Category Archives: Mazak Mill

G28 G53 Zero Return

Tags :

Category : Fanuc Mill Fanuc Turn Haas Mill Haas Turn Mazak Mill Mazak Turn

G28 G53 Zero Return

CNC Training (Call David: 07834 858 407)

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.

Ignore This If You Get Bored Easily

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.

G28 G53 Zero Return
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)

Using G53

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

Advantages Disadvantages (G28 G53 Zero Return)

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.

 

On Machines Like The BMC 800 from Toshiba

Tosnuc 888

This machine has the Tosnuc 888 control.

Tosnuc 888

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:

  • 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.

Jumping Sections of Programme Using M99 and Block Skip

Category : Fanuc Mill Fanuc Turn Haas Mill Haas Turn Mazak Mill Mazak Turn Useful Stuff

 

Click for M99

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

Contact: 07834 858 407

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.

Jump Around Using M99 Plus Block Skip

Category : Fanuc Mill Fanuc Turn Haas Mill Haas Turn Mazak Mill Mazak Turn

Using M99 Plus Block Skip

Call David 07834 858 407

M99 Plus Block Skip, M99 on a Fanuc, Haas or Mazatrol ISO control can be used to jump sections of code.

Learn to use this in conjunction with the block skip command to switch it off and on.

Now I know you are all thinking “Dave you’re wrong it’s the end of a sub-program”. (Please in the name of holy shit do not call me Dave.)

Well you are right and you are wrong.

Yes it means continue and is used at the end of a sub program.

But it also has another nifty use.

Imagine you want to skip a complete section of program in the case below it’s the Spot Drill.

Let’s See Some Crap Ways Of Doing This

(If you want to do this on a Toshiba Tosnuc 888 or similar control go to the end of the article)

In this example it’s a spot drill we want to miss out.

M99 Plus Block Skip
Standard Code

You could delete it and make two programmes (sounds like hard work and loads of errors). Not to metion wear on your finger tips. Truth is it’s just a shit way to do it.

M99 CNC Code
Block Skip

The programme above  contains BLOCK SKIPS sometimes called BLOCK DELETES.

When you switch on your BLOCK DELETE/BLOCK SKIP switch, each time a forward slash (/) is seen that block will not be processed and the control will move on to the next block.

M99 Plus Block Skip

On most Fanuc controls it’s B.D.T not to be confused with CBT (Cock and balls torture) please do not google this in company time.

It works ok but it is very time consuming. If you want to skip a big section of code you will have to write in loads of block skips.

Call me a lazy bastard but I definitely couldn’t be arsed with that.

Some controls even have two three and four block skips so you can switch on any combination of these switches, mmmm complicated. Good luck with that one.

Do You Have Adequate Life Insurance?

M99 CNC Code (Now let’s use it)

The next example is the easiest way.

You probably normally see an M99 at the end of a sub programme.

In the case below it tells the control to jump to N100 (M99 P100).

The P part is the N number you want to jump to.

M99 P600 (Jump to N600)
M99 P6666 (Jumps to N6666)

 

M99 Plus Block Skip
M99

If you put the BLOCK SKIP/BLOCK DELETE on it will not jump the spot drill.

You would have a choice. If you temporarily want to skip a section of code.

Be careful what N Numbers you choose so as not to mix them up.

Maybe you broke all the taps and you don’t have anymore so you want to skip the tapping. In this case I’d just jump with M99 and then take it out before saving the program.

However, see the next Example.

For this last example you might have to think a bit. Call me finicky but I like the BLOCK SKIP/BLOCK DELETE as a default to be off.

Most machines now don’t have a mechanical switch for BLOCK DELETE/BLOCK SKIP so when you turn on the machine block skip will always be off.

That means the default would be to jump the code.

My way of looking at it, is that you would want the default to be running the whole program as normal.

So We Are Agreed

The default should really be the way the programme was originally done.

In the example below if the block skip is off, which it will be when you start up your machine.

The first thing it will do is jump over the bit that tells it to jump the code.

Meaning it runs as normal not jumping any tools.

The Clever Shit (M99 Plus Block Skip)

M99 Plus Block Skip
What’s This?

Now I know this is a bit confusing and maybe I didn’t explain it too well. Trust me it works.

What’s the matter with you lot just take some time to fuckin read it.

Sorry I’m losing my temper a bit here, the dog’s just pissed on the TV remote again. Just read through it a few times and the penny will drop.

CNC Training Centre Classroom Training

Where the teacher is never angry.

DO NOT PASS GO DO NOT COLLECT £200

Yes you can do this with GOTO

This is my pet Cockroach his name is Boris

GOTO 100
Same as M99 P100

To do this you must have the Macro Option if you don’t then this is where M99 comes in handy.

Best way to see if you have macro is to try using it in MDI.

In MDI Type in #1=6 if you have macro it will work if you don’t you’ll get an alarm and your machine will self destruct in 15 minutes.

Jumping Sections of Code on a Toshiba Tosnuc 888 or Similar

This is how you do it on a Toshiba (the blue bit).

Don’t forget it’s GO (that’s G and letter O) not G0 which is G and number zero (Rapid Command).

Don’t get your letter O’s and your number zeros mixed up.

/M99 P50                                   /[GO,50]               (JUMP TO N50)
M99 P100                                    [GO,100]            (JUMP TO N100)
N50                                              N50                      (ARRIVE HERE
THE CODE
THE CODE
THE CODE
ETC
ETC
ETC
ETC
N100                                            N100                      (ARRIVE HERE)

Without Fancy Shit  (Just jump some code)

M99 P100                                    [GO,100]            (JUMP TO N100)
THE CODE
THE CODE
THE CODE
ETC
ETC
ETC
ETC
N100                                            N100                      (ARRIVE HERE)

If you have macro you can do a similar thing on Mazak, Haas or Fanuc.

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.

Call 07834 858 407

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.

Rigid Tapping G84 Canned Cycle

Tags :

Category : Fanuc Mill Haas Mill Mazak Mill New Stuff

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.

Rigid Tapping G84 Canned Cycle

What is Rigid Tapping?

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.

Rigid Tapping G84 Canned Cycle

So What Use Is This You Say

Well here are some of the advantages.

  1. No need for expensive tension and compression tapping heads.
  2. You can control the depth of the thread very accurately.
  3. It is ok to re-tap the same hole if it needs to be deeper.
  4. Peck Tapping of difficult materials is possible (Yes there is such a thing).
  5. Quicker set-up times.
  6. Feed is the same as the tap pitch.

Rigid Tapping G84 Canned Cycle

But There’s a Catch

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.

Rigid Tapping G84 Canned Cycle

Rigid Tapping G84 Canned Cycle, Fanuc, Haas, Mazak.

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)

Just another interesting note (Read This G98 G99)

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.

Heidenhain Uses Cycle 207

Rigid Tapping G84 Canned Cycle

 

Rigid Tapping G84 Canned Cycle

Oh! And did You Know This??

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.

Rigid Tapping G84 Canned Cycle

On Machines Like The BMC 800 from Toshiba

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)

When you don’t have rigid tapping you need a tapping head like this.

Rigid Tapping G84 Canned Cycle

Notice how it pulls out when the tap stops and reverses.

Ok So what’s Going on Here?

  1. Let’s tap a hole.
  2. Start spindle forward.
  3. Feed to depth at correct speed.
  4. Stop spindle (tap starts pulling out).
  5. Reverse spindle (tap pulls out a bit more).
  6. Start spindle (Needs to reach speed).
  7. Feed out of hole.

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.

Not An Exact Science.

Definitely not, depths will vary. You will probably need to do some hand tapping too.

Tapping Clutches

These are special collets designed to slip at a certain torque. This allows you to get to depth without breaking the tap.

Rigid Tapping G84 Canned Cycle

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.

Haas Have The Answer

Rigid Tapping G84 Canned Cycle, check out this great video on how to stop the machine half way through tapping.

Recover it without busting the tap!!

Ok So Let’s Talk About Peck 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

Why would one want to peck tap?

  1. Holes that clog with swarf.
  2. Difficult materials.
  3. To impress visitors.

Don’t Have It? Don’t Despair You Don’t Need It if You have Rigid Tapping

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?

Thanks For Reading

Don’t forget there’s loads more folks.

And a YouTube channel

Contact Me

Services offered at CNC Training Centre

Edgecam programming and training.

Classroom programmer training.

Onsite CNC Machine 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

 

 

 

Weekend and Online Courses

Onsite Training

Careers in CNC

View all current vacancies in CNC

Click here

Classroom Courses

Apply Now

Call David: 07834 858 407

© Copyright 2020. All Rights Reserved

WP to LinkedIn Auto Publish Powered By : XYZScripts.com