[jimgeo7]

Is it possible to create G-code using a generic size cutter, say a .375 then after loading the code into Mach3 use the DRO pictured here to compensate for a cutter size of say .342. If it is possible how is it done? I know how to input the information, highlight the "Tool" DRO, enter the tool number, press enter, highlight the "Dia." DRO enter the new diameter, press enter and so on. Doing this just doesn't seem to make any changes in the path. Am I wrong about what the purpose of this section is? Or am I skipping something?

[ger21]

You need to use G41D# or G42D#, and enter the diameter in the tool table. The D is the tool number.

[CitizenOfDreams]

Stupid question - how does the controller know which way to compensate the radius?
Let's say, I'm running this code that cuts a square:
G0 X0 Y0
G1 Z-1
G1 X5
G1 Y5
G1 X0
G1 Y0

How would the controller know whether I am:
- cutting out a square part (the path should be offset one way);
- cutting out a square hole (the path should be offset the opposite way);
- engraving (the path should not be offset at all)?

[jimgeo7]

AHH! I figured it out. You can enter the tool diameter in the DRO but it's not a very well documented procedure as far as I can tell and isn't straight forward at all. So I've been testing this for about the last two hours (very hit and miss) and finally this is what I've come up with. My default tool size cutter is .375 but the actual size out at my shop is .342 the difference being of course -.033. That's the number you enter into the DRO, -.033. Then in your G-code you edit a G41 or G42 depending on which direction your cutting, Climb or Conventional. Also have a tool change in your G-code ahead of the G41 or G42 and you have to edit a G40 when you're finished using it or Mach3 wont even load it. Below is an example of what your code would look like. After testing it and running the numbers to make sure it works I'm confident this is how it's done.

G20 G90 G91.1 G64 G40 G0 Z0.25 ( T1 : 0.375 ) T1 M6 ( Pocket1 ) G17 M3 S19000 G4 P15 G41 G0 X0.7787 Y0.4257 G0 Z0.0625 G1 F120.0 Z0.0 G3 X0.7075 Y0.4755 Z-0.0154 I-0.3212 J-0.3832 G3 X-0.0425 Y0.0425 Z-0.2 I-0.25 J-0.433 G1 Y-0.0425 G1 X0.0425 G1 Y0.0425 G1 X-0.0425 G1 X-0.1175 G1 Y-0.1175

[ger21]

That's really not the way that Comp in Mach3 is designed to work. Your CAM program is doing the offset, and you want to use comp for wear offset. Mach3 doesn't support wear offsets in the normal way.

[jimgeo7]

I'll be going out to the shop today at some point, It's a couple of miles from where I live, and test this on my router. If it works as well as my testing at home seems to show it does, I won't be caring if the programs designed to do offsets this way or not, I'll be doing this way. Of course only if it actually works.

[reuelt]

Did you get it going?
I think ONLY Tool # 0 (zero) is reserved for manual entry at the DRO.
Tool #1 and above are usually added into the MACH3 the tool table or added there by a CAM program you use.
If you change at DRO, you will stuff up the table and your previously working Gcode program will start running incorrectly - since Mach 3 will keep changing & storing the values in the tool table of tool #1 and above.

[jimgeo7]

I lost track, I started getting busy with a change in product and R&D went a little crazy.

Did you get it going?
I think ONLY Tool # 0 (zero) is reserved for manual entry at the DRO.
Tool #1 and above are usually added into the MACH3 the tool table or added there by a CAM program you use.
If you change at DRO, you will stuff up the table and your previously working Gcode program will start running incorrectly - since Mach 3 will keep changing & storing the values in the tool table of tool #1 and above.

That’s not what I found to be. This is how I interpret the wear offset to work in Mach3. In Tool Information, once you load G-code, the tool number given in the G-code is displayed in the “Tool DRO”. Mach3 uses the G-code “T#” as a reference. Example: T1 points to the “Tool Table, tool 1” the Tool Table reference is posted in the DRO’s. There is no reference to tool diameter or height in G-code that is read by Mach3 ergo, (T1 0.25 which is not read in this form). The G-Code and Tool Table have no other relationship than that of reference.

Now, I have a tool that is marketed as .375 diameter. I’ve had it sharpened a few times so now its .355 D. the difference is .02. Since you’re only cutting on one side of the cutter divide .02 by 2 and your wear is .01. In the Diameter DRO you enter -0.01. Mach3 requires that you have a lead-in and lead-out of at least one diameter to start and end cutter comp. Now comes G40, G41 and G42, and this is where I could write a small book. Basically, you can use cutter comp. to compensate either side of the cutter you need. That is, other than what is “Correct” small simple edits to the G-Code can fix a lot of mistakes that may otherwise require large cumbersome edits. That was a hint if you missed it. That is, if you find the cutter is not cutting as close to tolerances as you expect you have a lot of control over the cutter path in the Dia. and H DRO’s.

It’s very important to write a G40 when you’re done with cutter compensating.

[reuelt]

You are correct as long as you are NOT pre-entering (populating) tool diameter, tool length and tool wear data into the MACH3 tool table as done in machines with auto tool changer.

If you are manually changing diameter etc when the machine stops for tool change, what I am saying is you can always specify t0 in gcode for tool#0 for that.
G41 & G42 should retrieve the tool diameter, tool length and tool wear data from the tool# specified in the tool table otherwise AUTO TOOL CHANGERS will not be able to work without operator intervention.

[jimgeo7]

I've never used a tool changer. In the event that I do I'll keep this in mind. Thanks for this. Would it be possible for you to explain the use of T0 a bit further?

[RCaffin]

Not sure whether this affects you, but you should use T0101, not T1. The two parts of the T number are 'tool number' and 'table number'. It is best to to always use T0non rather than Tn.
Well, that's how I read the Mach3 manual.

Cheers
Roger

[ger21]

Not sure whether this affects you, but you should use T0101, not T1. The two parts of the T number are 'tool number' and 'table number'.

That's for Mach3 Lathe, not Mach3 Mill.

[RCaffin]

@Gerry

Indeed. I don't bother with T codes in Mill, but I use Tnn a lot in Turn as I am set up for gang tooling.

Cheers
Roger