[Joe2014]

I'm new to CNC machining and just recently converted a G0759 mill to CNC using Hoss designs and recommendations. All appears to be working well but I just ran into the following problem with peck drilling cycles. This probably isn't the correct place to post the problem but thought someone here could point me in the correct direction.

I generated a fairly simple G Code file via CamBam and when I tried to machine the part I ran into problems with the peck drill cycle. Specifically, the first hole or drill cycle is the problem, all holes following are fine. The first hole cycle appears to jump high speed down about .25 inches at the end of each peck. The drill lowers at the correct feed rate of 5.0. The drill then appears to drill down .125” as expected but then the drill goes high speed down another .25” and then retracts out of the hole high speed to where it started. For some reason MACH, or maybe my controller board AKZ250 is adding the additional .25” high speed plunge at the end of each peck.

Strangely, the second peck drilled hole in the G file works properly. I’ve even ended the drill cycle and started a new one in the G Code and it also works fine, just the first hole of the first peck drill cycle in the G Code file behaves this way.

Below is a simple code snipet that demonstrates the problem on MY system which is running MACH3 Version R3.043.066 on Windows 7 and talking to a AKZ250 USB interface controller.

Any help or advice appreciated.

G20 G90 G91.1 G64 G40
G0 Z0.125
M3 S2200
G0 X-0.613
G98
(the following peck cycle exhibits the problem)
G83 X-0.613 Y0.0 Z-0.6 Q0.125 R0.125 F5.0
(the following peck cycle works properly)
G83 X0.613 Z-0.6
G80
G98
(the following two peck cycle work properly)
G83 X-0.613 Y0.0 Z-0.6 Q0.125 R0.125 F5.0
G83 X0.613 Z-0.6
G80
G0 Z0.125
M5
M30

[onocyclone]

Hi man,

Im quite sure that the line where it says :

G20 G90 G91.1 G64 G40

you can't have a decimal G Code. It should be G20 G90 G91 G64 G40.......

I think this is correct but don't hold me to it

[Joe2014]

Actually, I'm pretty sure the G91.1 code is valid. It’s documented in the MACH3 G Code screen as “G91.1 Set IJK Arc Mode”. CamBam inserts it into all of the G files I've generated and MACH seems to accept the code.

After my original post, I did some more researching and I think this is a MACH3 bug first reported over a year ago. The original report indicated the problem was random G83 Random Bug. Final status seemed to be no solution offered by MACH support and user stopped using the canned G83 (peck drill) cycle.

I just documented my version of the problem on their support forum so will wait to see what they say.

[SCzEngrgGroup]

Hi man,

Im quite sure that the line where it says :

G20 G90 G91.1 G64 G40

you can't have a decimal G Code. It should be G20 G90 G91 G64 G40.......

I think this is correct but don't hold me to it

That is not correct. There are quite a few "decimal" G-codes, including G91.1, which sets increment IJK mode for arcs, G90.1 which sets absolute IJ Kmode, and G59.n which gives you 255 fixtures.

What version of Mach3 are you using? Pretty much ALL have bugs, and I've seen some in drill cycles, worse than what you're seeing. The latest version (066?) is especially buggy, and should not be used at all.

Regards,
Ray L.

[Joe2014]

That is not correct. There are quite a few "decimal" G-codes, including G91.1, which sets increment IJK mode for arcs, G90.1 which sets absolute IJ Kmode, and G59.n which gives you 255 fixtures.

What version of Mach3 are you using? Pretty much ALL have bugs, and I've seen some in drill cycles, worse than what you're seeing. The latest version (066?) is especially buggy, and should not be used at all.

Regards,
Ray L.

As stated in my original post, I'm using MACH3 Version R3.043.066. I'm drilling aluminum mostly and not very deep so I will try switching to a normal G81 Drill Cycle instead of pecking, hopefully that will work. Or... would you suggest I load an older version of MACH?

[SCzEngrgGroup]

I would definitely suggest an older version of Mach3. The guys on the ArtSoft forum can tell you for sure what the "best" version is, but they will also tell you not to waste time with 066 - it has many major problems. I believe 060 is considered pretty stable.

Regards,
Ray L.

[Joe2014]

OK, thanks for the information Ray, will first try regressing my MACH version to 060 before giving up on the peck drilling method. - Joe

[ger21]

G20 G90 G91.1 G64 G40

Unrelated to your issue, but you want to put G90/G91 and G90.1/G91.1 on separate lines.

G20 G90 G64 G40
G91.1

They are in the same modal group, and when they share a line, only the last one will be applied.
You can check by putting your machine in G91 mode, and then loading and running your code. It will stay in G91 mode, even with the G90, because of the G91.1