Categories

 

G-Wizard Calculator:
Fast, Easy, Reliable Feeds and Speeds

Subscribe

Join 50,000+ CNC'ers!  Get our latest blog posts delivered straight to your email inbox once a week for free. Plus, we’ll give you access to some great CNC reference materials including:

  • Our Big List of over 200 CNC Tips and Techniques
  • Our Free GCode Programming Basics Course
  • And more!

 

GCode is Complicated
G-Wizard Makes it Easy

Thinking About High Speed Machining, Corners, and Stepover

Jun 19, 2012   //   by Bob Warfield   //   Blog, FeedsSpeeds, Techniques  //  No Comments

I recently got a note from a G-Wizard customer who was interested in understanding some tool wear issues he was seeing.  He had two toolpaths, one an HSM (High Speed Machining) toolpath and one a conventional toolpath.  He was cutting hot rolled steel with a 1/2″ stub length carbide endmill, and making lots of small pockets just over 1/2″ deep.  The scale on hot rolled can be tough on cutters, so he made a pass to remove that first.  His question was all about tool life after that pass which was made with a different cutter.

The HSM cut was made by pre-drilling an entry and then running 2800 rpm, 0.005″ chipload, and stepping down 0.185″ per step.  Stepover was 65%.  The conventional cut was made by contour ramping entry and constant stepover of 0.045 and a much higher chipload of 0.014″ and higher rpm of 4500 rpm.  Tool life was far better on the conventional, so his question was basically, “Why didn’t the miracle HSM toolpath do better?”

This is a very interesting case because it really gets into the nuts and bolts of what the advantages of HSM toolpaths are versus conventional toolpaths.  Here was my answer back to him:

It’s all about the stepover or radial engagement.

On the high speed version, you’re running 65% stepover.  On the non-HSM version, you’re running 0.045 / 0.500 = 9% stepover.

So two things to consider.

First, the only difference between an HSM and a non-HSM toolpath is the HSM plays tricks to avoid radically increasing the engagement of the cutter in corners.  For square corners, and 50% stepover, you go from 90 degree engagement to 180 degree in the corner, so the cutter works 2x as hard in the corner.  So, the HSM path doesn’t have to work as hard in corners as your ramping path, but there’s no other special advantage it has as a result of the HSM paath.

That brings me to my second point.

With G-Wizard, we can convert stepovers to tool engagement angles.  So, the 65% stepover, if we key all that in, turns out to be 107 degrees.  It’s a little better than the 180 degree case, but not hugely.

Tool Engagement Angle Calculator

G-Wizard’s Tool Engagement Angle Calculator

If the 9% stepover were done with an HSM toolpath, it would be a 34 degree engagement–which is really starting to cook with fire.

The reason this engagement angle matters so much is due to two factors: chip clearance and the ability of the tool to cool.  It’s pretty easy to see, once we start thinking of these angles, why they matter.  If the tool’s flutes are shrouded only 34 degrees out of 360 of a full rotation, they’re pretty wide open.  It’s easy to get the chips out of the way and the flutes have a lot of time in air and coolant to chill down during the revolution.  With 107 degrees, there is a lot less time.  We go from only cutting about 9% of a rotation to 30%.  The cutter is working at least 3x harder.

So let’s put all this together.  If we were only cutting in a straight line, every toolpath would be an HSM path–no corners to worry about.  And, of the two cuts you used, the 0.045″ stepover cut is 3x easier on the cutter.  All other things being equal, it can go 3x as fast in feedrate or it can have 3x the tool life at same speed, etc..  Those are over simplifications, but you get the idea.

In this case, the stepover on the HSM path, was so close to a non-HSM in a square cornered pocket (e.g. 107 degrees engagement vs 180 degrees) that you didn’t get a lot of benefit from the HSM path.

FWIW, a good starting stepover to try for HSM is 15%.

In other words, if you use too much stepover with an HSM path, you’re negating its potential advantages.  With enough stepover, it’s almost like you’re still going through corners even with an HSM path.
 

Like what you read on CNCCookbook?

Join 50,000+ CNC'ers!  Get our latest blog posts delivered straight to your email inbox once a week for free. Plus, we’ll give you access to some great CNC reference materials including:

  • Our Big List of over 200 CNC Tips and Techniques
  • Our Free GCode Programming Basics Course
  • And more!

Just enter your name and email address below:

Full Name
Email *
100% Privacy: We will never Spam you!

Rate this post

Leave a comment

 

Do you want to be a better CNC'er?

Get Better Tool Life, Surface Finish, and Material Removal Rates.

 

Start Now, It's Free!

Home

Software

  GW Calculator

  GW Editor

  Gearotic

  Conversational

  Deals and Steals

CNC Blog

  Software

  Techniques

  Beginner

  Cool

  Projects

 

Cookbooks

     Feeds and Speeds

     G-Code Tutorial

     CNC Machining & Manufacturing

     DIY CNC Cookbook

     CNC Dictionary

CNC Projects

Resources

     Machinist's Search

     Videos

     Online Groups

     Individuals

     Reference Data

     Books

     CNC Dictionary

     Suppliers

     Tool Brands

Workshop

     Hall of Fame

     Organization: Soon!

 

About

     Customers

     Partners

     Our History

     Privacy Policy

 
All material © 2016, CNCCookbook, Inc.