F360 - returns to machine zero not work offset

[routercnc]

Hi Charlie,

When you post process the toolpath you get this menu:

(red box)
Select G28 - no
I've also looked into searching the post processor library (green box) and there is another Mach3 PP in there which mentions various features including G28. I'll look into that.

Hi Neale,
Here is the code comparison with and without G28:

1) With G28
OP3_COUNTERBORE_6MM_0P5_300)
(0.5MM PITCH)
(T1 D=6. CR=0. - ZMIN=-15. - FLAT END MILL)
G90 G94 G91.1 G40 G49 G17
G21
G28 G91 Z0.
G90

(BORE1)

... boring operating in here

G0 Z15.

M9
G28 G91 Z0.
G28 X0. Y0.
M30
___________________________________________

2) Without:
(OP3_COUNTERBORE_6MM_0P5_300_NOG28)
(0.5MM PITCH)
(T1 D=6. CR=0. - ZMIN=-15. - FLAT END MILL)
G90 G94 G91.1 G40 G49 G17
G21

(BORE1)

... boring operating in here

G0 Z15.

M9
M30

I've not run the without G28 code on the machine but the last G0 just moves to Z15 above the feature just cut, not the work offset zero. Might be good enough.

[Clive S]

I think you need to edit the F360 post. as a workaround you could just hand edit the file in notepad and change the G28 to a G0 and put the numbers in where you want it to go. Don't quote me though

[Neale]

I think that the use of g28 by F360 and what happens with g28 in Mach3 show how there are differences in interpretation. F360 takes a fairly strict interpretation so throws in a G91 Z0, which should mean that the tool goes to the tool change point via machine coord Z0. However, Mach3 treats G28 as "go to SafeZ, then move to tool change point", making the G91 Z0 redundant. Generally, a safe option but I'm not sure if it is documented, just what I have observed. As it happens, my favourite tool change position is close to the corner of the bed where I normally have work zero, so it's not much of an issue for me - not too much unnecessary tool travel. Remember that it is easy to set the g28 position so if you are doing a big job, it might be worth temporarily changing it.

I'm guessing that for this F360 CAM you have the clearance height (is that the right one?) set to 15, so as far as F360 is concerned, this is a safe z value.

My personal bete noire is the M6 start/finish macro sequence, because what I want it to do might vary according to whether I shall be doing a tool height set/reset in the middle of it. Still working on that one. Especially when you find that the CSMIO plugin doesn't do what it's supposed to...

What it comes down to is that whoever writes the post-processor/Mach3 gcode interpreter etc has their own mental model of the "ideal" work flow, which is a bit of a pain if you work differently

[routercnc]

Forgot to say thanks Graeme. As you can see from the above switching off G28 could be an option for me.

Clive, Neale,
Thanks for your thoughts on it. I thought about editing the code in notepad with find replace (G28 > G0) and am sure that would work, but bit of a pain to do it every time.

I will try and look into the F360 online site of post processors as this mentions a Mach 3 version with various features including something about G28 usage. . . With a bit of luck it will create G0 instead of G28

[charlieuk]

thanks for this will be interested to hear if you figure anything else as I have just got in to using fusion and while mostly great there are a few things throwing me.