Future software update...

[dezsoe]

You can change tool diameter during code run, you just need to update the source. E.g. you can have a memory variable that a macroloop changes when needed. Here is a little code samle (with bad approach ). I wrote fix numbers in the G10 L1 lines, but if you write #variable then it updates while running.

Code: Select all

G10 L1 P48 R1.5
G17 G40
G0 X0 Y0 Z10
G0 X2 Y2
F500
G41 D48
G1 Z0
G1 X5 Y5
Y15
X15
G10 L1 P48 R1.4
G41 D48
Y5
X5
G0 Z10
G40
G1 X0 Y0
M30


[awschmitz7]

And as I explained before about how I'd stop a program mid cut to add/subtract from the tool wear (or as been mentioned here, simply modify the tool radius for example), would UCCNC recalculate the tool path from the mid cut restart point.

I.E. UCCNC would have to be programmed to "take note" that a tool radius had been modified mid cut. I have no idea at present how it works if tool radius compensation was working. Would it just look at the TRC at the beginning of a cut, and not again ??

I’m not sure what you mean by modifying tool radius in the middle of a program. Unless of course you forgot to compensate for the exact tool diameter prior to running a program. Where I’m coming from is making these fine adjustments at setup in the controller itself prior to running a part. I believe Mach software allows you to do this. I may be wrong. It’s not a deal breaking feature to have, like I said, I can program my cam software with these values in mind. It’s more of a convenience factor being that I don’t have to readjust my actual tool values in cam if my tool has wear or I’m using a brand new tool.

[cncdrive]

You can change the tool diameter value any time. For example if your tool dia is 6mm, but it worn out to 5.95mm then you can type in the new tool dia value.

[ger21]

As I said before, the current test release of UCCNC supports G41/G42, which allows you to do this. There are still some issues with lead-in moves, but other than that, it seems to work well.

As Terry said, you must use G41/G42 for tool compensation.

Mach3 does not have a wear offset, but Mach4 does. But you still need to use G41/G42.

[limited660]

Just to add some information, the tool comp information is only updated when the offset is called. In Fanuc this is typically done by using H and D words. You can change the offset in software but it doesn't change compensation until the H/D word is run.

M6 T5 - Loads tool 5
G43 H5 - Loads tool 5 height offset
G41/G42 D5 - Loads tool 5 diameter offset

Wear offsets on lathes are a little different as they apply without cutter compensation but still are not updated until a command like T0544 is called (T05 = index tool 5, 44 = load offset 44, they are usually the same numbers but I changed them for easier understanding).