G81 Drilling cycle - can dwell at bottom of hole be changed?

[ArtEngineer]

Hi Friends,
We're using a G81 drilling cycle on plastic parts but we're finding the dwell at the bottom of the hole is too long and starts melting the plastic. We would like to remove the slight dwell time at the bottom of the hole which seems to be built into the canned G81 cycle.

Does anyone know if a parameter of the G81 cycle can be changed to remove the dwell? Will I need to create my own canned cycle to accomplish this?

Thank you for your help.
-ArtEngineer

Similar Threads:

• SIEMENS 828D CYCLE83 DEEP HOLE PECK DRILLING CYCLE
• SC10 tap bottom dwell time
• Combining peck drilling cycle with deep hole peck
• Hole Machining - Deep Drilling Cycle in Sprutcam
• how to dwell during a peck drilling cycle? HELP!!

[deadlykitten]

hi / try to replace " G01 Z-10 & dwell & rapid out " with " G01 Z-10 & G01 Z-10+0.07 & rapid out "

it delivers a smooth disengagement between the cutting edge and the material, and it may deliver a nice hole bottom, without using the dwell code


at higher feeds ( like when machining plastics ) it may be possible to use only " G01 Z-10 & rapid out ", thus no dwell at all : this trick may work when the deceleration/acceleration is agresive ( and specs are high and tool dia is little ), especially if the spindle is heavy : there will be a time window, during which the spindle will be almost stationary, because inertia will change direction ... of course, you may break the tool, etc

stuff depends on real scenario

kindly

[mactec54]

Hi Friends,
We're using a G81 drilling cycle on plastic parts but we're finding the dwell at the bottom of the hole is too long and starts melting the plastic. We would like to remove the slight dwell time at the bottom of the hole which seems to be built into the canned G81 cycle.

Does anyone know if a parameter of the G81 cycle can be changed to remove the dwell? Will I need to create my own canned cycle to accomplish this?

Thank you for your help.
-ArtEngineer

There should be no dwell at the end, post a snip of the code, a G81 should is a feed in, once it reaches the Z depth it should Rapid out

G81 does not have any dwell built in

[angelw]

Hi Friends,
We're using a G81 drilling cycle on plastic parts but we're finding the dwell at the bottom of the hole is too long and starts melting the plastic. We would like to remove the slight dwell time at the bottom of the hole which seems to be built into the canned G81 cycle.

Does anyone know if a parameter of the G81 cycle can be changed to remove the dwell? Will I need to create my own canned cycle to accomplish this?

Thank you for your help.
-ArtEngineer

Hello ArtEngineer,
As well as posting a snippet of your code, identify for the Forum the make of the control. By convention, G81, as mentioned by mactec54, G81 has no dwell at the bottom of the hole; that is in the realm of G82.

If you have a pattern of holes to drill, I wouldn't call Deadly Kitten's suggestion a solution, but more a fudge; it will force long hand coding of the whole operation and therefore losing the convenience of the Drill Cycle; somewhat like having a dog and barking yourself.

Regards,

Bill

[deadlykitten]

If you have a pattern of holes to drill, I wouldn't call Deadly Kitten's suggestion a solution, but more a fudge; it will force long hand coding of the whole operation and therefore losing the convenience of the Drill Cycle

it is possible to create a parametric code ( pattern included ) that will perform better, be more versatile, etc: especially for such a common operation like drilling

i have such a thing for okuma mills

i can improve it even futher, making it so easy to be used, that you may put a dog as an operator yeah, it will have bones & handles

[sinha_nsit]

Is it Fanuc?
Fanuc G81 has no dwell, nor can it be specified.
G82 is similar to G81 plus a user-specified dwell (P word) at the bottom. You may try G82 with small P, say P500, meaning 0.5 s dwell.

[angelw]

it is possible to create a parametric code ( pattern included ) that will perform better, be more versatile, etc: especially for such a common operation like drilling

i have such a thing for okuma mills

i can improve it even futher, making it so easy to be used, that you may put a dog as an operator yeah, it will have bones & handles

This is not my first rodeo and I find it difficult to imagine that a G81 drilling cycle, the most basic of the canned drilling cycles, needs to be made any more versatile. The cycle is to rapid to a Retract Plane, Drill to a Depth without peck and Rapid return to a Retract, or Initial level. All the parameters to perform these functions are contained in the existing G81 cycle; accordingly, I see no useful purpose in reinventing that particular wheel.

However, your suggestion in your initial Post had nothing to do with recreating the cycle with a Macro Program, nor answering the OP's specific question, just long hand coding for what can be achieved with a one block G81 command.

[deadlykitten]

i find it difficult to imagine that a G81 drilling cycle, the most basic of the canned drilling cycles, needs to be made any more versatile : i don't, and i also can improve it

just long hand coding : there are other methods, like custom conversational software, faster than editing a G-code; few keystrokes, and you are done; you interface the controller with 3rd party software

https://www.youtube.com/watch?v=8y5MjguI-pM

[angelw]

: i don't, and i also can improve it

coulda woulda shoulda; still nothing beneficial for the OP

[deadlykitten]

is good to know that there are alternatives, beside editing controller parameters

[mactec54]

is good to know that there are alternatives, beside editing controller parameters

No control parameters to change, just simple normal coding

[angelw]

is good to know that there are alternatives, beside editing controller parameters

With the G81 cycle there are only three components that can be changed, Drill Depth, Retract Plane and Feed Rate. I can see how good it would be to know that, rather than quickly edit any one, or all of these at the control, you could, say, use a Third Party software application to repost the program and then download it to the control; NOT.

As succinctly pointed out by mactec54, just simple, normal coding.

[deadlykitten]

changings through software can be faster than editing a code

some cnc brands may develop their own pallete of applications, and this allready happened

" offical "applications are " general "; if someone wishes for a " particular " behaviour, than he must know where to look

if the controller does not has an intrinsec capability, than there will be costs with its implementation ( if you know what you are doing, than it may worth a try and the results should be at least as expected )

main problem is that improving an action with +10% requires much more time than making it deliver the initial 90%; real goal is to have the tools to deliver fast those 90%

i have " particular " applications for the okuma controller; for the future, i wish to deliver same thing on machines from other cnc brands; onestly, at this moment, i don't exactly how to do it ...

kindly

[harshal]

G82 X_ Y_ Z_ R_ P_ F_ K_;
Where , XY- Position of hole
Z- Depth of operation performe
R- R plane position
P- Dwell time when tool reach at bottom
F- cutting feed rate
K- no of times operation repeats.
Operation :- First tool positioning at XY axis , after the tool rapidly traverse up to R-plane level , after that tool is start drilling operation . When the bottom of the tool has been reached, a dwell is performed. Then tool is retracted rapidly.



O5124
N10 M06 T04 ;
N20 G90 G80 G17 G00 G54 X0 Y0 ;
N30 G43 Z100 H4 ;
N40 M03 S1500 ;
N50 M07 ;
N60 G99 G82 X20 Y20 Z-10 R5 P1000 F120 ;
N70 X50 Y20 ;
N80 G98 G80 G00 Z100 ;
N90 M05 M09 M30 ;
More examples..........!!!!
DESCRIPTION OF PROGRAM


N10- Tool change command , select tool no. 4
N20- Absolute co-ordinate command , cancel canned cycle command , selection of XY plane, rapid command, work coordinate for tool positioning at X0 and Y0.
N30- Tool height offset compensation command , where tool is 100 along Z axis , tool hight code H4.
N40- Spindle on clockwise , speed is 1500 rpm .
N50- Coolant ON .
N60- Return to R-plane in canned cycle , counter drilling command ,first drilling position is X20 and Y20 Depth of drilling is 10 , R- plane distance is 5 ,dwell time is 1 sec , feed rate is 120.
N70- Second drill position where X 50 and Y20 and drilling depth is 10.
N80-Tool return initial position , cancel canned cycle , rapid command , where tool along Z axis is 100 .
N90-Spindle off , coolant off, Main program end .

DETAILS WITH DIAGRAM MY LINK IS - http://www.hdknowledge.com/2018/08/h...ing-cycle.html

[harshal]

Fanuc G81 cycle is used for normal drilling . Cutting feed is performed to the bottom of hole , then tool is retracted from the bottom of the hole in rapid traverse. When a tool length compensation (G43, G44, or G49) is specified in the canned cycle for drilling, the
offset is applied after the time of positioning to point R.



G76 X_ Y_ Z_ R_ F_ K_ ;
Where , XY- Position of hole
Z- Depth of operation performe
R- R plane position.
F- cutting feed rate
K- no of times operation repeats.



O5124
N10 M06 T06 ;
N20 G90 G80 G17 G00 G54 X0 Y0 ;
N30 G43 Z100 H4 ;
N40 M03 S1500 ;
N50 M07 ;
N60 G99 G81 X20 Y20 Z-45 R5 F120 ; [A]
N70 X80 Y20 Z-45 ; [B]
N80 X20 Y50 Z-45 ; [C]
N90 X80 Y50 Z-45 ; [D]
N100 G98 G80 G00 Z100 ;
N110 M05 M09 M30 ;
FOR DETAILS MY LINK IS- http://www.hdknowledge.com/2018/08/h...vmc-cycle.html