[dneisler]

I was machining a part tonight with a tool clearance level of Z.4", when I drilled the hole and it attempted to go to the next it broke my bit.

Not sure what this code means, I know I do not have tool off set in use.

%
N5 G0 G40 G49 G80 G20 (Initialization)
N10 G0 G53 X0 Y0
N15 (Tool # 2 - Diameter 0.328 D2 H2)
N20 T2 M6 D2 H2
N25 S1200 M4
N30 M8
N35 (D-Hole.Drill-T2)
N40 G0 G54 X0.34 Y0.604
N45 G43 H2 Z0.4
N50 G83 Z-0.588 R-0.171 Q0.063 P2000 F2
N55 X2.282 Y0.622
N60 G80
N65 G0 G53 Z4 M9
N70 G0 G53 X0 Y0 M5
M30
%

Any idea what went wrong?

[Geof]

It is possible you had G99 R Plane Return active not G98 Initial Point Return.

With G99 active your drill would have been at the R position when it moved to the next hole.

I think it is a good practice to include G98 in the initialization line just to be safe.

[Mitsui Seiki]

You need a G98.

[dneisler]

Wow, over my head.
I was just using solidcam at my wifes work to do this project. I just did a peck drill cycle with it. How do I do a G98, I thought it would do all that for me or there is something simple I am leaving out.

[Mitsui Seiki]

Just put it in this line:
G83 G98 Z-0.588 R-0.171 Q0.063 P2000 F2

[Geof]

Wow, over my head....

Do a bunch of reading before pushing buttons if things are over your head. The simple thing you are leaving out is an acknowledgement that the software and machine cannot make up for an incompetent operator who is unwilling to learn enough to be safe. You were lucky, with a small drill pulling the trick you pulled breaks the drill, with a large drill you can break the machine and have large pieces of drill shrapnel flying around.

[dneisler]

Geof,
I do understand what you are saying. I have spent many hours learning and getting machine time, and I believe I am competent enough to keep my self safe. One of the reasons my machine is totally enclosed too. I do admit that drilling I have done little of and probably should read a little more and figure it out. What i do not understand is, should the CAM package put the G98 in?

Off to read...

Happy holidays everyone.

[stevo1]

From what I understand about Cam software is that it is pretty standard and you must modify your post processer to input the “special” things that you need for certain machines into your code.

I am not sure what kind of control you are on but most machines that I run G98 is the default code so it should have came to your initial Z of .4” before it moved to the next hole. It could be that your machine is set for R-plane return.

The first line before you enter into your canned cycle mode has to have a Z, this will establish your “initial level”. This you have with your G43 H2 Z.4. Your initial level is .4”. Now in your canned cycle line you establish your R level with the R-.171. Your R level is -.171”. This is below your part. If you have a G98 in your canned cycle line your tool will move to the initial level before going to the next hole. If you have a G99 your tool will move to the R level before moving to the next hole. As you can see that is a problem for you given your R level is below the part.

I never use G98 or G99 given the fact that every machine that I have is G98 default and I never have a reason to retract to the R level when moving hole to hole. Check your book for the control and see if maybe you have parameter that can change the default code from G99 to G98. It strikes me as pretty odd that your G99 is default I have never seen that before.

Stevo