G71 is sometimes known as a canned cycle when in fact it is a multi repetitive cycle. The G70 cycle goes with it and can pick up the same lines to finish.
The N numbers are important as the cycle uses these as the points of reference to jump to.
G71 cycle interprets the shape between these two N numbers and then breaks up the shape for roughing.
Basic Turning, in the early days of CNC Turning G96 was one of the things that really made a massive difference.
It meant that instead of having to turn a part at a fixed speed and feed, the part could be programmed in G96 which was a constant surface speed.
Where diameters changed, particularly when facing, it made a massive improvement to tool life and surface finish as well as speeding up the whole process.
G97 Speed In RPM
In Basic Turning when you program G97 your machine will start the chuck up at a speed in RPM. So if you program. G97 S1500 M3
Your chuck will start revolving clockwise at 1500 rpm.
G97 for Drilling Tapping and Screwcutting
When drilling a hole you are on the centreline of the machine so you just want plain old simple RPM.
G96 however means meters per minute. This is a surface speed. G96 S200 M3
Your machine would start up at a surface speed of 200 meters a minute. Now your RPM would depend on where on the diameter the tool was positioned.
If the tool was positioned at a 100mm diameter it would be as if the tool were able to run around this diameter at a speed 200 meters a minute.
It’s a bit like being on a running machine if you ran at 200 meters a minute and placed various diameters under your feet the large ones would turn at slow rpm and the small ones would turn at high rpm. (Just like the hamsters above)
That’s why on a manual lathe it is hard to face a large diameter without changing speed half way.
Neeeeeoooooooowwww
You know when you face a part on a CNC Lathe and you hear that change in pitch? It’s the spindle increasing in RPM as it gets closer to the center of the part.
Well I bought my hamster loads of different wheels to play on just like the one above.
My hamster suffered with depression on account of being stuck in a cage all day and not having a girlfriend oh and he had a lot of credit card debts too.
These wheels varied in diameter from about 6 inches to a massive 2 foot one. They kept him happy all night. He was so tired he slept all day.
Harold could only run so fast but I noticed when he was on the small 6 inch wheel it absolutely whizzed around. Now on the big two foot diameter one it took him ages just to get it to spin around once.
G96 G97 all about hamsters
Harold Had G96
A CNC machine in G96 will give a lovely finish because the surface speed always remains the same.
So even though Harold ran at 200 metres a minute (this is fuckin lightening speed for a hamster)
The wheels ran at different RPM depending on what diameter they were.
Harold Was a Clever Bastard
Oh by the way Harold had a tail (unlike other hamsters) and a maths qualification.
He knew that if he multiplied the diameter of the wheel by .00312 it would give him the circumference of whatever wheel he was running on in meters.
200 mm wheel (.00312 x 200 = .6864)
All he now needed to do was divide this answer into the speed he was running at and he would know how many RPM his wheel was revolving at.
If he was running at 200 meters a minute not only would he be fuckin knackered but the wheel would be running at 291 rpm
200 / .6864 = 291
Basic Turning Manual Machining
Using a manual machine you have to compromise. At the outside your speed is too fast and when you get to the centre you are too slow.
Manual Lathe
On a CNC lathe we would normally program in mm per revolution as well because the speed is changing all the time so we need our feed to be locked into the speed.
With a machining centre our cutter is always revolving at the same speed so the feed can be constant in mm per minute.
Someone out there will be thinking “what happens in G96 when you get to the centre of the part”. Well the spindle will be flat out!
See how surface speeds are translated to speeds in RPM. There are many converters online that you can use for this and I do recommend their use. It will also mean you don’t have to watch my tedious video.
When I train people at the CNC Training Centre my emphasis is on understanding not memorising. I usually start by saying “please don’t remember all the things I am telling you”.
In the early days training students in Basic Turning I remember them saying to me the next day that they had G codes floating around in their head from the lessons the day before.
G96 and G97
What I really mean is that the most important thing is to understand what the machine can do and the concepts of programming and Basic Turning.
You could say “I know there is a G code that makes the machine run in RPM” so all you need is a list of G codes.
If you can be bothered to work through the simple maths above. It will help you to fully understand how G96 is works.
This is a video explaining cutter compensation in CNC programming.
You will come across various terms to describe this such as:
Tool cutter comp.
CNC cutter comp.
G41 G42 cutter compensation.
Cutter diameter compensation.
Cutter radius compensation.
Heidenhain RL RR.
Cutter compensation is referred to as cutter diameter compensation and cutter radius compensation
Haas cutter compensation, Fanuc cutter compensation and Mazak cutter compensation all work in the same way.
Although Heidenhain cutter compensation or Heidenhain cutter comp looks different. In the programme it functions in exactly the same way.
In the parameters or settings of your control you can set up your system to use the radius or the diameter of your cutting tool.
This means that when you input the data for your cutting tool in your offset table you can use the diameter or the radius of the tool. This depends on your settings.
When people talk about cutter compensation G code they may say “cutter comp G code” it’s often shortened.
(Cutter compensation G code)
The G codes used in this video are:
G41 cutter compensation left
G42 cutter compensation right
G40 G code to cancel cutter compensation
This Video shows you :
How to program G41.
How to program G42.
CNC cutter compensation examples.
Cutter compensation Heidenhain style.
Heidenhain RL RR.
We always recommend that you climb mill so you will be using G41 most of the time.
Milling the outside of a square using G41.
Milling the inside of a square using G41.
Milling the inside of a square using G42 (should you want to conventional mill).
Milling the outside of a square using G42 (should you want to conventional mill)
The rules when using compensation on a CNC Milling machine.
This is simple on a square sided figure or a simple radius. Anything more complex and it’s a nightmare.
I just heard some smart arse say “Ah well my CAD system takes care of that”.
So it should my friend but, and there is a but:
What will you do when your cutter wears?
What if you want to use a different size cutter?
The cutter may not run true.
What if the cutter is not exactly size?
In the old days of paper tape and Corned Beef we as programmers would write several programmes.
This was so that we could re-grind the milling cutters in fixed increments. A different programme could be used each time the tool was changed.
Sorry I can’t talk about this much longer as I still have the nightmares (mainly about corned beef sandwiches).
Anyway enough of that. So when we machine our first profile we can add some on to the tool radius in the offset file. When we check the part we can adjust the offset and re-cut the profile to achieve an accurate result.
The Rules:
Shape must be continuous and consistent.
You can’t cut along a line and then go back along it.
It’s important to allow more than the tool radius when entering tool compensation. The same applies when you come out of tool compensation.
Internal corner radii and steps must be greater than the tool radius.
Always allow more than the radius because when you adjust it it may be larger than the actual tool you are using.
Don’t ask
For example if you have a 12mm endmill but you have .2mm in the wear compensation. The machine thinks that the tool is 12.4mm in diameter.
You can’t do this in cutter comp:
You would have to apply one cut in G41 and cancel with G40 then do another cut in G42 and cancel with G40:
