G41\G42 Haas mill-turn.

[uladzimiruser]

Good day to all. I was interested in this question. When boring a hole on the Haas ST 20 ssy with a radial cutter and the adjusted setting, the type of compensation in the rack. During postprocessing, there is no parameter D (tool number) next to parameter G41 or G42. Where in the postprocessor is it possible to add or add? Or do you need to add this parameter yourself?

[AchimN]

As far i am aware of this is not needed on the lathes since offsets are called with the tool call itself. There is no D-value in any of the programming examples into the lathe / live tool manuals.

[uladzimiruser]

For a tool, yes. But when milling the boring (milling cutter) of the exact holes as indicated?

[AchimN]

As said, i did not see that in ANY sample program for milling on the lathe, there is also nothing mentioned about it into the manuals. Do you have issues with it?

[uladzimiruser]

In general, no, but sometimes it is necessary to indicate in the program a smaller diameter of the mill. For example, instead of a cutter with a diameter of 8mm, I specify 7.9mm. Or in the opposite direction.

[uladzimiruser]

Here's what is written in the manual to the machine:

---

G17 Plane XY / G18 Plane XZ / G19 plane YZ (Group
02)
This code defines the plane in which the path is traversed
tool. Programming the tool nose radius compensation G41
or G42 applies a tool radius compensation in the plane G17, independently
whether G112 is active or not. See the chapter "Tool offset" in the section
"Programming", which contains detailed information. Selection codes
planes are modal and remain in effect until selected
another plane.

This is if the processing is done without G112.

And this is a note, if with G112.

NOTE: When using G112, the tool offset is turned on
type cutter. The tool offset (G41, G42) must be
canceled (G40) before exiting G112.

With prolonged processing, tool wear (milling cutters) takes place and run constantly and make changes to the program is not very desirable.

[Laurens-3DTechDraw]

---

@uladzimiruser wrote:

Here's what is written in the manual to the machine:

---

G17 Plane XY / G18 Plane XZ / G19 plane YZ (Group
02)
This code defines the plane in which the path is traversed
tool. Programming the tool nose radius compensation G41
or G42 applies a tool radius compensation in the plane G17, independently
whether G112 is active or not. See the chapter "Tool offset" in the section
"Programming", which contains detailed information. Selection codes
planes are modal and remain in effect until selected
another plane.

This is if the processing is done without G112.

And this is a note, if with G112.

NOTE: When using G112, the tool offset is turned on
type cutter. The tool offset (G41, G42) must be
canceled (G40) before exiting G112.

With prolonged processing, tool wear (milling cutters) takes place and run constantly and make changes to the program is not very desirable.

---

Yes the G41 and G42 are added to the program.

In the mill you need G42 Dtoolnumber in the lathe you just give G42.

That's what Achim is trying to explain to you.

So the in control compensation works, but it doesn't need a D value in the lathe's.

[uladzimiruser]

I understand, but after the postprocessing in the program there is no D parameter. Is it necessary to add it to the manual? For example, in the program for milling machines, the reference to the corrector is made by parameter H.
G43 Z15. H1

And in the turning milling machines, parameter D is picked up automatically when selecting a tool? And if I want to use a corrector for another tool? Tool T5, and the corrector 25.

[Laurens-3DTechDraw]

---

@uladzimiruser wrote:

And in the turning milling machines, parameter D is picked up automatically when selecting a tool?

---

Yes. When you select a tool it automatically selects length and diameter offsets. So D does not exist. 

Haas lathe tool and offset numbers work like this:

T303 is turret number 3 and offset number 3

T509 is turret number 5 and offset number 9

I believe T3 would automatically also set the turret to 3 and the offset to 3.

So during the tool change you set the offset value's you want.

[uladzimiruser]

Then why when choosing a tool in the program, the corrector for the diameter does not change in any way, and when the length corrector is changed, the corrector in the program changes. Can there be an error in the program?

[Laurens-3DTechDraw]

Because in a Haas Lathe the Length and Diameter offset will always be coupled.

So we could edit the post so that in the CAM you have to have the Length and Diameter the same or it to error out.

But the default is T(toolNumber)(ToolLengthOffsetNumber)

And the diameter or compensation offset is not used because haas lathes only allow for Tool/Turret Number and one number for the line in the compensation table.

[uladzimiruser]

Thank you.