[pwilson101]

Hi,

I have a CNC programming question. I am pre-drilling a hole with a carbide drill for a long HSS drill which will follow. The HSS drill doesn't have thru-the-tool coolant capabilities and I wanted to save time by drilling as deep as I could with the carbide drill first. Anyway, I have to peck with the HSS drill, which I know is a G83 with a Q-value. My question is, how would you program this so the drill retracts all the way back to the R-plane of the solid carbide drill after each peck? Is there a way to do this in a canned-cycle, or am I going to have to program this point-by-point? Obviously, I'm trying to accomplish this without point-to-point programming.

Control is a Mitsubishi Meldas 500M.

Thanks for any help.

[BlueChip]

The MITS control, I believe is "fanuc compatible" ... so Fanuc G codes apply.

You should have two choices when it comes to Peck Drilling :
G73 ... is a simple chip breaking cycle ... tool just backs away a parameter set amount to break the chip.

G83 ... which is what you atre looking for ... is a "deep hole chip breaking" cycle. Here the tool retracts to the R plane to break the chip.

Hope this helps.

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

[uperez]

I believe he wants to start off the drilling right at the depth the carbide drill had made but wants to retract the tool outside the hole to cool it off. I'm not sure if this is possible to Mits and Fanuc control, but in Okuma it's easy.

[BlueChip]

Dddooohhhh!! Stupid me ... that's what happens when you don't read.

I don't believe this is possible in any standard "canned cycle" routine.

You'll need to think outside the box :

(1) Do something incremental with sub programming ??

(2) If you're control has macro ... good time to write a macro which you could re-use as needed in the future.

(3) Tooling change / re-think the process ?

Sorry ...

[ChattaMan]

This will work on a Fanuc control. I don't know anything about the Mitsubishi Meldas 500M language. Just alter the values for #501-#504 to suit your needs.

N1T1M6(HSS DRILL L/S)
M1
G0X0Y0G54S500M3
G43Z10H1M8
F100

#501=1 (R PLANE)
#502=-50 (START DEPTH)
#503=-100 (END DEPTH)
#504=2 (PECK SIZE)

G0Z#501
#505=#502-#504
N100G0Z[#502+0.5]
G1Z#505
G0Z#501
#502=#502-#504
#505=#505-#504
IF[#505GE#503]GOTO100
G0Z10M9

N2T2M6(NEXT TOOL)

[uperez]

The statement IF[#505GE#503]GOTO100 is dangerous if you have controlled depth. You have to consider the depth where you're starting because the increment in every cut is 2inches or 2mm whichever you're using.

should be like this

N1T1M6(HSS DRILL L/S)
M1
G0X0Y0G54S500M3
G43Z10H1M8
F100

#501=1 (R PLANE)
#502=-50 (START DEPTH)
#503=-100 (END DEPTH)
#504=2 (PECK SIZE)

G0Z#501
#505=#502-#504
N100G0Z[#502+0.5]
G1Z#505
G0Z#501
#502=#502-#504
#505=#505-#504
IF[#505LT#503]GOTO200 (depth check)
IF[#505GE#503]GOTO100
N200G0Z[#502+0.5]
G1Z#503 (drill to correct depth if remaining depth is less than 2)
G0Z#501
G0Z10M9

N2T2M6(NEXT TOOL)

[ChattaMan]

uperez

Thanks for the correction. Just did it off the top of my head.

At least the guy can now get on with his job rather than just knowing someone can do it easily on their Okuma.

[uperez]

..was actually going to write the codes but was really busy with the set up

The question now is if the machine is macro b capable.

[fordav11]

I worked a Meldas 500L that had Fanuc compatible Macro B. so the controller is capable if the machine has the option. not sure if it's an option or every Mitsubishi Meldas has it as standard.

[ChattaMan]

So uperez....

how do you do this on the Okuma? I've now got a job that needs this very same routine, would you believe. I can't see in the manual how to do the retract in the canned cycle.

Cheers

[fordav11]

its very easy on Okuma because they built it into the peck drilling G code.
About a dozen manuals are supplied with the machine. the info is in the 'Programming' manual.
if you tell us the control type someone may be able to point you to the exact pages.

[ChattaMan]

Control is P200M
I looked in the Programming manual but couldn't see a retract, after each peck, above the R plane. I could only see a final retract to R plane, stated height (G71) or machine zero.

[fordav11]

I'm a 9-axis L-Man (lathe) so I can't help with Mill-specifics :-D
but here's the G183 Deep Hole Drilling Cycle + other pages related to setting the reference plane/initial point and repeat from P200L manual. You should have similar pages in the P200M manual.

[ChattaMan]

Hmm ok, thanks for the info. But.....
The origional poster and my example were asking for a milling example.

I have seen the example, you attached, in our Multus manual with P200L control, only the milling and lathes cycles are different. I have used the L and D in the G183 cycle on the Multus but they still only retract to the cutting point.
If the cutting point is below the surface it's still the same problem. If you start drilling (cutting point) at Z-30 it will not retract to Z0 after each peck.
L and D are just different peck types. When peck L is performed it still only retracts to the cutting start point. Or have I missed something.
But tell me if I'm wrong.
In the G183 cycle which letter do you use to tell it to retract above the cutting start point
G183 X Z C I F E D L

I'm babbling on now!! The Lathe and Mill cycles are not the same so it's irrelevent. The question is still unanswered. How do you retract above the R plane, easily, on an Okuma.
BTW, this is still a G-code question. So we are still in the right forum section...just.

[pwilson101]

Hello. I am the original poster and I just got back to checking this out, thanks everyone for helping me out. I'm having some trouble follow the macro, though.

I get lost when it starts with: IF[#505LT#503]GOTO200 (DEPTH CHECK). What are we trying to determine & do in this line? I would think at first glance that you are trying to see if the final drill depth has been satisfied, and if not, then peck drill again. But if you follow the macro to N200, it is rapiding above the last drilled depth by 1 (that's fine), but then it's feeding to the final drilled depth WITH NO PECK. What if you had more than the 2 you wanted feed before pecking? Thats what I see anyway, but I'm far from an expert at this, so I'm sure you are correct and I just don't understand, so could you help me understand?

Thanks

[pwilson101]

Instead of "IF[#505LT#503]GOTO200", shouldn't you write something like "IF[#503-#505LE#504]GOTO200"? Because after the program goes to N200, it is just rapiding above the previous drilled depth, then drilling to the final depth, with no peck, and with "IF[#505LT#503]GOTO200", isn't that just asking if the last drilled depth is less than the final drilled depth, go to N200, regardless of the amount of difference between the two? --- I don't see where it's checking to see if the remaining depth is less than 2 (the peck depth).

So that's what I don't understand ... how the line "IF[#505LT#503]GOTO200" is checking if the remaining depth to drill is less than 2, because if you follow the macro after this line to N200, the rest of the program just drills to the final depth regardless of the how much is left when it should only do that if it has 2 or less to drill.

What am I missing? Thanks again for any help....

[ChattaMan]

#501=1 (R PLANE)
#502=-50 (START DEPTH)
#503=-100 (END DEPTH)
#504=2 (PECK SIZE)

G0Z#501
#505=#502-#504
N100G0Z[#502+0.5]
G1Z#505
G0Z#501
#502=#502-#504
#505=#505-#504
IF[#505LT#503]GOTO200 (depth check)
IF[#505GE#503]GOTO100
N200G0Z[#502+0.5]
G1Z#503 (drill to correct depth if remaining depth is less than 2)
G0Z#501
G0Z10M9

Simple Example: R1 Z-10 Q2

So you drill your hole starting at Z1
Pecking 2mm
Next to last cut will reach Z-9
Another peck of 2mm would take it to Z-11
This block...IF[#505LT#503]GOTO200...means...if next cut Z-11 (#505) is less that finish size Z-10 (#503) jump to N200
Z-11 is less than Z-10 so it jumps to N200 where it rapids to Z-8.5 and drills to Z-10, so a last peck of 1mm + 0.5mm of clearence (which is less than the peck size of 2mm)
It will never peck more than 2mm

My example was simpler to understand for beginners but the programmer has to make sure the total drilling will be divided equally by the peck amount.
To drill from Z1 to Z-10 will not divide equally by a peck of 2. So the final depth would end up at Z-11. So uperez added the extra check to avoid this and it will now only drill to the total Z depth and not beyond it. Meaning any size peck can be used.

[pwilson101]

Ah ha! I didn't follow it all the way thru. I see where #505=#505-#504 it would put it at -11, and -11 is less than -10 (dang minus numbers had me messed up with the less than stuff), and etc etc. It's clear now to me!

Thanks for the help! Much appreciated!

[NIRAV1OO7]

Hello
I got one job today. 360 brass,Having 6 Npt threads in a single part itself.
fortunately i have program ready, but I do not know how it was created. its 1/8-27 nptf thread.
according to the charts for internal thread i should drill .332?
My question is I do not know how to produce codes in mastercam as there is no thread tool available
in the standard library of mastercam X5. I Google it and i found thread milling by single point tool. but this program didnt support for thread mill tool.
can anyone tell me how to use or create thread mill tool and its program.
it will be much appreciated.