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/

Leave a Reply

Your email address will not be published.

You may use these HTML tags and attributes:

<a href="" title=""> <abbr title=""> <acronym title=""> <b> <blockquote cite=""> <cite> <code> <del datetime=""> <em> <i> <q cite=""> <s> <strike> <strong>

three × two =