Categories

 

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

Subscribe

Join 100,000+ 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

What Every CNC’er Ought to Know About Tool Deflection

Mar 21, 2016   //   by Bob Warfield   //   Blog, FeedsSpeeds, Software, Techniques  //  7 Comments

MillDeflectWhat are the limits of Tool Deflection?  Why?  And is G-Wizard Calculator optimistic or conservative about those limits?

I recently finished several fairly in-depth discussions with folks running expensive production machining jobs about the limits of Tool Deflection and how to think about them.  First, Tool Deflection is extremely important to Tool Life, Chatter, Surface Finish, and the Tolerances on your jobs.  If your Feeds and Speeds ritual does not involve checking the Tool Deflection, you’re leaving money on the table and likely dealing with problems you’d rather not deal with.

But how much is too much deflection, and how should we think about it?

Tool Deflection has four evils:

  • It can instigate chatter.  If deflection is low enough, chatter is much less likely.
  • It can reduce tool life.  Deflecting a tool is bending the tool, and we all know what happens when we bend a paperclip too many times!
  • It can ruin surface finish.  Depending on the conditions, the tool may deflect into the wall of the cut leaving a chatter-like ripple.
  • It messes with tolerances.  Your CAM software assumes a perfect cylinder, not a deflected bent up one that is thrashing around in the cut.

Based on these evils, how much deflection is too much?  Like so many things, it depends.

 

How G-Wizard Sets Chatter Limits

Let’s start with how G-Wizard determines deflection limits.  They’re very conservative and are based on recommendations from major tool manufacturers like Ingersoll designed to limit the onset of chatter.  These are in fact the most conservative limitations on deflection.  For roughing, a limit of 0.001″ is set for a typical solid endmill of 1/2″ or so, and this is scaled based on cutter diameter when you start talking really small endmills or really big ones.  Since this is the most conservative limit on deflection, we can be assured that Tool Life, Surface Finish, and Tolerances are likely taken care of too with this limit.

If you wonder about chatter and deflection, pop over and watch the great Haas video where they vary spindle speed to control chatter on a lathe.  The reason they have the chatter is they’re hanging bars out too far without a tail stock and they’re deflecting.  This time it’s the workpiece and not the tool, but the principle is the same.

When finishing, we will want a tighter limit, primarily for surface finish and tolerances.  We rely on the finish pass to clean up tolerance issues that may have developed due to deflection, and in fact, tolerance is the most generous allowance for deflection, so we can mostly ignore it given a finish pass for clean up.  After all, if we’re going to shave 15 thou for the finish pass, we can tolerate up to 15 thou in the roughing pass.  Our deflection should be much less than that under any circumstances.  G-Wizard will automatically tighten the limit in Cut Optimizer for Finishing.

 

What if There’s No Chatter?

Can you exceed G-Wizard’s chatter-based Deflection warnings?  Absolutely–chatter may not have been a risk for the combination of parameters you were using for the cut.  But you need to think about what your strategy for chatter is going to be.  For many, avoiding even the possibility of chatter is better than dealing with it in the heat of a job.  If that’s the case, respect the limits G-Wizard sets.

OTOH, if you’re going for broke on your Material Removal Rates, you need to consider more aggressive strategies.  You could just forge ahead and choose to deal with chatter if it comes up.  That being the case, you can probably tolerate a higher deflection limit.  G-Wizard provides a means to change that limit on the Setup Other tab:

DeflectLimit

You can override G-Wizard’s Deflection Limit on the Setup Other tab…

Try bumping it up, particularly if you run a more rigid machine like a Horizontal Mill.  You may get by with it set quite high.

If your shop is fortunate enough to be taking a scientific approach to chatter, you can probably quit worrying about chatter when choosing your deflection limits.  Chatter is highly repeatable and largely depends on just four variables:

  • Machine
  • Tool Holder (not the exact holder, just the same brand and model)
  • Tool (again, just the same brand and model)
  • Stickout

That’s a manageable number of variables, and if you know the chatter danger zone in terms of spindle rpm for those variables most of the time, you’ll know whether chatter is even an issue for the Feeds and Speeds you’re contemplating.

 

Deflection and Tool Life

Moving along from Chatter, the next issue for Deflection is Tool Life.  Here, Tool Deflection acts like Tool Runout.  In fact, they are additive.  Think of your Tool Life as being subject to Runout + Deflection.  Now given that combined number, and for a good spindle, you might assume runout is nil and view it totally as a function of Deflection, let’s look at the impact on Tool Life (taken from our article on Tool Life vs Runout):

Tool Life as a function of Runout, where Runout is measured as a % of chipload…

The chart measures Runout (or Deflection as we’re talking about here) as a % of chipload, which makes sense.  Bigger cutters allow more chipload and more runout.

Let’s say we’re running a 3/4″ endmill for a roughing operation.  G-Wizard’s default on a TiAlN Carbide Endmill suggests a max of 0.0036″ chipload.  You can buy endmills that allow more, but let’s run with this.  If we take G-Wizard’s 0.001″ deflection limit, that’s about 28%.  We can see from the chart we’re still going to get 90% of our Tool Life or so.  Deflection is probably not the big factor.

But, what if we run 0.003″ of Deflection–3 times G-Wizard’s recommended limit.  Now we’re at 83% of chipload and the chart suggests we’re probably going to break that tool in short order.  I look at that chart and about 80% Tool Life, which corresponds to 35% of chipload for the Deflection, seems like what I’d be willing to put up with to get a little more aggressive cuts.

That tells me I might set G-Wizard’s Deflection Limit (on Setup Other) up to maybe 120-125% if I wanted to live life on the aggressive side.  As it turns out, G-Wizard’s default is pretty reasonable for most users.

 

Other Odd Tool Deflection Pitfalls

Sometimes, there will be other considerations for Tool Deflection.  I was visiting a shop one day that had just gotten Volumill in for HSM toolpaths.  They wanted to try it out and fired off a job.  Things were going nicely when suddenly we heard that telltale “PING” as the cutter bounced off the enclosure window.  Dang, broke a cutter.  What happened?

He hadn’t used G-Wizard for Feeds and Speeds, so I immediately checked it out.  The only thing amiss was an excess of Tool Deflection.  Upon examining the part closely, here is what we saw:

See the tiny wall the red arrow points too?

See the tiny wall the red arrow points to?  Because of tool deflection, the cutter wasn’t where it was expected and we got that little wall.  It shrouded the cutter from coolant reaching it for a very short time before the cutter broke.

Problems like this are almost unpredictable, but they can crop up if we’re too aggressive all the time with Tool Deflection.

Using a Chipload Budget to Manage Deflection on Tough Jobs

More recently, I had a conversation with another customer about why a cut was working.  It seemed like it had an awful lot of deflection.  But it turned out something very interesting was happening.  This was one of those tough jobs that required a lot of stick out to get down into a hard to reach place.  They were running very little Cut Width and as a result, there was Radial Chip Thinning, which meant chiploads were artificially low.

It turned out that the sum of the Tool Deflection and the actual chipload were well within the limits of max chipload for the endmill.  In effect, we had a “Chipload Budget” where part was allocated to the actual chip and part was allocated to the Deflection.  It was working out just fine for them.

This trick is worth keeping in mind for those difficult jobs.  Sometimes you may need to trade some excess Deflection for some reduced chipload to get those jobs done without taking too many passes.  Doing so enabled this particular job to be done in one full flute length pass.  Very clever!

 

Conclusion

It should be obvious by now that Tool Deflection can have a big impact on your work.  If you’re not using a tool like our G-Wizard Calculator that automatically incorporates it into Feeds and Speeds, you’re missing out on some vitally important information.

It’s also critically important to understand how your calculator sets a limit on Tool Deflection. As mentioned, G-Wizard’s limits are based on the recommendations of Tooling Manufacturer’s like Ingersoll. If your calculator sets higher limits, ask for a sound explanation of why–they may not be doing you any favors, especially if the answer is they ran some experiments themselves.  Fortunately, it’s easy to get started with great Tool Deflection calculations with our 30-day Free Trial of G-Wizard.  Check it out!

 

 

Like what you read on CNCCookbook?

Join 100,000+ 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!

What Every CNC’er Ought to Know About Tool Deflection
Rate this post

7 Comments

  • Gwizard is full of machining tricks! To all the power gwizard users out there, “give thanks to the all mighty deflection tools, MRR data, chip thinning!, and hail to Mr. Tortoise and the March hare. May they guide us to machining success! 🙂 ”
    Hey Bob, if you ever insanely retire the tortoise and the hare, would I be able to suggest on the left side is a picture of a prototrak and on the right, a picture of an operator sweating bullets hovering the feed hold button. JK

    Thanks for the tips and tricks!
    Genuel

    • LOL, Genuel, I like your operator sweating bullets–been there sweated some 45 cal slugs.

      But, Mr Tortoise and The March Hare can’t retire–I fell in love with them the very first time I saw a Bridgeport with those symbols on that crazy ole Varispeed pulley. We don’t need no stinking VFD’s back then boys!

      Though the Monarch 10EE basically had a vacuum tube equivalent of the VFD long ago in those machining galaxies far away. We young upstarts must never think the old timers haven’t already seen most of what we think of as new.

  • […] in an apprenticeship model, and CNCCookbook broke down those barriers. When GWizard introduced tool deflection calculation, I fell in love. It has never left my side since then. We now use our Tormach in almost every […]

  • […] is a complex topic, and I’ll refer you to a dedicated article for more information.  Suffice it to say we allow more for roughing than finishing because too much deflection is bad […]

  • […] is a complex topic, and I’ll refer you to a dedicated article for more information.  Suffice it to say we allow more for roughing than finishing because too much deflection is […]

  • […] About 9:43 looks like one end of the mag well was chain drilled.  Why not chain drill both ends at this time?  Is it because the other ends has different radii in the corners perhaps?  Also, not that the milling of the deep magazine well is done from both the top and the bottom.  This limits the required stickout of the endmill and minimizes tool deflection challenges–nice! […]

  • […] About 9:43 looks like one end of the mag well was chain drilled.  Why not chain drill both ends at this time?  Is it because the other ends has different radii in the corners perhaps?  Also, not that the milling of the deep magazine well is done from both the top and the bottom.  This limits the required stickout of the endmill and minimizes tool deflection challenges–nice! […]

Leave a comment

 

Do you want to be a better CNC'er in 37 Seconds?

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

It's that easy. You can install and get results in a matter of minutes.

 

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.