Category : Fanuc Mill Fanuc Turn Haas Mill Haas Turn
O0001(G28 Example)
(PROGRAMMED BY ANDY MURRAY)
G21 G90 G40
T01 M06(20MM ENDMILL)
G90 G0 G54 X200. Y0 S1500 M3
G43 Z3. H1 M8
G81 G98 Z-5. R1. F100.
X100.
X50.
G0 X25. (No hole drilled here cycle would be cancelled)
G80 (This also cancels the cycle)
Category : Fanuc Mill Fanuc Turn Haas Mill Haas Turn Mazak Mill Mazak Turn
G28 is used to send a machine to Zero return for a tool change or at the end of a program.
G28 G91 Z0 (Z axis moves up to tool-change)
G28 G91 X0 Y0 Z0 (All three axis move to their respective zero return positions)
I know some of you don’t like three axis moves like the one above. If it don’t hit anything it’s just fine “Get Over It”
Below are the two ways of doing this.
G28 actually means return to the zero point via a reference point.
If you programmed
G28 G90 Z0 or you forgot the G91 this means return to zero point via a reference point. The reference point is Z0 so the spindle would rapid to Z0 (Bang) and then move up to reference return point.
That’s why if you have single block on you will notice this is two presses of the cycle start (two blocks).
Therefore if we use G28 G91 Z0 the first press will take it to the reference point which is incrementally zero form where you are (no move) the second press move to zero (no collision)
Some older machines won’t have this so try not to get over excited.
G53 uses your absolute machine position (Machine) this means all moves are from home position and are not affected by datums (G54 etc) or tool length offsets.
It is one of the very few non modal commands so you can’t write
G53 Z0
X0 Y0 (this will use works offset not G53)
You need to write
G53 Z0
G53 X0 Y0
G28 uses G91 incremental so you must remember to write G90 (absolute) for your next command. In fact many a collision is caused by misuse of G28.
G53 is best if you have it just remember it is non modal.
So you write it in each time you need it.
Note:
Some machines have return to tool change built into the tool change line.
T01 M6
On a Haas machine for example where the return command is built in you would not need to send the Z axis home.
I recommend that you always put one in.
G53 Z0
T01 M6
If you are in single block you can stop before the tool-change if you wish.
Also I know someone who got into the habit of doing this and crashed a Fanuc Controlled machine that needed the command. (If you read this you know who you are)
G53 has another really good use and that is if you want the machine table (on a vertical machining centre) to move to a standard position to do things like changing the parts. It will always put the table in the same place regardless of work offset.
Bare in mind that if you put a position in that is relative to your work offset and not use G53 then the next time you set the fixture up your machine may over-travel because the fixture is in a different place.
If you read this article you will see how it could be used to set a vice in a known position regardless of datum.
Remember G53 is a position from the machine zero, it does not take into account the tool length offset or the datum. The other important thing is that it is non modal. That means you will need it on every line that you wish to use it for.
This machine has the Tosnuc 888 control.
For this control use G73 instead of G53.
If you have any questions about G28 G53 Zero Return or you are affected or have been affected by any of the issues in this post please contact me 07834 858 407
Please contact me if you require:
Classroom programmer 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.
Category : Beginners Fanuc Mill Haas Mill Mazak Mill New Stuff
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.
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.
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 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.
If you prefer dogs read on.
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.
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:
Classroom programmer 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.
Category : Fanuc Mill Haas Mill Mazak Mill
Rigid Tapping G84 Canned Cycle.
Let’s face it tapping on a CNC Machine can be a “right pain in the arse” as we say in the Midlands. But help is at hand. All you need is a bit of knowledge and the right equipment and it’s a dream, an absolute pleasure.
You mean you didn’t know? Well the first step is admitting you didn’t know.
Rigid tapping means the tap can remain rigid throughout the tapping cycle. It can be held in a chuck just like an endmill or a drill. The machine spindle locks in with the feedrate just like when you are screw cutting. You can buy tapping heads specially for this. They are no different to holding in a chuck but you get to use collets for holding the tap. These make it easy to change and it can’t spin.
Oh and you don’t need to remeasure the tap if you replace it.
Well here are some of the advantages.
It’s an option. Sorry you might not have it.
Most modern machines do have Rigid Tapping as standard but the older the machine the less likely it is that you will have it.
Sorry but you need to look in those boring manuals.
T06 M06 (M10 x 1.5 Tap)
G90 G0 G54 X50. Y50. S300 M03
G95 (Feed per rev)
G43 Z3. H06 M08
G84 G98 Z-15. R1. F1.5
X75.
X100.
G80
On some Fanuc controls you will need M29 for rigid tapping.
T06 M06 (M10 x 1.5 Tap)
G90 G0 G54 X50. Y50. S300 M03 (S300 M03 Optional)
G43 Z3. H06 M08
G95 (Feed per rev)
M29 S300
G84 G98 Z-15. R1. F1.5
X75.
X100.
G80
G94 (Feed per minute)
In the above cycle the tap will rapid down first to Z3. as in the G43 line. On beginning the cycle it will then rapid to what is know as the R Point. In this case R1. (one mm above the hole).
It will tap to a depth of 15 (Z-15). Depending on whether you programme G98 or G99 it will return to either the Z3. or the R1. before moving to the next position.
If you want to know more about G98 and G99 then read the article above.
G94 feed per minute (feed is in mm per minute).
G95 feed per rev (feed this amount every revolution)
These two G codes are your friend when you’re tapping or should I say G95 feed per rev is your friend.
Why?
When Rigid Tapping G84 Canned Cycle on a Fanuc, Haas, Mazak or similar control it is best to use G95. This means that when you programme your G84 (Tapping Cycle) your feedrate is your pitch.
The really great thing here is that if you change the speed of the tap you don’t change the feed because it’s the pitch.
Bet you have made that mistake before???
You change the speed and forgot to change the feed. We all know what happened next.
How easy is that?
Oh and don’t forget to change back to G94 at the end of the tapping.
You will notice the Heidenhain does this automatically for you.
This machine has the Tosnuc 888 control.
T06 M06 (M10 x 1.5 Tap)
G90 G0 G54 X50. Y50.
G43 Z3. H06 M08
G95 (Feed per rev)
M05
S300
M843 (Synchronous Rotation command)
G84 G98 Z-15. R1. F1.5
X75.
X100.
G80
M845 (Cancel Synchronous Rotation command)
Notice how it pulls out when the tap stops and reverses.
So the problem is that when the spindle stops, reverses and starts up everything goes wrong.
But this tension and compression tapping head can take up all the slack.
Definitely not, depths will vary. You will probably need to do some hand tapping too.
These are special collets designed to slip at a certain torque. This allows you to get to depth without breaking the tap.
You adjust the collar at the front to give the required torque.
You can’t use these on Rigid Tapping G84 Canned Cycle because the last thing you want is for the tap to stop rotating.
Rigid Tapping G84 Canned Cycle, check out this great video on how to stop the machine half way through tapping.
Fanuc (if you have the option) is G84.2 just programme your normal tapping cycle but replace G84 with G84.2 and add a Q value which is your pecking depth.
G84.2 G98 Z-15. Q5. R1. F1.5
If you programme this.
G84 G98 Z-5. R1. F1.5
Z-10.
Z-15.
Z-20.
G80
There you have it Peck Tapping.
So you move to a position and it taps a hole 5mm deep. Because you are in a canned cycle it will repeat the procedure at Z-10. Z-15. and Z-20.
How cool is that?
Don’t forget there’s loads more folks.
Edgecam programming and training.
Classroom programmer training.
CNC Programming and 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
Category : Fanuc Mill Haas Mill Mazak Mill New Stuff
CNC Milling G02 G03
To produce a full circle on a Fanuc or Haas G code type programming system is really easy.
Last week I was training four very experienced programmers and I asked them how they would programme a full circle.
The answers they gave shocked me, I had to take out my hip flask and drink a large shot of brandy.
What they were doing was perfectly correct but definitely not the simplest way.
One said he broke the circle into two halves. One said he copied some code he already had in the machine. The other one said he got the bloke who did it in two halves to do it for him. Oh and the other one used I and J and X and Y.
OK so just imagine you want to mill internally around a 40mm diameter circle.
G0 X0 Y0 S1500 M3
G43 Z3. H01 M8
G1 Z-5. F100.
G41 X20. Y0 D1 F200. (Apply Cutter Compensation)
G3 X-20. R20. (First Half)
X20. (Second Half)
G1 G40 X0 Y0 (Cancel Cutter Compensation)
G0 G53 Z0
G1 G41 X20. Y0 D1 F200.
G3 X20. Y0 I-20. J0 (Mill Full Circle)
G1 G40 X0 Y0
G1 G41 X20. Y0 D1 F200.
G3 I-20. (Mill Full Circle….. Sooo Simple)
G1 G40 X0 Y0
Remember that song by the Average white Band “Let’s Go round Again”? I used to love it.
Actually I still do, as an old twat I’m allowed to like this shit.
G1 G41 X20. Y0 D1 F200.
G3 I-20. (Mill Full Circle)
I-20. (Lets go round again)
G1 G40 X0 Y0
CNC Milling G02 G03 to produce a full circle you just need this:
G13 D1 I20. F200. (Everything all in one)
G13 (Counter Clockwise) G12 (Clockwise)
D1 (Use offset 1)
I20. (20mm Radius)
G13 does everything. It’s the an all inclusive holiday of circular milling except you don’t gain weight and you’re not pissed everyday.
How cool is that and you even get a tangential approach. At my age you’re glad of all the tangential approaches you can get.
No there is no sexual innuendo here it just means you approach the circle using a circular move. You sort of creep up when it’s not looking.
Know what I mean??
Here is a nice picture to demonstrate.
Think about it, why would we do this?
Well the older and more inaccurate your CNC machine is the more likely it is that your machine will leave a mark at the entry and exit point. This is also dependant on the material and the size of the cut you are using.
A quick workaround for this is to just go round the circle twice (let’s go round again). It very often does the trick.
Oh by the way if I saw a tangential move that big I would think it was a wasted move. (It’s just to demonstrate). You only need a short tangential move to do the job.
The easiest way to programme a tangential approach is like the ones above. Coming in from North, South, East or West on the compass.
Now look at this.
This is the best way, although it’s more difficult to programme.
I think it’s South West on a Compass?? 
The reason is that there is no axis change of direction and no animals are injured or hurt in any way during the process.
If you watch the movement above and watch carefully what the X axis is doing. It changes direction before it is in contact with the circle. And the same thing on the way out of cut with the Y axis.
When milling a full circle each time an axis changes direction there is a chance you will be left with a visible mark on the circle. These points are North South West and East on a compass.
Watch below to see where these points are. If you have a new machine there should be no visible mark on this change of direction.
On an old machine this can be really noticeable and cause real problem.
If you have an old machine you will know what I mean. Those little annoying marks where the machine changes direction. If CNC Machines were underpants then these would be the skid marks.
For my American readers in the UK we call those annoying brown marks at the back of your underwear skid marks. I don’t think you get them in America.
I have been working on a 12 year old Mazak Horizontal machine recently and was amazed at just how good a circle it produced. It beats the shit out of using a reamer. Oh and you can easily adjust the size with your D offset.
Just a note. If you do use circular milling to produce a bore just remember that if your cutter is not parallel then your bore won’t be either. So don’t use that crappy old re-ground cutter. Try n get the boss to buy you a shiny new one.
oh and just one other thing………..
Measure the bore at the top and the bottom.
G1 G41 X20. Y0 D1 F200.
G3 I-20.
G1 G40 X0 Y0
There are actually four choices which produce four totally different circles.
And potentially a scrap part. So use those machine graphics to check your code if you got em!!
G3 I-20. (The one on the left and the one we used)
G3 I20. (The one on the right)
G3 J20. (The top one)
G3 J-20. (The bottom one)
CNC Milling G02 G03
If you want to do this on a Sinumeric Siemens 840D read this
Don’t forget there’s loads more folks.
Edgecam programming and training.
Classroom programmer training.
CNC Programming and 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.
