Category Archives: Mazak Mill

Canned Cycles Using G98 G99

This article is about CNC Canned Cycles Using G98 G99

Canned Cycles Using G98 G99

(G Code CNC Programming)

It’s not a competition G99 vs G98. sometimes you need G98 sometimes you need G99.

CNC Canned Cycles Using G98 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.

G98 G99

  •  Depth
  •  Feedrate.
  •  Point to rapid to before drilling
  •  Point to rapid back to after drilling

Canned Cycles Using G98 G99

G Code Programming Haas Fanuc (ISO) Mazak

What happens then is each time we give the machine a new position it will drill one of these holes. Each hole will be identical unless we change one of the parameters. So if on one hole we put a different Z depth that hole and all subsequent holes will be to the new depth.

CNC Canned Cycles Using G98 G99

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.

Machine says OK he don’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. Anyway they all do different stuff like.

  • G84 Tapping
  • G73 High speed Peck Drilling
  • G83 Deep hole Drilling
  • G81 Drilling

They all work in the same way as each other but with variations.

Now the video at the bottom of the page is about CNC Canned Cycles Using G98 G99 and that’s in all the drilling and tapping type cycles.

Ok what does it do? You may well ask, G99 vs G98

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. Maybe you don’t care.
Anyway it’s simple.

  1. You rapid to an initial point
  2. You rapid down close to the hole (this is the R point)
  3. You feed down to depth (Z Depth)
  4. Then you rapid out to either the initial point (1) or the R point (2)

Canned Cycles Using G98 G99

Now if you program G99 it returns to the R point .
If you program G98 it returns to the initial point (that means the first one)

Ok why on earth would I want that?

Well……. if you made the first point say 50mm above the job (About 2 inches) and the rapid point was 1mm above the job (.040”).
You could drill all your holes in G99 and the drill would each time return to 1mm (.040″) above the part. You get to a clamp and you put G98 and it jumps to 50mm (2”) above the part and misses the clamp. Change back to G99 and it stays down returning to 1mm (0.040) above the part.

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

Canned Cycles Using G98 G99

CNC Canned Cycles Using G98 G99

Take a look at the CNC Training Courses on offer at the CNC Training Centre

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

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

Please don’t let on if you don’t like it as I am easily offended.

If you want to learn to program CNC Machines

If you want to learn to program CNC Milling Machines

If you want to learn to program CNC Lathes

Look no further Contact CNC Training Centre

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

We offer training on all types of CNC Machines and controls check em out.

contact@cnctrainingcentre.com

Or fill out the contact form below



G28 G53 Zero Return

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.


Jump Around Using M99 Plus Block Skip

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


Jumping Sections of Programme Using M99 and Block Skip

 

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.


WP to LinkedIn Auto Publish Powered By : XYZScripts.com