[JetForMe]

Gcode lets you specify which tool you want separately from which tool offset you want. Usually, these two are the same (e.g. M6 T7 G43 H7).

Does anyone ever really use different numbers for these commands? E.g switch to tool 2 but use the offset for tool 4?

[metalmayhem]

there are occasions where it can be helpful but for the most part it's not common . D comp on the other hand - there are many occasions for needing multiple numbers . Some machines will trip an alarm if the h is different from the tool number , but that can usually be resolved in the parameters

[JetForMe]

Can you give me a real-world example of using separate tool & offset numbers?

And what's D-comp?

Thanks!

[metalmayhem]

I've done it in the past but off hand can't think why , it was a matter of having 2 separate heights . Otherwise ethers no reason to have the numbers different .
d comp is diameter compensation , complex parts may at times need a different diameter comp with the same tool on the same part

[JetForMe]

Can you think of a D-comp example? I appreciate it.

[metalmayhem]

if the tool is cutting the part larger or smaller than wanted then you would use diameter compensation . I suggest you read up on g41 and g42 , it should make sense after a bit of reading

[JetForMe]

I get how G41 & G42 work, but why would you ever write it with a "D" parameter different from the current tool number?

[metalmayhem]

every job has different situations , sometimes one bore for example is coming out to perfect size while another portion of the part isn't coming to nominal size with the use of the same tool , This is where you'd use a separate d comp

[JetForMe]

Interesting, okay. You wouldn't just specify that with an O word?

[Superman]

I get how G41 & G42 work, but why would you ever write it with a "D" parameter different from the current tool number?

In my situation, the machine doesn't have H & D offsets, it has G & W (geometry/wear), where each G&W are added together
for one total offset ONLY.
So for me for each tool used.... T# , G#(tool length) , G[#+30](tool radius)
Tool length & radius offsets are still called up by using the H & D addresses.

[deadlykitten]

Does anyone ever really use different numbers for these commands? E.g switch to tool 2 but use the offset for tool 4?

hy here are a few examples :
... lathe :
...... using 16 tools on a turret that handles only 12 posts
...... a quad toolholder, that can handle 2 tools towards main spindle and other 2 tools, towards the 2nd spindle
...... a normal drill that has also a chamfering attachement
...... an u-drill, that also delivers id turning
... mill :
...... 90 degree chamfer end mill, that can use 2 different diameters ( among it's cone ) in order to chamfer same part
...... a drill that also cuts the counterbore
...... a 90 degree atachement that has 2 chucks
... gauging :
...... a probe with non standard linear stilus, but having a cross/plus apearcane ( uses 4 rubies )
... operating :
...... using same finish tool, with different offsets, for 2 different diameters

such situations are refered in practice as using a multioffset tool, a combitool, a multi edge tool, a combi holder, etc / kindly

[Superman]

Err kitty.... it's a milling forum