[MikeMeezy]

Hey guys, new to the forum and the CNC machining world...always looked at threads and never really had a question until now. I'm currently working on a VF-6, I have these steel blocks with toolpath from my CAD room using cutter comp to mill tight tolerance pockets. I have to make a drill program for 5 holes. I had no trouble making a full program until I realized I had to drill one hole on a different surface on the lower end of these blocks. I was wondering what was the most efficient way to do this in the same program. Maybe using a z offset somewhere in the program or having a separate offset code from my G54 that I use for everything else. I'm pretty new to machining and even the guys with years of experience that are training me can't figure it out. They don't know the Haas controller like I do, I took the operator class and programming class Haas offers for any company for free with the purchase of a machine. Any advice will help me. I appreciate it.

[Geof]

Read about G52 in your Manual and do a search here on CNCzone about G52. It is a way a creating a secondary work zero within your main work zero.

[moriboy1]

Here's two solutions:
(Hopefully you are using canned cycles)

When you position over to the hole that needs to be deeper, just change your Z- for that hole only. You can also change the R to a - value too if you don't want to cut air.

Drill all holes on the same plane, cancel canned cycle. Position to the hole that is on a different plane, make a new canned cycle for that hole.

[MikeMeezy]

Ok I understand where your coming from for the hole on the other plane by making a new canned cycle for it, but would I change my R or my Z? Can you give me an example from a normal drill program to a different program with a different plane? Would I have to use a G98 or G99 to bring Z up far enough to clear the part? Thanks for the help guys.

[MikeMeezy]

I don't think I quite understand using the G52 code either :/ like I said I'm
new to machining

[obiwon]

Lets say surface A is 1.00in higher than surface B. Set your tool offset to surface A.

T1M06 (DRILL)
G00 G54 G43 G90 H1 X1.00 Y1.00 (surface A)
S2500 F25.
G00 Z.1(surface A initial point)
G81 G98 R.1 Z-1.00
G00 X2.00 Y1.00 (surface B)
G81 G98 R-.9 Z-2.00

You will drill both holes 1.00 in deep starting from .1 above each surface. The drill will return to the initial point of .1 above surface A after each canned cycle call out

[Geof]

This is how you would do it using G52 to offset the Z work zero 1.00" down.

T1M06 (DRILL)
G00 G54 G43 G90 H1 X1.00 Y1.00 (surface A)
S2500 F25.
G00 Z.1(surface A initial point)
G81 G98 R.1 Z-1.00
G00 X2.00 Y1.00 (surface B)
G52 Z-1.0
G81 G98 R.1 Z-1.00
G52 Z0.0

As I said read the manual and search on here about G52. Everybody at one time was new to machining and didn't understand things. The path to understanding is reading and working examples, many of which are available on this forum.

[rlockwood]

That's ludicrous, why in the world would you use g52 in this instance? Just call another subroutine and use a negative R value.

Much safer.

[moriboy1]

That's ludicrous, why in the world would you use g52 in this instance? Just call another subroutine and use a negative R value.

Much safer.

100% agree. G52 had its place when there were no canned cycles, no reason to do it that way now, IMHO.

[Geof]

Why thank you, I never knew before that I was ludicrous.

[moriboy1]

Why thank you, I never knew before that I was ludicrous.

I think the main thing here is that you can get into trouble sometimes using G52. For a new programmer, we never even teach our guys to use it. I do agree it is a valid way to do what the OP is asking. I for one do not think you are ludicrous, my apologies for agreeing with that part of the statement.

[BlueChip]

Here's a link to our Blog where we posted an article on this subject ... hope it helps :
Making Chips: Canned Cycle Drilling and R Plane Tricks

Real World Machine Shop Software at Kentech Inc. - Real World Machine Shop and CNC Software

[Geof]

I think the main thing here is that you can get into trouble sometimes using G52....

Are you sure you are thinking about G52 not G92?

I cannot imagine how it is possible to get into trouble with G52 but it is very easy with G92 because they work differently: G92 changes the primary work zero location and after a few G92 commands it can be difficult to remember where you are. Also the work zero stays changed and if a program stops part way through it is almost certain you don't know where the work zero is and it is not easy to get back to the original location.

G52 does not change the primary work zero. The G52 coordinates are stored in a G52 register; if you look at the Haas offset screen it is at the top. The contents of this register are always included by the controller when it does a calculation for moving an axis. If the value is zero of course it has no effect but when a value has been entered by the G52 command that value is combined with the primary work zero location to give a secondary work zero which is used. In Haas mode the values in the G52 register are zeroed by RESET and M30 and can also be zeroed by using G52 X0. Y0. Z0. so you cannot get lost because once these values are zero G52 has no effect and you are back working in the primary work zero.

[rlockwood]

Eh, I guess I just never looked at that as an intended use for G52. Just don't forget to zero it out when moving on.. OTOH, I make good use of G52 for patterning/repeating on a regular basis.

Its much safer to maintain an I plane above the part, and use an R plane to minimize air cutting. If you're certain the pattern is clear, switch to g99 to minimize retracts. When you're done, G80 will cancel everything with no chance for any remaining offset.

I dunno, there's certainly a billion ways to skin a cat.