Other Drilling Cycles
When we drill continous, the drill bit is retrieved suddenly, leaving a step at the bottom. If we need a soft even finish, we must stop the feed and cut at least one turn on the same Z depth. Here Dwell is useful, and Cycle G82 is specifically designed for that. Let`s see.
G99 G82 X5.66 Y9.178 R0.3 Z-0.75 P100 F7.6;
On this program line, we will start drilling an X and Y from a height of 0.3 above, and will return to that position because of the G99 after we complete the drill. The depth of the hole is 0.75 and the Drill will remain spinning at the bottom for 100 milliseconds because of the P, if it where an X as in a previous example in which we left the coolant over the part for 10 seconds we would have left the drill spinning at the bottom for 10 seconds. P is for miliseconds, X is for seconds, we do not use X or seconds when drilling or we would burn or dull the drill. We must calculate one or two turns at the most to leave a good finish without dulling our drill bit on each hole. Here is how we calculate the precise time according to the rpms at which we are spinning.
Minimum dwell = 120/RPMs
So for our previous example, at which we where spinning a 3/16 drill bit at 1280rpms, a proper dwell time is 120/1280 =0.094 seconds, that is fairly 0.1 or a tenth of a second...P100
There is a rule for Drilling most materials, that is, A drill bit can go in a single strike 3.5 its diameter before getting clogged, after that the risk of breaking the Bit and loosing precious time removing the broken bit is big. We must then retrieve the Drill bit to evacuate the Swarf and chips or well inject high pressure coolant through the spindle and Drill bit that would push up the swarf...How many have a high pressure coolant unit in his shop?. Then we must retrieve the bit every 3 diameters. For very deep holes as we approach the bottom we might need to do it more often. Well, The CNC can do that for you when drilling among other nice features. Let`s see some more cycles.
G83 Is a cycle that includes all previous functions and features but adds the feature of retrieving the drill bit every distance we program. It is called Peck Drilling. This is how is written
G99 G83 X5.66 Y9.178 R0.3 Z-0.75 Q0.56 F7.6;
We removed the Dwell and added a Q function that is simply calculated by multiplying the Drill bit diameter by 3. The CNC will then drill for 0.56 straight, then return to R or 0.3 above the part, to clean the swarf, then return IN RAPID to the depht left less a clearance usually programmed by default at the parameters list. Then start drilling again at the feed ordered until he reaches the next Q depth or finished to the depth requested.
This is tremendously useful when drilling deep holes or on sticky materials. Be generous in short strokes and avoid:nono: going deep in a single stroke. Get the feel by watching how much of the flutes get filled, never let it stick to the drill. Plenty of oil or coolant.
Once you get the feeling and start using short strokes, you will start to feel discomfort that the Drill retracts to R every time and wish it could only retract enough to move the swarf up enough to clear for the next swarf to fit and then continue the Drill...Well, is your lucky day as Code G73 gives you that wished feature. It is called high speed drill because it retracts only Q and not all the way to R. Let`s see how is written
G99 G73 X5.66 Y9.178 R0.3 Z-0.75 Q0.56 F7.6;
As told, Drill retracts only to the last Q and only in the last peck, to R. So it sorts of Pumps up the swarf in Q increments, Drilling faster. A precious tool when making thousands of holes on Grills or Filter screens.
hew:
When we drill continous, the drill bit is retrieved suddenly, leaving a step at the bottom. If we need a soft even finish, we must stop the feed and cut at least one turn on the same Z depth. Here Dwell is useful, and Cycle G82 is specifically designed for that. Let`s see.
G99 G82 X5.66 Y9.178 R0.3 Z-0.75 P100 F7.6;
On this program line, we will start drilling an X and Y from a height of 0.3 above, and will return to that position because of the G99 after we complete the drill. The depth of the hole is 0.75 and the Drill will remain spinning at the bottom for 100 milliseconds because of the P, if it where an X as in a previous example in which we left the coolant over the part for 10 seconds we would have left the drill spinning at the bottom for 10 seconds. P is for miliseconds, X is for seconds, we do not use X or seconds when drilling or we would burn or dull the drill. We must calculate one or two turns at the most to leave a good finish without dulling our drill bit on each hole. Here is how we calculate the precise time according to the rpms at which we are spinning.
Minimum dwell = 120/RPMs
So for our previous example, at which we where spinning a 3/16 drill bit at 1280rpms, a proper dwell time is 120/1280 =0.094 seconds, that is fairly 0.1 or a tenth of a second...P100
There is a rule for Drilling most materials, that is, A drill bit can go in a single strike 3.5 its diameter before getting clogged, after that the risk of breaking the Bit and loosing precious time removing the broken bit is big. We must then retrieve the Drill bit to evacuate the Swarf and chips or well inject high pressure coolant through the spindle and Drill bit that would push up the swarf...How many have a high pressure coolant unit in his shop?. Then we must retrieve the bit every 3 diameters. For very deep holes as we approach the bottom we might need to do it more often. Well, The CNC can do that for you when drilling among other nice features. Let`s see some more cycles.
G83 Is a cycle that includes all previous functions and features but adds the feature of retrieving the drill bit every distance we program. It is called Peck Drilling. This is how is written
G99 G83 X5.66 Y9.178 R0.3 Z-0.75 Q0.56 F7.6;
We removed the Dwell and added a Q function that is simply calculated by multiplying the Drill bit diameter by 3. The CNC will then drill for 0.56 straight, then return to R or 0.3 above the part, to clean the swarf, then return IN RAPID to the depht left less a clearance usually programmed by default at the parameters list. Then start drilling again at the feed ordered until he reaches the next Q depth or finished to the depth requested.
This is tremendously useful when drilling deep holes or on sticky materials. Be generous in short strokes and avoid:nono: going deep in a single stroke. Get the feel by watching how much of the flutes get filled, never let it stick to the drill. Plenty of oil or coolant.
Once you get the feeling and start using short strokes, you will start to feel discomfort that the Drill retracts to R every time and wish it could only retract enough to move the swarf up enough to clear for the next swarf to fit and then continue the Drill...Well, is your lucky day as Code G73 gives you that wished feature. It is called high speed drill because it retracts only Q and not all the way to R. Let`s see how is written
G99 G73 X5.66 Y9.178 R0.3 Z-0.75 Q0.56 F7.6;
As told, Drill retracts only to the last Q and only in the last peck, to R. So it sorts of Pumps up the swarf in Q increments, Drilling faster. A precious tool when making thousands of holes on Grills or Filter screens.
hew:
