

G0 Z0.1000
G0 X4 Y-.5
G42 D1 (Turn on compensation)
G1 X6 Y0 Z-0.2500 F50
G1 X12 F100
G1 Y10
G1 X0
G1 Y0
G1 X7
G1 X8 Y-.5
G40 (Turn off compensation)
G0 Z0.1000
M5
M30

Note that the D1 in the G42 line refers to the diameter of tool #1. D2 = tool 2, and so on.
The white line is the path that the tool actually follows. Play around with the diamter in the tool table and you'll see how the white line moves.
Try diameters of 0.25 and 0.75. (Regen the toolpath after making changes to the tool table)

[Robert M]

thanks very much on all your input, much appreciated
Test this out & get back to you
cheers @_#

[jask]

wow! Ger21!! way to step up.

[ger21]

I was in Kamloops last summer.

[jask]

... you should have come by for a beer!! and that applies to all the rest of you if you are out this way!

[Robert M]

One of these days.....I'll treat my self and go to BC...
Then, u bet, I'll knock on ur dore....for that beer....