Cutter Compensation

  • Home
  • TagG Code Video

Cutter Compensation

Tags :

Category : Fanuc Mill Haas Mill

Cutter compensation explained.

Call 07834 858 407

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.

Cutter Compensation

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.

Cutter Compensation

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.

Cutter Compensation

Milling the inside of a square using G41.

Cutter Compensation

Milling the inside of a square using G42 (should you want to conventional mill).

Cutter Compensation

Milling the outside of a square using G42 (should you want to conventional mill)

Cutter Compensation

 

The rules when using compensation on a CNC Milling machine.

Rules are the same as the tool nose radius compensation on a CNC Lathe.
If you programme a shape and you do not use cutter compensation you will have to work out the size of the shape with your tool radius added.

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).

Cutter Compensation

 

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:

Cutter Compensation

You would have to apply one cut in G41 and cancel with G40 then do another cut in G42 and cancel with G40:

Cutter Compensation

Call 07834 858 407

Please contact me if you require:

  • Fanuc training.
  • CNC programming training.
  • Want to Learn CNC programming.
  • Fanuc programming   training.
  • Yasnac programming training.
  • Any type of CNC course.

Don’t forget to watch my Tutorial Videos

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.

G96, G97 and How To Calculate Surface Speeds

Tags :

Category : Fanuc Turn Haas Turn Mazak Turn New Stuff

Basic Turning

Basic Turning
G96 Hamsters Large wheel Small wheel
Call us for CNC Training and hamsters

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.

When tapping or spot drilling it’s the same.

Screw Threading (G76) can only be done in G97

G96

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.

Basic Turning

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)

Basic Turning

 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.

When it gets to the center your spindle is flat out so the G50 becomes crucial.

The G50 restricts the speed of the machine.

G50 S2000 machine will go no higher than 2000 rpm.

 

G96 G97 hamster on a Wheel

Did you have a pet hamster as a child?

I know it’s a random question but bear with me there is a point to this.

Well maybe you still have a Hamster and that’s not a problem. Time you fuckin grew up but it’s not for me to judge.

Anyway I did and his name was Harold Wilson (British Prime Minister at the time).

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.

Basic Turning
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!

Could be a problem. That’s where your G50 comes in to restrict the speed. Very important! CNC Basics G50

cnc turning basics
G50 Warning

Watch the video

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.

Basic Turning
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.

Here is a list of Basic Turning G Codes.

The ones you use every day you will remember whether you want to or not.

G96 Whoopee It’s amazing

So use G96 for everything.

Except for:

  • Drilling.
  • Tapping
  • Threading (Screw cutting)
  • Cutting the Lawn

If you feel you have been affected by any of the issues mentioned in this post please Contact me

If you liked this video, please don’t forget to subscribe to my YouTube channel by going to: CNC Training Centre

Please contact me if you require:

  • CNC programming training.
  • Want to learn CNC programming.
  • Fanuc control training.
  • Yasnac programming training.
  • Any type of CNC course.
  • Fanuc training courses
  • CNC lathe training
  • CNC Vertical Machining Centre training

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.

G98 and G99 It’s About Jumping Things

Tags :

Category : Beginners Fanuc Mill Haas Mill Mazak Mill New Stuff

G98 and G99 It’s About Jumping Things

G98 and G99, a canned cycle is usually one line of code for example to drill a hole. This one line of code tells the machine all it needs to know about drilling my holes.

  •  Depth
  •  Feed-rate
  •  A point in the Z axis to rapid to before drilling
  •  Point to rapid back to after drilling
Sample program of G81 Drilling Cycle G98 and G99
G81 Drilling Cycle Sample Program G98 and G99

What happens then is each time you give the machine a new position it will drill one of these holes.

This is great because you don’t have to worry about what’s going to happen.

Each hole will be identical unless you change one of the parameters in the cycle like the Z depth or the feed-rate.

Therefore if on one hole you put a different Z depth that hole and all subsequent holes will be to the new depth.

Easy As ABC

So all in all it’s a really easy way to drill holes. You tell it what you want and then each time you give a position you get a hole. Then when you get sick of drilling holes you type in G80 and it stops drilling holes.

Machine says “OK this turkey doesn’t want anymore holes” so from now on when the machine moves to a position nothing happens.

Mitsubishi Drill In Action G98 and G99
Mitsubishi Drill In Action

Mitsubishi Carbide

There are loads of Canned Cycles I can’t be bothered to tell you about them all cos I’m going out tonight otherwise I would explain them all. If you scrat around this website for a while you’ll find them all.

Anyway they all do different shit.

They all work in the same way but with some variations.

Now the video at the bottom of the page is about G98 and G99.

G98 and G99 are in all of the drilling and tapping cycles. You have one or the other. You can even miss it out if you can’t be arsed with it.

OK so assuming I want it, what does it do?

You may well ask.

I know for a fact that some of you, and I won’t mention names, put this on the line with the canned cycle but you ain’t got a clue what it does. Maybe you don’t even put it in because you’re frightened of what it might do..

Now’s the time to learn or you will have it on your conscience for the rest of your life.

By the way if you don’t give a flying shit what it does then I wouldn’t waste anymore time reading this.

Here is a lovely video on kittens for you to watch. Off you go.

G98 and G99 How it works.

If you prefer  dogs read on.

  1. First of all the tool will rapid to what we call an initial point which the control remembers ready in case you decide to program G98. (This is the last Z move you made before the cycle is called).
  2. The tool will then rapid down close to the hole (this is called the R point). Don’t make this too far away or you will waste movement.
  3. Tool feeds down in Z to the Z depth at the feed-rate you specified.
  4. Then the tool will rapid back out of the hole. It can either rapid out to initial point (1) or the R point (2) depending on if you programmed G98 or G99.
Parts of the G81 drilling cycle with G98 and G99
How G81 works in action

Now if you program G99 it returns to the R point (2)
If you program G98 it returns to the initial point  (1)

OK why on earth would I want that? Maybe you wish you had chosen to watch the kittens video, but read on.

Well……. if you made that initial point 50mm above the job (about 2 inches) and the rapid point was 1mm above the job (.040 inches).

You could drill all your holes in G99 and the drill would each time return to 1mm (.040 inches) above the part.

If you add a clamp to jump over just put G98 on the hole before and it will jump to 50mm (2 inches) above the part. Oh and it misses the clamp.

Change back to G99 and it stays down returning to 1mm (0.040 inches) above the part.

Admit it, you like it don’t you?

Please don’t try this at home by the way.

Get it? So you eliminate wasted moves. Good init.

 

demonstration of G98 and G99 in action
G98 and G99 in Action

Oh and here is my video it explains how to use G98 and G99 to jump over clamps on a fixture.

The video is shit by the way but I had to learn (it’s been ages ago).

If you are completely crazy and you like this video, please don’t forget to subscribe to my YouTube channel by going to: CNC Training Centre

Please contact me if you require:

  • CNC programming training.
  • Want to learn CNC programming.
  • Fanuc control training.
  • Yasnac programming training.
  • Any type of CNC course.
  • Fanuc training courses
  • CNC lathe training
  • CNC Vertical Machining Centre training
  • Siemens Training
  • Hatha Yoga
  • Flower arranging

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.

G84 Rigid Tapping Program Example

Tags :

Category : Fanuc Mill Fanuc Turn

G84 Rigid Tapping Program Example

G84 is a tapping canned cycle.

G84 taps holes.

This simple part has four M12 holes, drilled, countersunk and tapped. The datum is the centre of the part so the holes positions are.

X55. Y55.
X-55. Y55.
X-55. Y-55.
X55. Y-55.

G84 Rigid Tapping Program Example

G84 Rigid Tapping Program Example

Here is the CNC code

G84 Rigid Tapping Program Example

The machine first moves to X-55. Y-55. and rapids the Z axis to 3mm above the part.

G84 Rigid Tapping Program Example

The G95 selects feed per revolution which means we only need to program the tap pitch for the feed-rate.

See full rigid tap G84 Rigid Tapping Program Example

The M29 engages the rigid tapping mode and the S800 is the speed. (It does not start the spindle)

It then rapids the Z axis down to 1mm above the part R1.

The G84 Cycle instructs it to tap a hole 17.mm deep (Z-17.) at a feed of 1.75mm per revolution (F1.75) 

So it feeds at 1.75mm per revolution with the spindle turning clockwise to depth.

At the bottom of the hole it reverses the spindle and feeds back to the initial point.

This initial point was in the line.

G84 Rigid Tapping Program Example

This is because of the G98.

If it were G99 it would return to 1mm above the job (R1.)

See explanation of G98 and G99

Once the cycle is active each time it sees a position it repeats the tapping process.

When the G80 is programmed it no longer taps holes.

Single block and feedhold do not work in a tapping cycle.

Why? You ask.

IT BUSTS THE TAP

Now watch the video to see it all in action (not breaking the tap).

Thanks

If you have been affected by any of the issues in this post or need CNC Counselling then contact me.

If you want to learn to program CNC Milling Machines

Look no further Contact CNC Training Centre

 

 

 

Polar Programming G16 Fanuc

Tags :

Category : Fanuc Mill

Polar Programming G16

Polar programming is cool.

No one loves polar bears more than me.

Polar means you are working around a pole. So your programmed position is determined by a radius and an angle.

No use??? Think about it. Polar Programming G16.

Holes on a pitch circle. Mill a hexagon. Piece of piss. Honestly.

Read on….

Polar bears, polar programming here we go. Don’t go too close to polar bears as they have a propensity to rip you head off.

Oh No Polar Programming G16 is an Option

Sorry yes it’s n option. Anyway hopefully you have it. Don’t blame me blame the tight arse who bought the machine.

Imagine you had some holes like this to machine.

Polar Programming G16First thing you need to do is program a G16 to say you want to use polar programming.

G16 on its own means your datum is the centre of the pole (X0 Y0)

G16 X50. Y50. would put your pole centre at X50. Y50.

Anyway we want it at zero which is the centre of this pattern of holes. So it’s just G16.

Once G16 is active then X becomes your radius and Y becomes your angle.

What’s The Time Mr Wolf?

The angle is always measured from 3.15 as below. (If you’re reading this mum sorry about busting your clock but I needed the picture)

And the angle is measured counterclockwise. This applies to all CAD CAM.

So this angle would be Y60. (60 degrees) and the X would be X25. (Radius)

Polar Programming G16

So you program looks like this

Polar Programming G16

Now see it running.

Lets look at the milling in more detail

Polar Programming G16

Note that the distance to the sharp corner is 46.188 The line N1 uses this.

Polar Programming G16

Polar Programming G16 It’s So Easy

Then we just program each position as an angle (no need for the radius because it does not change)

Polar Programming G16

Each point you are going to has a radius from centre and an angle.

Incremental What’s That All About?

Don’t forget this works in incremental as well so be careful (you’re not insured for this)

Incremental

It gets even better when you use the L command.

Polar Programming G16

Polar Programming G16 Action

Now when it comes to the milling it’s so simple don’t you just love this.

Polar Programming G16

Action

 

What do you think?

G16…..

Add it to your digital toolbox??

Thanks

If you have been affected by any of the issues in this post or need CNC Counselling then contact me.

If you want to learn to program CNC Milling Machines

Look no further Contact CNC Training Centre

Weekend and Online Courses

Onsite Training

Classroom Courses

Apply Now

Call David: 07834 858 407

Copyright © 2015 CNC Training Centre. All Rights Reserved. Website Originally Developed By Jabberdog

WP to LinkedIn Auto Publish Powered By : XYZScripts.com