Peck Drilling

[RBrandes]

I have to peck drill .128" for about 1/2" at the bottom of a 1/2" deep .136" hole. This is for a 1/8" rollpin. The larger hole provides a guide and makes it easier to assemble the pin and part.
With Haas' peck drill (G83?) and single step, you can't single step! It runs through the entire routine and I can't see the Z values. What I am trying to do is to rapid down to the bottom of the clearance hole and then start peck drilling, yet retract to clear chips to Z+.01. What it seems to do is feed for the first 1/2" cutting air. This is a four-up table load and I am trying to reduce the run time.

[manny007]

Hello Ray, Have you tried adding the .500 depth value to the .128 drill offsett value and starting from there?And if you want it to clear beyond the .500 as it peck drill change the R value in pecking cycle line. example G98 G83 G1 Z-.5 Q.1R.51F10.;
just make sure that the line before this is G0Z1. then the pecking cycle after this line.
hope this helps out a bit

Good Luck

[Ken_Shea]

EDIT:
It is amazing how I read your post 3 times then again only after mypost to find that the code below is not what you are after, sorry.

Let me retry.


Ray,
Here is the code my cam program is putting out using a G83 and Haas post.

%
O0000
T1 M06 (.250 HSS SPOT DRILL 120 Degree)
G90 G80 G40 G54
S3009 M03
G43 H1
/M08
G00 X0. Y0. Z1.
G99 G82 R0.05 Z-0.135 P F18.054
G80
G00 Z1.
M01
T2 M06 (#29 DRILL FOR #8-32 OR 4 X .5MM TAP)
G90 G80 G40 G54
S2808 M03
G43 H2
/M08
G00 X0. Y0. Z1.
Z1.
G99 G83 R0.05 Z-0.5 Q0.05 F3.3696
G80
G00 Z1.
M01
T3 M06 (#30 DRILL FOR 4 X .7MM TAP)
G90 G80 G40 G54
S2972 M03
G43 H3
/M08
G00 X0. Y0. Z1.
Z1.
G99 G83 R0.05 Z-0.5 Q0.05 F3.5664
G80
G00 Z1.
M01
M30
G91 Z0
%

[Geof]

Originally Posted by RBrandes I have to peck drill .128" for about 1/2" at the bottom of a 1/2" deep .136" hole. This is for a 1/8" rollpin. The larger hole provides a guide and makes it easier to assemble the pin and part. With Haas' peck drill (G83?) and single step, you can't single step! It runs through the entire routine and I can't see the Z values. What I am trying to do is to rapid down to the bottom of the clearance hole and then start peck drilling, yet retract to clear chips to Z+.01. What it seems to do is feed for the first 1/2" cutting air. This is a four-up table load and I am trying to reduce the run time.

There is a setting #22 CAN CYCLE DELTA Z which works with G73 and I think you can set it at something like +0.6 so you use R-0.45 for the smaller drill but the peck retract comes above the surface of the material.

I suggest drilling air first with your rapids down at 5% to see if it is doing what you want.

[Haas Apps 1]

RBrandes,
Here is what you need to do. Read the operators manual regarding setting 52 (G83 RETRACT ABOVE R). This setting will force the Z-axis to move above the R-plane on each peck retraction by the amount you specify. In your case, set setting 52 to .500. Program your start point to Z.01 and your R-plane to -.49 and your final Z-depth to Z-1.0. This will bring your drill to Z.01, then rapid to Z-.49 (R-PLANE) and begin peck drilling to a depth of minus one inch. On each retract move, your drill will move up to Z.01 (.500 above the R-value of -.49) Here is a SAMPLE program. Feel free to contact Haas Automation Inc. directly for applications help in the future. Go to www.haascnc.com. Select USA/International. Click on Solutions/Applications then click on The Question Man. Fill out the form, include your question or problem, and you will receive an e-mail reply within 36 hours, maximum.

%
O00001
T1 M6
G0 G90 G54 X0. Y0. M3 S3000
G43 H1 Z.01 M8
G99 G83 Z-1.0 R-.49 Q.075 F5.
G80 M9
G53 Z0.
G53 Y0.
M30

Regards,
Haas Apps 1

[Jedi]

Hi there apps I have a question. Why do you use the g53 y0.0 instead of a g54 y0.0? Does it matter ?

[Geof]

Originally Posted by Jedi Hi there apps I have a question. Why do you use the g53 y0.0 instead of a g54 y0.0? Does it matter ?

I am not Haas apps but have the answer; G54 is your work coordinate system, G53 is the machine coordinate system. G53 Z0. takes the spindle to Z home, the tool change position; G53 Y0. takes the table home on the Y axis

[Wiseco]

I just had to drill a 1/4" hole 17 1/8" deep in aluminium this morning. As the first hole my drill was too short, I had to do a second setup which is to start the drilling 15" deep in the stock to 17 1/8" deep. On my TL-2, I just put 15" in setting 52 and in the g83, I put r-15. and the job is done!

The easy way is to set the job from the conversationnal mode, start it but just to have the code in mdi and stopped it imidiately after this. With the code, you just have to modified some minor value and your ready to go.

[Haas Apps 1]

Originally Posted by Jedi Hi there apps I have a question. Why do you use the g53 y0.0 instead of a g54 y0.0? Does it matter ?

Jedi,
Geof is correct. G53 puts the machine in "Machine Coordinate" system for the block in which it is programmed. It is not necessary to command G54, for example, after using G53. G53 Z0 sends the machine to Z-zero in the Machine Coordinate system, which is Z-axis all the way up. G53 Y0 will bring the table all the way forward.

Haas Apps 1

[Scott_bob]

This is a good thread on the subject of understanding Drill cycles.
Let me ask you this: "What would the consequences be to not use G98 in your programs"?

Also, Does Haas have a default setting for rapid retract after drill cycles?

Sincerely,

[Haas Apps 1]

Scott_bob,
G98, Canned Cycle Initial Point Return, is the default G-code for canned cycles in the Haas control. If you always want to use G98, you don't have to command it. If you have changed to G99, Canned Cycle R-plane Return, and want to go back to G98, you must command it.
I am not sure what you mean by "does Haas have a default setting for rapid retract after drill cycles". I take that to mean returning to Z-zero after all holes have been drilled. If that is the case, all you need is a G80 to cancel the drill cycle and then command the next tool. The M06 call for tool change will automatically turn off the coolant, stop the spindle, and rapid to the tool change position.
If you mean the rapid retract after a hole has been drilled and before the next hole is drilled, G98 is the default.

I hope this helps.
Haas Apps 1