Haas Lathe in Y Axis Program Template

CNC Broaching on Haas Lathe in Y Axis Program Template

CNC Broach Tool contracted out the broaching templates we offer and that is exactly what they are, a guide to build from for those interested in broaching on their Haas Lathe. 
 
We do not provide ongoing programming support or details for your specific application
      
We are not programmers and do not have one on staff
 
The reason for this is we could never get you the right answer anyway as we can never know which of the many coding options you have or have not purchased with your machine. Every year Haas updates and changes their controls
 
The foundational information you find here is all we can provide for you. If you are struggling with programming you need to reach out to the company that sold you the machine to see what options you have purchased and see if Haas has tweaked code or if you need to add an option.

CNC Broach Tools offers free broaching program templates for Haas Lathe. If you want to broach your keyways or splines CNC Broach Tools can help!

Click to download .NC file >Y AXIS CNC keyway broaching HAAS

CNC Broach Tools

Haas Lathe in Y Axis

CNC Broach Tools

Haas Lathe in Y Axis

  • Please do not ask CNC Broach to program your machine for the keyway slotting application.
  • We can never know the different CNC program options purchased with your lathe or mill. Please reach out to your Haas dealer and find out what CNC programming options you purchased with your lathe or mill.
  • CNC Lathe and Mill manufacturers come out with updated controls frequently. Things may have changed since this CNC Broach Template.
  • The CNC broach program templates are a guide or foundation for the user to tailor to their specific application.
  • There is more advanced CNC Keyway Slotting program information in our Keys to Programming CNC Broach Tools guide.
Pleas feel free to leave a comment below to better help improve our templates to help you!

“The Only Inserted CNC Broaching System Manufactured in the USA”

http://www.cncbroachtools.com

DISCLAIMER: This CNC Broach Tool Program Template is for informational and reference purposes only. It is provided without guarantees or warranty. CNC Broach Tool LLC makes no warranties of any kind, either express or implied, including but not limited to warranties of merchantability, fitness for a particular purpose, of title, or of non infringement of third party rights. Use of this programming template by a user is solely and completely at the user’s risk.

Broach Keyways on Haas Mill

Haas Mill Broaching Program Template

CNC Broach Tool contracted out the broaching templates we offer and that is exactly what they are, a guide to build from for those interested in broaching on their Haas Lathe or Mill. 
 
We do not provide ongoing programming support or details for your specific application
      
We are not programmers and do not have one on staff
 
The reason for this is we could never get you the right answer anyway as we can never know which of the many coding options you have or have not purchased with your machine. Every year Haas updates and changes their controls
 
The foundational information you find here is all we can provide for you. If you are struggling with programming you need to reach out to the company that sold you the machine to see what options you have purchased and see if Haas has tweaked code or if you need to add an option.

Click here for YouTube video >> Ruland Manufacturing

CNC Broach Tools offers free broaching program templates for Haas Mill. If you want to broach your keyways or splines CNC Broach Tools can help!

Click to download Haas Mill Broach PDF >> CNC BROACH HAAS MILL
Click to download Haas Mill Broach .NC >> HAAS MILL G CODE BROACH.NC

Haas Mill Broaching

Mill Broaching Blind Keyway

Great Client Input on a common question,

From: Joe
Drifton Precision Machining in Pennsylvania:
We were having trouble indicating the keyway broach square in our Haas Minimill. Here’s the solution:
When orientating the spindle to square up the broach we use an M19 code. We needed to move the position to indicate the broach square. When you use a whole degree you can do M19 PXXX when you need to go less than a whole degree you use an R example M19 R45.05 If you don’t use the R code the spindle will quiver and make indicating difficult. When we got this figured out we had very good success. 

thanks Joe!! also readers, here is a sample Haas mill program provided by a client back in 2008 when our broaching tool was sold through Razorform Tools, we do not vouch for it or provide programming for use, but it is an example:

CNC Mill Broaching a Blind Keyway

– When cutting a blind keyway in a mill, gravity is not working with you

– The material you are cutting can pile up into your relief area causing a crash

– We highly recommend a cross-hole relief when using a mill because the coolant can flush your chips out either side

– With a groove relief your chips can pack the groove, resulting in a crash

THINK ABOUT IT, with a cross hole the chip can get flushed out either side, with a groove, oriented vertically there is a chance that your groove gets packed with chips…

  • Please do not ask CNC Broach to program your machine for the keyway slotting application.
  • We can never know the different CNC program options purchased with your lathe or mill. Please reach out to your Haas dealer and find out what CNC programming options you purchased with your lathe or mill.
  • CNC Lathe and Mill manufacturers come out with updated controls frequently. Things may have changed since this CNC Broach Template.
  • The CNC broach program templates are a guide or foundation for the user to tailor to their specific application.
  • There is more advanced CNC Keyway Slotting program information in our Keys to Programming CNC Broach Tools guide.

To read more about slotting blind keyways click here >>

Blind Keyway Broaching

Please feel free to leave a comment below to better help improve our templates to help you!

“The Only Inserted CNC Broaching System Manufactured in the USA”

CNC Broaching Macro Program For Lathes with Fanuc Controller

Do you need to write a program to broach a keyway, spline, or slot in your CNC machine? Push broaching is continually evolving as manufacturing operations are becoming automated.

– MACRO PROGRAMMING CAN ONLY BE PERFORMED IF YOU HAVE ALREADY PURCHASED THE MACRO OPTION FOR YOUR MACHINE –

The following example is from a DMG Mori lathe with Y axis. The 5 lines at the top of the program which are shown in RED, are theoretically the only numbers you’d need to adjust for your keyway application. Although this is a proven program, it may not work the same in every machine. Use caution when running.

Adjust the numbers in RED with your Length of cut, Starting diameter, Ending diameter, Depth of cut, and Feed rate (in inches per minute).

%

O4567 (BROACH MACRO EXAMPLE)

G0G17G54G40G80G97G99

#501=2.26(ENTER KEYWAY LENGTH HERE)

#502=1.303(ENTER STARTING DIAMETER HERE)

#503=1.520(ENTER ENDING DIAMETER HERE)

#504=.0010(ENTER RADIAL DOC PER PASS HERE)

#505=300(ENTER IPM FEED RATE HERE)

(DO NOT EDIT THESE 3 LINES)

#506=[[#503-#502]/2](AUTO CALCULATES FULL DEPTH)

#507=[#506/#504](AUTO CALCULATES NUMBER OF PASSES)

#508=1(RESETS PASS COUNTER)

N1G00G30U0V0(BROACH)

G30W0

G18G54

T1212

G98

G0Y0.

G50S500

#508=1(RESETS PASS COUNTER)

M45(C-AXIS MODE ON)

G0C0.

M68(SPINDLE BRAKE ON)

G0Z1.0M8

G0X[#502]

M98P0070L[#507]

G0G99Z1.M9

M69(SPINDLE BRAKE OFF)

G30U0.V0.

G30W0.

M46(C-AXIS MODE OFF)

M30

%

Keys To Using CNC Broach Tools

Things you should know when setting up a CNC Broach Tool:

Setting up a broach tool to cut in a lathe  

  1. Mounting the tool: We recommend mounting the tool in a boring bar sleeve. Split sleeves have the most accurate and solid connection when clamping on the shank of our tool . This is because they contact a full 360 degrees around the shank. Solid sleeves can work as well, however when solid sleeves become worn out they are not nearly as accurate or rigid. Slop in the boring bar sleeve could allow the tool to chatter and deflect off center. When using a solid sleeve, always use a sleeve with a minimum of 2 set screws in line with our insert (not 90 degrees to the insert) to prevent taper in the ceiling of the keyway. Never use a solid sleeve with only a single set screw. This creates a pivot point which allows the tool to deflect. If your boring bar sleeve set screws do not orient onto our factory flat, you will need a different sleeve. Please do not modify the tool.
  1. Always use a stop behind the butt of the tool to prevent it from slipping in the boring bar sleeve. 
  1. Dial in the tool’s orientation to be in line with the X axis: To do this, first remove the insert from the holder and find a gauge block that will fit into the insert pocket (any gauge block smaller than the pocket width will work). Lightly snug the set screws down just enough to hold the gauge block in place. Dial the gauge block in as shown in the image below. We recommend dialing in to within .0005”.
  1. Once the tool has been dialed in rotationally along the X axis, dial in the front diameter of the tool in the Y axis. We recommend dialing this in to within .0005” as well.
  1. Once the tool is dialed in, replace the insert. Do not over tighten the set screws as this could cause the pocket to crack or spread open.

Setting up a broach tool to cut in a mill:

  1. Mounting the tool: Our first choice when clamping a broach tool in your mill is to use a Hydraulic holder. If this is not an option due to expense, a solid holder with a minimum of 2 set screws will work as well. Always use a solid back stop behind the tool to prevent it from pushing back. Rigidity is always key when broaching so we recommend using a CAT40/50/60 connection or Big-Plus connection. We only recommend using HSK when it is type A, and we do not recommend using a Capto connection. How you clamp our tool is the difference between whether it works or not. Never use a holder with just one set screw as it will create a pivot point and will most likely chatter.
  1. Dial in the tool’s orientation to be in line with either the X or Y axis: To do this, first remove the insert from the holder and find a gage block that will fit into the insert pocket (any gage block smaller than the pocket width will work). Lightly snug the set screws down just enough to hold the gage block in place. Load the tool holder into the machine and orientate the tool using an M19. Once the spindle has been oriented, dial the gage block in to within .0005” along the X or Y axis.
  1. Once the tool is dialed in, replace the insert. Do not over tighten the set screws as this could cause the pocket to crack or spread open.

Blind holes, Thru holes, Clearance grooves, & Cross holes

When broaching a keyway, the cutting tool must pass completely through the material before retracting out of the cut to prepare for the next cut. This is easy when broaching completely through a part, but can be tricky when broaching a blind keyway.

CNC Broach Tools clearance Relief examples

Turned Undercut                                        Cross Hole                                 Milled Slot /Undercut

Warning – If you have a through keyway application but are broaching bar stock prior to it being parted off, you will still need clearance as shown above

Blind keyways are tricky! You must have an appropriate groove or cross hole relief

The pictures above show 3 options when dealing with a blind keyway. As we mentioned earlier, the cutting tool must continue straight and must pass through the material before pulling out of the cut. If the tool stops accelerating forward without first passing through into a clearance relief, the chips will be compacted in front of the tool and will cause issues. Therefore, you must use either an undercut, a crosshole, or a milled slot /undercut.

  1. Turned Undercut:  This of course is the best option when in a lathe. We recommend the clearance groove to be at least .250” wide min (to allow for Z axis deceleration) and the diameter of the groove must be calculated to allow for the keyway width and radial depth. You can either do the math as shown below, or you can use our online Blind Keyway Undercut calculator which can be found here:  https://cncdirt.com/keyway-time-calculator/
  1. Cross hole: A drilled cross hole is a good option in both turning and milling applications. A crosshole can be drilled from the outside of the part. When drilling, we recommend using a drill which is at least 25% larger in diameter than the keyway width to allow for proper clearance. For example, a .250” wide keyway should broach into a cross hole that is at least Ø.300”. This should give adequate room for chip evacuation.
  1. Milled Slot /Undercut: If a turned undercut or a drilled hole isn’t an option, we recommend milling a slot using a woodruff keyseat cutter. Just like the turned undercut, we recommend the clearance cut to be at least .250” wide (to allow for Z axis deceleration). The radial placement of the slot must be calculated to allow for the keyway width and radial depth of the keyway. There must always be clearance in the corners as shown below.

     4.   Programming:

 We have tons of resources on our website to help you write your program. We even offer machine specific  templates for you to use to make it easy. But, here are our main “keys” to programming:

  1. We recommend taking .0008”-.0015” per pass
  2. We recommend feeding the tool at 250-450 IPM (inches per minute) on the rough passes and 150 IPM for the final finish pass
  3. Program the start of the cut to be .625” in front of the part. This allows your machine enough space to completely accelerate to the programmed feed rate
  4. Program the end of the cut to be at least .080 past the end of the keyway. This allows some room for the machine to decelerate prior to the end of the cut. 
  5. Once the cutter has passed through the material, program the cutter to pull completely down & out of the keyway prior to retracting out of the hole.
  6. We recommend using water soluble coolant with 15% concentration, especially for stainless and other hard to machine materials.
  7. Most machines have an M-code for exact positioning. M61 on Fanuc, for example, will check to verify positioning prior to starting the next move. If your application has too little room to allow for deceleration at the end of the cut and you are seeing taper in the end of the keyway, try using the exact stop m-code. If this m-code is not available, you may need to slow the feed down.

    5.  Questions and answers:

Why does my insert keep pulling out of the holder?

This is usually caused by a programming issue. The insert must pass through the material into air before pulling out of the cut. If the tool retracts down out of the keyway before it has passed through, the wall of the keyway will pull the insert out. The insert was designed to be pushed, not pulled. This is a clue that you do not have enough relief space or the chips are not evacuating the relief space and pinching the tool. 

Why is there a lip at the end of the keyway?

The machine does not have enough room to decelerate in air and is pulling out of the cut prior to reaching the full depth. To fix this you can either program the tool to cut deeper, slow down the feedrate, or add an exact positioning m-code to your program..

  Will I need to change out my set screws on my CNC Broach Tool?

The set screws can wear down over a few months time. Examine the set screw point. If it appears to be flattened it may not grip properly. A worn set screw could potentially cause the insert to pop out. Do not over tighten the set screw as this could cause the pocket to crack or spread open.

Will CNC Broach Tools write my CNC program for me?

We do not have a full time programmer on staff. We can subcontract your programming if needed for an hourly fee. We also however offer templates to get you started. Check out: https://www.cncbroachtools.com/category/cnc-broach-programs/ for more information

Will CNC Broach Tools create a custom shaped insert?

Yes, we have the ability to create custom inserts which include custom widths, custom splines, hexes, and others. These generally take 2-4 weeks to ship. Learn more at https://www.cncbroachtools.com/cnc-spline-broach/

For more questions & answers go to: https://www.cncbroachtools.com/cnc-broaching-faq/

Fadal Mill Broaching Programming Template

Fadal Mill Broaching Programming Template

CNC Broach Tool contracted out the broaching templates we offer and that is exactly what they are, a guide to build from for those interested in broaching on their Fadal Lathe or Mill.   

We do not provide ongoing programming support or details for your specific application       

We are not programmers and do not have one on staff  

The reason for this is we could never get you the right answer anyway as we can never know which of the many coding options you have or have not purchased with your machine. Every year Fadal updates and changes their controls   The foundational information you find here is all we can provide for you. If you are struggling with programming you need to reach out to the company that sold you the machine to see what options you have purchased and see if Fadal has tweaked code or if you need to add an option.

CNC Broach Tools offers free broaching program templates for Fadal Mill. If you want to broach your keyways or splines CNC Broach Tools can help!

Click to download PDF >> CNC Keyway Broaching Fadal Mill

Click to download .EIA >> Click for the .NC file

Mazak Mill
Fadal Mill Keyway Broaching
  • Please do not ask CNC Broach to program your machine for the keyway slotting application.
  • We can never know the different CNC program options purchased with your lathe or mill. Please reach out to your Fadal dealer and find out what CNC programming options you purchased with your lathe or mill.
  • CNC Lathe and Mill manufacturers come out with updated controls frequently. Things may have changed since this CNC Broach Template.
  • The CNC broach program templates are a guide or foundation for the user to tailor to their specific application.
  • There is more advanced CNC Keyway Slotting program information in our Keys to Programming CNC Broach Tools guide.

“The Only Inserted CNC Broaching System Manufactured in the USA”

DISCLAIMER: This CNC Broach Tool Program Template is for informational and reference purposes only. It is provided without guarantees or warranty. CNC Broach Tool LLC makes no warranties of any kind, either express or implied, including but not limited to warranties of merchantability, fitness for a particular purpose, of title, or of non infringement of third party rights. Use of this programming template by a user is solely and completely at the user’s risk.

CNC Broach Tool LLC

PR News Wire

External Blind Spur Gear Broaching

“Hey John Gardner this is John at OE, We finally got around to using your your spur gear carbide cutters that you engineered for us and I wanna let you know they were perfect. Just thought I’d call you to give you that feedback. I know it’s been a long couple months since you made these spur gear inserts. But we finally got around to the project and you know how the wheels the government turns slow. So anyway they worked out great. Just wanna let you know that we appreciate you and I thank you very much. If you need to call me or send me an email you got the information. Talk to you soon with the next project. Appreciate it thanks.”

“Good shit deserves recognition. I wish I could send you pictures of this gear box that we used your tools on to cut these spur gears but unfortunately  government security protocols prohibit it.  We appreciate the design and the ability to still do this without an EDM.  A machined surface is way more cosmetically appealing than a EDM surface anyhow.”  

CNC Broach Tools Blind External Spur Gear
CNC Broach Tools Blind External Spur Gear

Haas VF-6 Automatic Tool Changing Process

Client:

I’ve used both the 36 teeth spline tooling and the .474” keyway tooling. We encountered an issue with our Haas VF-6 automatic tool changing process.  It has nothing to do with your tooling (which worked exactly as advertised, thanks!). But, I have found that the slop between our arbor and spindle drive keys means that we can see up to 1 degree of orientation change during the automatic tool changing process. This leads us to currently have to re-check and adjust our M19 R value each time the tool is reloaded, to ensure it is properly oriented parallel to the Y machine axis.  I am going to attempt to see if hand loading with consistent rotation pressure will show repeatability.  I’m curious if any of your other customers doing CNC broaching have discussed this with you? If they have, what did they arrive at for a solution?

CNC Broach Tools:

Are you trying to hold orientation back to another machined feature? Or are you trying to hold orientation so the tool orientation matches the retract angle?

Is this in a CAT 40 holder?

Client:

This is in a Vertical Mill (Haas VF-6) with a CAT 50 holder. 

The variability I have observed is in the orientation relative to the machine Y axis. That is the stepover and retract axis being used. Z axis is doing the plunging. We believe it is possible to use this tool in our Haas lathe. But, doing so in the normal part production would exceed the available number of tool holders that can be used without interference so would have to be a “stand alone” setup to do it. Plus the initial alignment in the lathe would lack easy adjustability so I haven’t attempted it to date. 

In the Haas mill I simply use the M19 R(angle) to affect any necessary adjustment, provided the tool doesn’t get removed from the spindle.  But every time you send it out and then bring it back the clocking orientation changes by something in the range of a max of 1 degree is what we have seen to date.

CNC Broach Tools:

Is it always off the same amount everytime?


If it is you should have the machine do the auto tool change and then indicate the tool for the initial set up. Because, maybe the auto tool change is consistent. But, you are hand loading the tool to do the set-up and then once it auto changes it’s off. Does that make any sense ? 


If the off amount is consistent every time, I would have the machine change tools. Don’t take the tool out so it will be just like it would when the program runs and adjust it them to be parallel. Then run the tool change a few times and come back to the tool see if it’s still stright.


You  can always order new drive nuts depending on machine. Drive nuts are replaced easily and not expensive.

Also, maybe the specific tool holder you are using has been crashed or the taper is worn out (old) ect. Try a newer or less worn out holder.


Make sure there is no chip getting caught between the machine taper and the tool holder taper. I know this is always something so simple and sometimes over looked and can drive you crazy till you find the smashed tiniest chip stuck to the wall of the machine taper and all of sudden all issues are gone.


Thought of maybe a diffrent cause try changing the tool holder to a different pot or tool number location. Depending how your machine holds and stores tools perhaps the tool pot which is the ” pocket ” that stores the tool in the magazine or carousel is worn out. Allowing the tool to move when the arm or head retrieves it. So if you move the tool location number and the problem goes away you will know the pot is a little sloppy.

I guess the worst case would be the encoder is not repeating but I think that is not the issues, pretty unlikely.

Mill
Mill Broaching Blind Keyway

Broaching Internal Splines on CNC Mill

A client reached out to us for help on Broaching Internal Splines on their CNC Mill.

“Thanks again for all of your help organizing our custom broach tool for our spline work.  We received everything the other day and have it installed in the machine and ready to go. 

I have a question about programming this specific project.  I’ve read through the website and paperwork that we received but can’t seem to find this specific topic addressed. 

In the examples discussing this for a mill, there is only one instance of broach work being illustrated – for example, one instance at 12 o’clock for a keyway.  So moving into the cut and retracting are obviously going to be in that Y axis direction. 

However, for my situation I’ll need to rotate about the Z axis to cut another two splines and then repeat a number of times after that.  Therefore my movements into and out of the cut will not be directly on X or Y. 

So, my question is: what is the usual approach for this situation?  I’ve come up with a couple different solutions myself but wanted to see what the common or “normal” way of doing this is.  One thing I’ve realized in the world of machining is there’s many ways of arriving to the same solution!  Just some are easier than others, and right now my solutions are a bit time consuming. 

I know doing spline work in a lathe would be straightforward by indexing the C axis, but this part is not suitable for the lathe. 

Thanks, looking forward to your feedback.”

Our response:

“I’d recommend using G68 (work coordinate rotation). This should be the easiest way to get around the programming issues. You could create a subprogram which is programmed at 12 o’clock. Then use G68 to rotate the work coordinate before you call the sub program back up for the remaining splines. G68 rotates the work coordinate. G69 cancels it.

See this website for more details: https://www.cnccookbook.com/g68-g69-rotate-coordinate-cnc-g-code/

For more information on programming your CNC Mill

Broaching Internal Splines
Indexable Spline Broaching Systems

Anthony Machine Speed Feed Testimonial

Thank you Anthony Machine for the testimonial!

“Good morning John, 

Thought I give you a little feedback on the tool we discussed last week, now that we are in the stage of learning tool life. We started out at F250. With 0.0008”/pass and immediately learned, the machine feeds at a max of 144IPM. So we are actually rapiding through the cut to achieve more than 250IPM. 50% rapid is 196IPM and going to slow possibly being worse, decided to rapid at 100% at 392 IPM (As this won’t affect cycle time on retracts and positioning) No cutting parameter prevented ripples on the first tries yesterday. This morning the machinist realized he never switched the spindle to low gear (even if it’s physically locked, we wanted to be in low gear) Now we have the smooth cut we wanted to see. We are at 0.0012”/pass now at 396 IPMSeeing how the chips roll up I can see how the width of the relief groove was a concern for you, so far they are clearing fine. My boss plans to buy different sizes once future jobs require more internal keyways.

 Thanks, 

Daniel Goller 

Anthony Machine”

For speed/feed recommendations please visit: Single Point Broaching Speeds and Feeds

CNC Broach Tools Blind Keyway Broaching Groove Relief Testimonial
CNC Broach Tools Blind Keyway Broaching Groove Relief

Testimonial

CNC Broach Tool LLC

MFGgear

G-Tech USA Blind Keyway Testimonial

Thank you Ryan for the testimonial!

“Matt,
Thanks for all the info, feeds and instructions and all. Will be recommending this product to everyone who needs something like this. I chopped up one of the programs on your website for our okuma mill and it worked great.”

Ryan Rios

Ryan at G-Tech did an amazing job at taking our blind keyway broaching advise and put it to play with a functional groove relief at the end of his keyway.

For more blind keyway information click here: CNC Broach Tools Blind Keyway Broaching

CNC Broach Tools LLC

Custom Push Type Broach Tool Bars

Custom push type broach tool bars are frequently asked of our clients to fit the needs of their application. We have always offered special grind inserts to fit our In Stock Broach Tool bars to accommodate those special jobs. But we now offer custom, “one-off” broach tool bars.

There are many options we at CNC Broach Tools consider before we can generate a quote for custom broach tool bars.

  • Is your application high volume? If you only have a couple of one-off parts on a job that is not re-occurring, the special grind inserts option will be your fastest and cheapest path forward, or our tooling just might not be a best fit. If you are going into production and have numerous part runs per year you may want special broach tool bars. We do require a minimum of 2 special broach tool bars per order.
  • What is the time frame of your job? Common lead times are 3-4 weeks. If your job is required in a couple days we unfortunately can not help with custom tooling and the special insert grind option is best. In that scenario Modification to the tool might be necessary as well as special grinds on our indexable inserts.
  • What is the most important information CNC Broach Tools needs? Help us, help you. The most important information needed is your bore size, keyway width, length of cut, and depth of cut radially. But also time-frame, volume and repeatability of the job factor into our recommendations for special “one-off” CNC broaching tool bars.

Cost of custom push type broach tools vary from application. We pride ourselves on creating cost effective, Made in America broach tooling for your applications.

CNC Push-Type Broaching Cycle Time Calculator

Short of time, extra hands, and brain cells trying to figure out a new keyway broach application? Calculate CNC push-type broaching process cycle time on a mill or lathe. To broach keyways on a CNC lathe or mill, CNC Dirt makes understanding broach process time easier! What started out as a simple app has now made moves to replace the machinist handbook entirely.

Push-Type Broach Keyway Calculator
  • Calculate cycle time when push-broaching in a CNC Mill or Lathe.
  • App calculates cut time based on keyway depth, length, & depth of cut.
  • Visit CNCDirt.com for more details