Broach Tooling lathe and mill workpiece advice

CNC Broach Tools recently had a client call us for advice about a internal keyway he was cutting on his mill. He had been using our keyway cutter for a couple of days straight and everything was working great but then without changing anything suddenly he started hearing a noise every time our broach tooling hit the part and his keyway had divets and a poor finish.

Being an experienced user of our keyway cutters he checked everything we usually suggest and still was having problems. After several conversations with me both of us were frustrated as nothing had changed in his set-up. It was a mystery, what had changed?

Chatter just doesn’t magically happen. It’s always a result of something being loose.

99% of the time when clients call me for chatter/finish related issues the problem lies in how they are holding our tool. The other 1% of the time there is a machine issue. I learned something in this exchange about how machine issues can randomly creep in the broaching process.

The problem turned out to be 3 bolts that held the indexing table to the chuck. They each needed a 1/2 turn. Problem solved! How could CNC Broach know to suggest that?

So if you are getting chatter your clues will be the corners of the insert will chip and you will “hear it hit”. You will hear something moving.

  1. always check how you are holding our keyway cutter
  2. then check how you are holding the holder that is holding our holder. (read that a couple of times and it’ll make sense) Whether it is a collet or boring bar sleeve that is holding our broach tooling, that is being held and can move as well.
  3. Then check your workpiece
  4. For mill broaching check the bolts holding your indexing table/chuck
  5. for lathe broaching tighten your ball screws

But 100% of broach tooling users want to blame the keyway cutter! 🙂 of course! that’s the easy way,

CNC Broach knows the problem is never our keyway cutter as our design does not change. We do not walk into the shop, create a one-off design with never before tested dimensions, and send it to somebody interested in our broach tooling. We take a standardized item off the shelf that 3000 other shops around the world are using and send it to you. And these other people are getting great results.

So if you have a problem. Look in the mirror, check your set up then your machine. Then call CNC Broach for advice. We’re always happy to help and are very good at providing clues and steering the operator toward finding the problem.

But do not suggest your problem is the broach tooling. It’s like going to the hardware store, buying a hammer, and then calling the hardware store to complain when you hit your thumb.

  1. It’s not the grade of carbide.
  2. It’s not the design of the keyway cutter
  3. It’s not the feed and speed that your running the broach tooling.

If the insert pulls out of the pocket, thank us!! we just saved your spindle! Inserts pull out of the pocket for 3 known reasons, :

  1. You do not have enough relief for your blind keyway
  2. you did not go far enough past the end of the keyway to allow for deceleration
  3. programming error and you stopped in the material at some point

CNC Broach created our keyway cutter design to protect your spindle. This design is patented and has not changed since 2006 when it was sold through Razorform Tools.

 

Keyway Broaching 316 Stainless-Client Testimonial

Internal Keyway Broach

Internal Keyway Broach

Shane King at Atlantic Hard Chrome sent us this picture and his testimonial about broaching 316 Stainless with our Broach Tool. This feedback is extremely important because then we all learn common feed/speed details. This is a very long Keyway at 3.5″

The Broach Tool was ran at 250 Inches per minute and .001″ Depth of Cut per pass

Shane reported insert life of approximately 100 keyways per cutting edge.

Shane said before CNC Broach Tools it used to take his company 30 minutes to put a keyway in with transfer and set up time. With CNC Broach Tools the process is now 2 min per part.

Shane reported he had a job with 100 parts to do which used to take him 50 hours.

With CNC Broach Tools at 2min per part now the process took 3.3 hrs.

 

Broach Keyway

316 Stainless Broached with CNC Broach Tool

Holding your CNC Keyway Broach Tool

The number one rule for holding our keyway broach tool is to never, ever modify our factory rear shank. It has a flat on center-line of the insert. If the set screws for your boring bar sleeve do not line up at 12 o’clock, then get a different holder. Also, use fresh set screws in your boring bar sleeve.

The number two rule is to have a back-stop. Have the broach tool butt up against something so that it can not slide back. Whether you’re using a boring bar sleeve or the recommended ER collet you must have a back-stop.

If you’re using an ER Collet do not hold the collet in a VDI boring bar sleeve or similar holder. Hold the Collet directly in a Cat 40 or 50. The shank of the ER collet must be held from multiple directions off-set 90 degrees. The problem with a boring bar sleeve holding an ER collet is you are dangling our tool farther out. The VDI holder has set screws from the sides. Take a pencil and put 2 fingers on each side and run the pencil into a wall. What happens? the butt of the pencil moves up and down. And when you trig out the length of the pencil it’s moving the most at the tip. This movement will create taper in the ceiling of your keyway and possibly decrease insert life.

 

Tips for broaching internal keyways on CNC mills and lathes

CNC Broaching info:

use water soluble coolant if you can….and thicken up your oil to 10%, especially for Stainless.

1) Start cut with insert and tool face minimum 1.00” away from part being machined to allow space to accelerate to full cutting speed. .

2) How rigidly you hold our tool is the difference between whether it works or not. ER Collet sleeves are good. Holders with only one or two set-screws are NOT rigid enough. you want a holder that wraps completely around our shank and SQUEEZES down hard.

3) BLIND KEYWAYS are tricky. We recommend doing blind holes on a lathe. NOT a mill. Gravity makes the chips pile into the relief area and cause crashes. With a lathe they drop away.

If going into a blind hole there MUST be an appropriate relief

If the chip is taking up the back of your relief, you don’t want the insert impacting it and nudging the insert up in the pocket over time…program your cut to end closer to where you exit the Keyway into your relief, not at the back of the relief

4) Depth of Cut should be .0008-.0015 per pass”. We recommend 250-450 IPM (Inches per minute) on the rough-cut and 150 IPM on the final pass for finish.

5) Program the tool to drop down completely out of the keyway on the retraction.

6) For clients running months long production, change setscrews in your tool. Setscrews worn out by friction will “flatten” and not grip causing insert “pop-up” and crashes.

7) No Ramping, Slanting or Angled cuts. Razorform is designed for a straight-ahead cut. Improper use may result in the insert pulling out of the pocket or the tool crashing

Take the time to make sure you are square. tightening set screws on your boring bar sleeve or EM holder can “cock” the broach tool out of squareness. Put a gauge block in the pocket of the cnc broach tool, and indicate up/down/left/right to 100% guarantee you are square…..think!!! if you hit the part and you are not square the insert will chip. Take the time to indicate this in!!! It’s worth it.

these are long tools, the clearance needed to slide this tool into your EM or Boring bar sleeve can cause problems. If it’s cocked a hair at the base of the tool, 5 inches away at the tip of the cut it will be cocked much more because the broach tool is so long….

some of our clients love this hydraulic Cat 40 tool holder from Kennametal

Broach tool on lathe helps operator discover turret and headstock is out

Here are two examples where our tooling actually helped an operator discover how their machine was out:

The nice thing is I actually found a machine issue because of this tool. I discovered the turret was off in rotation by 0.075″. I never ran a part. I caught it while I was checking to make sure the tool lined up with the relief hole in the part. I noticed by eye that the tool was not centered with the part. I thought it was the holder, but after about 4hrs of troubleshooting I discovered it was the turret. I think the turret pins must be tweaked from a previous crash. I am now going to run the tool in a horizontal machining center where I have way more control.

-this was from an anonymous machinist working for a big corporation-

John,

Finally (about 3 months ago) figured out the whole off center broach issue. It was indeed the machines headstock was out of square to the tool turret. It apparently had been like this for years before I came to work here. I guess I never turned a long enough diameter to notice the taper/alignment issue. We aligned the headstock and turret back up and the first broached part we ran was on center within .003”.

Your tools are great and I always let people know about your products whenever possible!!

Thank you with all your help with this issue.

Sincerely,

Adam Waterhouse

Process Engineer

Clifton Machining CNC Dept.

Machining Division of Great Lakes Automation Services, Inc. / AMI

A Service Disabled Veteran Owned Small Business

Cage Code: 45RG9

 

Hi all,
recently was getting a 1/4 taper at the beginning of our keyway. Turns out that the milling head on our 5 axis Mazak doesn’t let the servo’s  kick in quite fast enough to recognize the load.
SO, don’t use the milling heads guys…
Happy Broaching,
un-named client

 

Broach Keyways on Haas Mill

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:

 

 

HaasMillBroachProgram

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…

A NEW Haas Mill Keyway Broaching program from our friend Lee at Cutting Edge Mfg in Arizona:
” Below is our program for cutting a traditional .250 keyslot.  Diameter on this bore is 1.00 with the height being .130 (dimensioned as 1.130 +.010 -.005 on print). 
 
Thanks.
 Lee”
 
%
O01234 (XXXXX OP-2) 
( PART # = XXXXXXXX ) 
( REVISION = X ) 
( CUSTOMER NAME = XXXXX ) 
( CYCLE TIME = 1:52 6/16 M1 ) 
 
(TOOL LIST) 
 (T23 =  BROACH TOOL) 
 
(WCS G59) 
(ORIGIN = CENTER, TOP OF PART) 
 
(*** SET TOOL TO CUT @ 12:00 ***) 
(*** MUST USE COLLET HOLDER ***) 
(*** CENTER OF TOOL TO EDGE OF INSERT = .486 ***) 
(*** APPROACH IS @ Y-.025 FOR CLEARANCE ***) 
 
G00 G17 G40 G49 G90 G94 
G91 G28 Z0 
M01 
 
T23 M06 (BRT-252 / BI-252 – BROACH TOOL) 
M01 
G90 G59 G00 X0 Y-0.02 M05 
G43 H23 Z1. 
Z0.5 M08 
 
G90 M19 P0. 
M97 P1000 
G90 G00 Z0.5 
 
G90 G00 Z0.5 M09 
G91 G28 Y0 Z0 
M30 
 
N1000 ( R/F SLOT ) 
( ROUGH ) 
G90 G00 X0 Y-0.02 
Z0.5 
M97 P100 L73 
 
( FINISH ) 
G90 G00 X0 Y-0.002 
Z0.5 
M97 P200 
M99 
 
N100 ( ROUGH BROACH – LOCAL SUB ) 
G91 G00 Y0.027 
G01 Z-2.875 F450. 
Y-0.025 
G00 Z2.875 
M99 
 
N200 ( FINISH BROACH – LOCAL SUB ) 
G91 G00 Y0.154 
G01 Z-2.875 F200. 
Y-0.146 
G00 Z2.875 
M99 
%

 

Secrets of Broaching on a CNC Mill

http://blog.cnccookbook.com/2014/11/06/broaching-cnc-mill/

Bob Warfield over at CNC Cookbook runs a great blog on all things related to CNC Machining and programming. When he posted about our keyway broaches being used on a clients Haas mill a lot of comments came from people “stuck in their ways” about the potential damage to the mill. People who had never done the mill broaching process but had a strong uninformed opinion.

The great thing is if you continue to scroll down through the blog post many of the CNC Broach Tool and Razorform Tools clients jump to the defense. I’ve always felt we have a strong following for our broach tooling but seeing the clients rally behind our product made us feel great!

More and more machine manufacturers are giving the OK for the broach process. At .001″ depth of cut there is no force! You are not hurting your machine! We have thousands of clients doing this. If they were damaging their expensive machines would they be using our product? The “old school” way of thinking about broaching as gouging out large chunks of metal needs to shift to a light shaving action at high speed. It’s a new approach. Watch the video link:
https://youtu.be/reErqhcUE7g
if you want to see a large successful valve company, Ruland Manufacturing broaching a blind internal keyway on 1215 steel taking .0023″ depth of cut per pass at 550 inches per minute. They have Haas mills dedicated for this.

Mill Broaching Blind Keyway

Mill Broaching Blind Keyway

Broaching a Blind Hole Keyway in 304 Stainless

In the video below, Derby Machine Shop in Kansas describes their success blind keyway broaching 304 Stainless with our broaching tools. Lathe broaching blind keyways is preferable to mill broaching them as gravity is your friend helping the chip you’re pushing in front of you drop out of the relief space. You can still mill broach blind keyways but a large cross hole relief is recommended. Derby Machine found the sweet spot for cutting 304 stainless keyways was .0008″ depth of cut per pass at 200 inches per minute. This gave them a minute and half cycle time per part with an astounding one hundred keyways per cutting edge in insert life. Our keyway broach inserts have two cutting edges per insert! Pretty impressive insert life in nasty material. Again this is a client testimonial, a third party describing their experience with CNC Broach Tools. Modern Machine Shop magazine was so impressed they wrote up an article about the lathe broaching process linked to here:
http://www.mmsonline.com/blog/post/id-broaching-a-blind-hole-in-304-stainless

http://https://youtu.be/KF9XvW-Oh54

lathe broaching internal keyway

lathe broaching internal keyway

CNC Broaching Process #1 most popular Blog post for 2015

http://http://www.mmsonline.com/blog/post/the-10-most-popular-blog-posts-of-2015

We are very proud that our slotting tool for cnc lathe and mill broaching was the #1 most popular blog post for Modern Machine Shop. We receive heavy interest in moving the broaching process away from the “old school” methods and having parts with internal keyways come off of cnc machines complete.