Learn CNC Programming (Canned Cycles)
A Canned Cycle What is It?
If you want to learn CNC programming then you need to know what a canned cycle is.
I’m going to have to be honest here it is a funny choice of words “Canned Cycle”. But a wild guess would be that all the information to drill a hole would be kept together in a “Can” ready to use.
In a Can…….
So let’s learn CNC Programming….
Make sure you read the end of this article to see a really cool way to drill equally spaced holes.
First of all we state the cycle:
G81 Z-20. R1. F100. X50. Y50. F200.
The machine will move to X50. Y50. then rapid to 1mm above the part (this is the R1.). It will then feed down to Z-20. at a feedrate of 200 mm per minute F200.
Finally it will rapid out of the hole.
It then sits ready for the next move.
All you need to do now is just keep giving positions.
G81 Z-20. R1. F100. X50. Y50. F200.
X60.
X70.
X80.
X90. Y60.
G80
The G80 at the end will cancel the canned cycle. It just means “Look I am a bit pissed off with drilling holes so can you stop”
So that’s it Canned Cycles it really is that easy you put all the information in the “Can” then each time you give a position you get another hole.
Want to know More?
Thought you would. You want to learn CNC programming don’t you?
There are loads of these canned cycle but I am not going to talk about every one in detail. No sorry you will have to read the boring old manual for that.
Not to Worry They Are All The Same
Well sort of. You state the cycle then it repeats at each position given until you cancel it (and that applies to all the cycles).
Anyway Here are a few:
G84 taps holes, tell it the pitch depth usual stuff.
G73 peck drilling is the same as drilling (G81) but you give it the peck depth.It pecks the hole breaking up the swarf.
G83 same as G73 but with each peck the drill comes right out of the hole. For deep holes or swarf that clogs.
G76 bores a hole, stops at the bottom, moves over and rapids out to avoid marking the bore.
Ok let me tell you this, you are doing great so far. This is how we learn CNC programming. Nice small steps.
I already wrote a post on this click to see it all (it’s truly amazing). I purposely didn’t include it in the cycle above which is ok. The idea was to keep it simple.
G43 Z50.H1 M8
G81 G98 Z-20. R1. F100. X50. Y50. F200.
X60.
X70. G99
X80.
X85. G98
X90. Y60.
G80
All it is in a nutshell. G98 returns to the Z point you were at before you started the canned cycle.
G99 will return to the R point (R1.)
Why you ask?
Easy you can jump over shit.
Clamps, high sections on a part, tall buildings, anything.
It Gets Better.
G81 Z-20. R1. F100. X50. Y50. F200.
The Z-20. the R1. the feed-rate etc are all known as parameters. These are the things that control your cycle.
These can be altered at anytime and stay in until you alter them again or cancel the cycle.
G81 Z-20. R1. F100. X50. Y50. F200.
X60.
X70. Z-30. (From here onwards the holes are drilled 30mm deep not 20)
X80.
X90. Y60.
G80
Now let’s alter the feed
G81 Z-20. R1. F100. X50. Y50. F200.
X60. F300. (Change feed)
X70.
X80.F200.(Change it back)
X90. Y60.
G80
Remember it stays in until you say otherwise.
Read the above article. Modal means that the information stays in the control until you cancel it or change it.
Do’s And Don’ts
Do Not………
Put in a rapid command G0 X50. Y50. it will cancel your cycle and the machine will just sit laughing at you. (No hole drilled).
See this post G0 cancels canned cycle.
G81 Z-20. R1. F100. X50. Y50. F200.
X60.
G0 X70. (Rapid to X70. no hole drilled)
X80. (Rapid to X80. no hole drilled)
X90. Y60. (ETC)
G80 (You already cancelled the cycle with G0)
Do Not Repeat Axis Moves.
G81 Z-20. R1. F100. X50. Y50. F200.
X60. Y50. (Don’t need Y50.)
X70.
X80.
X90. Y60.
G80
D0…….
- Always use a canned cycle if possible it saves loads of time. It is also really easy if you need to edit anything.
- Make your CAD/CAM system output canned cycles, not long hand code. I saves loads of time if you need to edit.
- Love engineering and be nice to your cat.
Really cool way to drill equally spaced holes
Imagine you need to drill and tap this part. Nine M10 holes.
Quite simple but 31.63 added up nine times? Mmmm I never learnt my 31.63 times table.
O0001(Drill and Tap M10)
T01 M06 (20mm Spot Drill)
G90 G0 G54 X0 Y0 S1500 M3
G43 Z3. H1 M8
G81 G98 Z-10. R1. F100 L0
G91 X-31.63 L9
G80
G0 G53 Z0
ETC
M30
Learn CNC Programming? How easy is that?
- The programme moves to the datum X0 Y0 which is the middle of the part at the right hand end.
- The G81 has an L0 at the end. L0 is not a Lionel Richie song it just means don’t do one. So it moves to X0 Y0 and does nothing.
- The next line, G91 means incremental move so it moves incrementally nine times (L9) X-31.63 and drills a hole each time.
Brilliant I told you it was worth waiting for.
Thanks For Reading
Don’t forget there’s loads more folks.
And a YouTube channel
Call David: 07834 858 407
Learn CNC Programming
Services offered at CNC Training Centre
Edgecam training.
Classroom programmer training.
Onsite CNC Machine Training.
CNC Training on all controls and machines.
Mazak Training Fanuc Training
Don’t forget we offer training on all types of Mazak Machines and all Fanuc Controls 6m to 31i Oi old to young.
