Setting cutter radius with G10?

[rcaffin]

I want to use cutter radius compensation.
M3M says that G10 L1 P1 R5 Z6 should set the tool table entry for tool diameter to 10 (and tool length compensation to 6) - although it is rather brief and hesitant about the radius bit.
However, I don't seem to be able to get the radius setting to do anything. The Z parameter works fine.

Would I be right in thinking that this radius/diameter feature has not yet been implemented in Mach3?
Or have I just not done the right thing yet?

Cheers

[ger21]

To use cutter radius compensation, you need to program using G41/G42. You can just enter the diameter in the tool table, there's no need to use G10 to do it.

[rcaffin]

To use cutter radius compensation, you need to program using G41/G42. You can just enter the diameter in the tool table, there's no need to use G10 to do it.

Oh yes, I know that.
But I would like to be able to specify the cutter diameter IN the program because I am cutting multiple units from one blank, and the separation of the units depends on the cutter diameter.
And, ... I may want to change the cutter diameter from 5 mm to 6 mm if the 5 mm cutter proves to be too weak (and breaks). What i don't want to have to do is manually adjust the layout because of the cutter diameter.

Cheers

[ger21]

You can specify the cutter radius along with G41/G42 by using the P word.

G41 P3 for a 6mm diameter cutter. This method doesn't use the vales in the tooltable.

[rcaffin]

You can specify the cutter radius along with G41/G42 by using the P word.
G41 P3 for a 6mm diameter cutter. This method doesn't use the vales in the tooltable.

Bingo! The instructions for G41 were not wildly clear either ...  Thank you.

Just out of curiosity, what about G10 R5 though?

Cheers

[BR549]

I think the G10 calls you are tryng to use are for TURN applications.

(;-) TP

[rcaffin]

I think the G10 calls you are tryng to use are for TURN applications.

Well... M3M does discuss the use of tool diameter compensation, and defines G10 thus:

To set the offset values of a tool, program
G10 L1 P~ X~ Z~ A~, where the P number must evaluate to an integer in the range 0 to
255 - the tool number - Offsets of the tool specified by the P number are reset to the given.
The A number will reset the tool tip radius. Only those values for which an axis word is
included on the line will be reset. The Tool diameter cannot be set in this way.

What I do NOT understand is the distinction between the A number and the tool diameter, which is defined elsewhere (eg EMC I think) as being set by R, not A. Is M3M talking about a square end mill with a radius rather than sharp corners maybe? I don't know, and such a tip radius does not appear in the tool table last time I looked.

My bigger problem at this stage is that if I don't use G41 the outline appears in the window exactly as it should, but when I insert the G41 line the system goes slightly ghaywire on me. I get an arc back to some arbitrary position from every corner, followed by a straight line to the nect corner. BUT, these arcs are superimposed on the correct outline?   Umm.....

Clearly I am doing something wrong, but right now i can't see what. Any suggestions very gratefully received!

Cheers

[rcaffin]

Well, I spent the afternoon creating test programs.
It would seem that if i create a simple shape, largely convex, and go around it with G41 turned on, all is well and compensation works.

But a complex shape (something like a wobbly starfish for instance) sends Mach3 haywire. This may be assisted (I am not sure) by a slightly complex program with quite a depth of embedded subroutines. It can't cope with all the inside corners, and starts arcing all over the place. Well, I have some sympathy.

It also gets upset when I have lots of sharp inside corners in a complex prgram - it complains that the cutter can't do a sharp inside corner. It manages with a simple shape though. yes, I KNOW the corner will come out radiused - that is intentional.

Yes, I have tested my complex programs with the G41 line in and commented out, and that is the determining factor. Pity - it would have been useful. I have reverted to creating the tool path outside Mach3 and not using G41.

Next version maybe?

[RICH]

When things get more complex it can be easier to just use a program which provides offsetting from the profile.
Even the offsetting from programs will provide some strange results depending on what the programs decide is the proper thing to do for
a "foot that dosen't fit the shoe". In manny cases it just plain poor design to begin with.

I don't hand code a lot but a quick look at requirements for G41/ G42 to work right ( Smid's book on programming ) will provide insight into limitations.

RICH


 

[ger21]

From what I understand, G41/G42 doesn't work well with subs. And it really requires inside corners to have a radius larger than the tool.

When I read tool tip radius, I think of turning tools, as Terry said.