Cycle Format:

G184 X Z C K (I) F Q E
OR
G184 X (Z) R C K (I) F Q E

G180 (Cancel)

• X:
  For face operation: Start Position
  For side operation: Target Diameter
• Z:
  For face operation: Target Position
  For side operation: Start Position
• C: C-Axis index position
• I: Shift from G00 for SIDE operation only
• K: Shift from G00 for FACE operation only
• F: Feedrate
• E: Dwell
• R:
  For face operation: Depth of hole, Negative
  For side operation: Diameter

• Q: Number of holes to repeat

Example:

As part of FS Wizard's development. 2 drills were tested today on T6061 Aluminum.

0.312 Dia and 0.390 Dia Dormer A002 Drill Jobber Drill with TiN coated tip.

Helix:30Deg

Point:Split, 118Deg.

Hole depth for both was 3.0"".

Peck equaled 1xDia

Speeds and Feeds for 0.312 Dia drill were

SFM: 250 f/min

Tool:0.281 dia 0 helix TIN coated carbide drill

Recenty ordered a 3Flute High Performance End Mill From NIAGARA.
Was very glad and slightly surprised that when punched in all of the endmill's data into my Calculator nothing broke down.I had a rason: At 5000RPM and 3/8" Deep slot cut. The feed came to around 92.0IPM. Chips were making this nice ringing noise that sounds like money.

Setup:
HAAS VM-3
Hudrolic Tribos Holder
3/4" 45DegHelix 3Flute 1.625FluteLen, 2.375"Overhang TICN HP End mill

S:5000RPM
F:92.0IPM
DOC: 0.375" Slotting
Coolant:FLOOD

The calculation was pretty much dead on.

A need arouse to drill and tap lots of blind 1/4-20 holes in 3/4" thick hardox 45-50RC hard plate.

So if you ever need to do this use:

1) DRILL
Tap hole: >0.202" or bigger.  5/8 deep.
Drill used: Tialn coated carbide drill.
S=1418 RPM
F=2.6 IPM
NO Peck, No Coolant

2)TAP
Tap: TIALN coated 4Flute PowderMetal tap from OSG.
S=100RPM
Rigid Tap Peck:0.05"
Depth: 0.40"
Used MAsters Cutting oil. Pretty standard for tapping.

Was able to drill/tap 16 test holes. After inspection tap did not show sings of severe wear. So its safe to assume you could make around 30 holes this way.

If you ever have to do this- GOOD LUCK

Renishaw OTS tool probe cycle for HAAS can set both length and diameter offsets.

Too bad there is no choice: it only puts absolute measured diameter of the tool into D- diameter offset and makes wear offset=0

But if your programming is done with the center of the cutter, then you actually only need the difference between actual and programmed diameters of the tool.

I.E.: When probing 5/8Dia end mill, we get D=0.6248. You would normally have to subtract 5/8 from it and leave the -0.0002 difference.

But there is an easier way

Warning:Make sure you know what you are doing.
Make sure you backup all files you are going to modify.
I simply WILL NOT care about any damage done to your machine in any case.

• Go to settings and set  protect 9xxx programs from edit to OFF
• Go MEM and edit program O09852 (RENISHAW DIA. SET)
• Go to line N31 and replace
• Code:OLD
  .....
  N31
  #[ 2400 + #7 ]=  #8 / #156
  .....
  
  with
  
  Code:NEW
  .....
  N31
  #[ 2400 + #7 ]= [ #8 - #19 ] / #156
  .....
• Go to settings and set  protect 9xxx programs from edit to ON

Thats it.

Now when you probe tool for diameter, D offset will contain the difference between approximate Dia and actual dia of the tool.

Problem: Work offset G54 Z0 shows some "weird number" which is very hard to relate to.

Can we make top of fixture show Z0=0.000 ?

Solution:

1. Go To Setting 33 (coordinate system) and Set it to HAAS. This will prevent G52 from clearing upon RESET or machine powerup and so on. (note: normal probing routines will require this setting to be Fanuk only).
2. Find actual Z0 offset of your fixture and enter it into G52.

Thats it, from now on the value you enter into your G54-G59 Z is actual distance from top of your fixture to the top of programmed part.

Note: AGAIN this solution will not work with any of the probing software. The workaround for that will be posted later.

FSWizard Online is:

FSWizard is here

It is the most accurate Online Feeds and Speeds Calulator.

In order for every user to enjoy latest modifications and most accurate results, it is WEB Based.
This means that you can use it across all imaginable operational systems and devices.
All you need is an internet connected WEB browser.
No download or installation is required: Just visit the web page.

Also a full functioning mobile version is available.

Key Features of FSWizard:

• Otimal Speed/Feed for particular tool/material combination.
• Axial and Radial chip thinning.
• RPM Reduction for extra long tools.
• Machinig Horse Power and torque estimation.
• Side Force and tool deflection estimation.
• Balancing Depth Of Cut (DOC) againt Width Of Cut (WOC) and vise-versa.
• Speed/Feed compensation for long cutters
• On the fly INCH - METRIC conversion.
• myCut Tool Database. Registered users can save calculations online and then retrieve them without the hassle of re-entering similar data. Each calculation has an unique ID Link and can be accessed and shared by anyone.
• Web based, so No download or installation is needed.
• Also Windows-based version is now available!

Interested?

Check out our FREE Online version here

G71 X Z A|I B D U H L E F J M Q

• D=First Depth of Cut
• U=Finish Depth of Cut
• J=Number of threads at F
• X=Target Depth (minor Dia of theread)
• Z=Coord of end Point
• A= Angle of thread
• B= Tool Cut angle
• H= Difference between major and minor dia of the thread
• M= Cut pattern
• M32= Longitudal
• Q= Number of leads

Note: Feed mode must be in G95(IPR)

Out Company used to have somebody else plasmacut cutting anvils for us.
This was expensive, plus heat generated by plasma caused already unstable anvils to warp like crazy making them very hard to grind flat.

So when foreman told me to machine one on CNC i immidately asked him to buy one of those nifty Hanita TiALN coated Varimill cutters.
Too bad they are too expensive. So the company bought same style of cutters made by Niagara. 0.5" end mill there is x3 cheaper than hanita's. Plus i believe cutting tools made to the same specs, out of the same materials are performing identical.

The machine we ve been using for this is really shaky and busted, so dont laugh at speeds and feeds that we came up with.

So basically, Specs Are:

• Material: Hardox pre-hardened steel Rc 45-50
• Cutter: 4 Flute, Stagger Flute TiALN coted 0.5" Micrograin Carbide End Mill, 2.5" Overall, 0.625" Flute Length, 1" overhang
• Operation: Slotting
• Speed: 1200 RPM
• Feed: 4.8 IPM
• Depth OF Cut: 0.125"
• Plunge method: 2.5 Deg Ramp/Helix, Or Plunge into 0.281Dia pilot hole at 3 IPM
• Coolant: Airblast + Oil