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

Who is Afraid of Tool Deflection?

Sep 4, 2014   //   by Bob Warfield   //   Beginner, Blog, FeedsSpeeds, Software, Techniques  //  1 Comment

MillDeflectWell, if you’re not afraid of tool deflection, you should be.  Here are 7 things to know about it:

1. Tool Deflection is bad for Tool Life

Tool Deflection is bad for Tool Life in several ways:

–  It’s actually forcing the tool to bend.  Like a paperclip, if you bend it back and forth too much, it will break.

–  If the tool bends more deeply into the cut, it can increase chipload to the point the tool breaks immediately.  Consider adding up the target chipload based on feeds and speeds, the runout, and the tool deflection to arrive at the true chipload the cutter will experience.  If you’d never consider running with several thousandths of runout, or exceeding your endmill’s recommended chipload by several thousandths, why would you be willing to run with several thousandths of tool deflection?  All these things look the same to the cutter flute and they all add up.

–  The bending means the tool won’t follow the toolpath that was intended, which can lead to unforeseen consequences.

The latter is one of my favorites.  Here is an example of an unforseseen consequence:

You can tell something bad happened here, right?

I was visiting a shop and they wanted to show me their cool new HSM toolpaths (Volumill and Gibbscam I think it was).  They were laying on the cutting forces pretty hard as HSM helps you to do, and the tool deflected just enough to create a little wall that should have been cut away.  That wall is what the red arrow points to.  It resulted in the cutter being shrouded from access to coolant and so this cutter was suddenly full slotting at HSM speeds.  As you can see, by the time it reached the end of the wall, the chips had built up, welded on, and we get that nice melted aluminum taffy I’m sure we’re all familiar with shortly before it snapped off.

We checked the deflection using G-Wizard Calculator right after it broke, and sure enough, we were in the red and could’ve avoided it had we checked before running the pass.

2. Tool Deflection excites Chatter

The subject of tool deflection originally came up for me when I was researching chatter.  I came across a number of tooling manufacturers that recommended keeping tool deflection below 0.001″ because their research had shown that beyond that value, the tool was working very hard to excite chatter.  Chatter is a resonance phenomenon–the resonance is about vibration and is also why it makes that distinctively painful sound.  Now think of your tool as a tuning fork.  It will resonate at a certain frequency.  Deflecting it a certain amount is like striking it with a little hammer on each flute once per revolution as it peels up a chip.  Are you starting to see how tool deflection excites chatter?

3. Tool Deflection is bad for Surface Finish

It should be pretty obvious that tool deflection is bad for finish.  Instead of getting a smooth wall, you get a wavy one as the tool deflects rhythmically in time with revolutions and flutes.  Here is what such a wall looks like:

The wavy wall on this cut is due to tool deflection…

This one also broke the tool as well as leaving the nasty wavy pattern on the wall of the cut.  And, sure enough, when checked in G-Wizard Calculator, the excessive deflection was very obvious and avoidable.

4. Tool Deflection is bad for Accuracy

This will be the last of the “4 Tool Deflection Deadly Sins.”  Accuracy has to suffer when the tool tip is flapping around due to vibration.  In practice, a little bit of this can be tolerated, although depend on your stepover, you’ll need to beware problems like the coolant wall described above.  A little thought tells us we want to have little or no deflection when the time comes to do the finish pass and accuracy counts.  Think about what you expect from your measuring tools.  If you need to measure within 0.001″, you can’t use a measuring instrument that is only good to 0.002″ or even 0.001″.  You need a tool that is more accurate than what you’re trying to measure.  Same here–you’ll want to make sure you tool deflection is much less than the tolerances you’re trying to hold, especially since it can stack up with the other errors in the job.

5. Tool Deflection is a function of Stickout, Diameter, and Tool Material (Rigidity)

Let’s start to get a handle on the root causes of deflection so we can get control over deflection.  A big part of it is tool rigidity, which is mostly determined by stickout (distance from toolholder to tip of tool), tool diameter, and tool material.  G-Wizard Calculator has a Rigidity Calculator that can help us to wrap our heads around rigidity.  We’re going to use it to explore what happens as we change these three variables:

HSSvsCarbide

Carbide is 3x more Rigid than HSS…

First, you can see the Rigidity Calculator is located under “Quick Refs” and “Rigidity”.  We’ve chosen a 1/2″ endmill with 1 1/2″ of stickout.  The only difference between the two choices is the lower one is made of carbide and the upper is HSS.  The Calculator tells us that this change alone is worth a 3X increase in rigidity.  That’s a big win and is one more advantage of carbide.  Should you then always use carbide?  Many do, but here is something that’s not as well known–if you must live with a certain amount of deflection, HSS will withstand more than carbide.  HSS is more flexible while carbide is more brittle.  This is sometimes helpful to know when all else fails.

BiggerDiameter

Increasing diameter from 1/2″ to 3/4″ is worth over 5x the rigidity!

This example shows what happens when we increase tool diameter.  Going from a 1/2″ to 3/4″ endmill, a 50% increase in diameter, netted over 5X more rigidity.  That’s a big win.  The goes to the topic of “Design For Manufacturing,” which is all about changing the design to make it cheaper to manufacture.  Designers are only human, so they will often specify a corner radius as a nice round number.  Say, 1/2″.  Of course endmill manufacturers are human too and offer the endmills in standard sizes.  What you want is use an endmill just slightly smaller than the corner radius because that’s going to make the nicest cut and be easiest on the endmill, but you want that endmill to be as large as possible while still being smaller than the radius, because the minimizes the deflection, lets us take a beefier cut, and so on.  The best way to handle this is for the designer to make the corner radius a little larger than standard endmill sizes.  But, there is also a sneaky back door approach.  Get out your endmill catalogs.  You could try a 7/16″ and see if you like that better than a 1/2″ endmill for a 1/2″ corner, or you could take a look at the metric sizes.  You can get either a 12mm or a 12.5mm, both of fall between the 7/16″ and 1/2″ Imperial sizes.  Go ahead, sneaky is good in this case!

LessStickout

Reducing stickout from 1.25″ to 0.75″ buys us 4.63x more rigidity…

The last variable we’ll play with is stickout.  Reducing the stickout from 1.25″ to 0.75″ (back on a 1/2″ endmill again) buys us 4.63x more rigidity.  Never use more stickout than you need to.

The Rigidity Calculator further tells us how much each variable impacts things and lists them from most impactful (Diameter) to least (Material):

–  Rigidity increases as the 4th power of diameter.  Little changes in diameter can make HUGE changes in rigidity.  Remember that sneaky metric diameter trick for those super deep pockets where you can’t reduce stickout.

–  Rigidity increases as the 3rd power of length (stickout).  You can still make a big difference by reducing stickout a little bit.

–  Switching from HSS to Carbide gives a flat 3X improvement.

6. Tool Deflection direction can decide whether to use Climb or Conventional Milling

Most CNC machinists use Climb Milling for everything and never try Conventional Milling.  There are very sound reasons to consider Conventional Milling that are covered in an article in the Feeds and Speeds Cookbook.  Take a look at that if you haven’t already, but we’re going to take a little mini-excerpt from it to consider the effect on Tool Deflection.  Basically, what changes is the direction the tool tends to deflect:

The arrows show direction of deflection, climb is at bottom, conventional is at top…

Note that its really hard to predict these directions by calculation, these were actually measured from real cass.  The cutter is feeding to the right, so lets see how that compares to the arrows.  Note that the examples to the right show progressively deeper cut widths.  What we can see is that in conventional milling, with lighter cut widths, deflection makes the cutter “pull back” from the cut a bit.  That’s a nice safety feature because it reduces chipload.  But, if we bury it, the arrow shifts to force the cutter to not only pull back, but also a bit into the wall.  This starts out as a wash, but eventually it results in increased chiploads.  By contrast, lighter climb milling forces the cutter to deflect forward into the cut and a bit inward away from the wall.

In general, imagine that Conventional Milling deflects out of the cut and Climb Milling deflects into the cut.  You’d prefer deflection along the direction of travel because that reduces waviness in the wall and if possible for the direction to be not only along the travel but pulling back from the cut.  That’s a really long-winded way to explain what some of the more experienced machinists have discovered by trial and error.  Quoting from the Cookbook article (link above):

You should switch to conventional milling for the finish pass if you’re at all deflection challenged (use G-Wizard to see if your tool diameter and stickout result in small enough deflection for your finish pass). At the very least, one should avoid too much depth of cut when climb milling lest it invite deflection. The same article suggests that when deflection is to be minimized, use no more than 30% of the diameter of the cutter for conventional milling and 5% for climb milling. Of course here again, if you have G-Wizard, you’ll know what kind of deflection to expect and whether it’s a worry.

Climbing to rough and conventional to finish is inline with the consensus over at Practical Machinist as well.

Properly managing deflection can help you avoid the need for an extra spring cut, which saves time and money.

7. G-Wizard Calculator can help you control Tool Deflection

If it isn’t obvious by now, Tool Deflection is important and you could use some help managing it.  We’ve built a number of facilities into G-Wizard Calculator to help with Tool Deflection.  You’ve seen the Rigidity Calculator above.  GW Calculator’s Feeds and Speeds Calculator will show you the deflection for any cut:

BadDeflection

Check the red:  almost 5 thousandths of deflection on this cut…

We’re trying to cut a slot 1″ deep with a 1/2″ HSS endmill.  Because the slot is so deep, we can’t reduce stickout which is stuck at 1.25″.  What do we do?

Well, as we learned, we could switch to carbide:

TriedCarbide

Switching to carbide helps a lot but isn’t enough…

Switching to carbide helped a lot, but it’s not enough.  Let’s say a larger diameter cutter is just not an option.  Rather, what we need to do is figure out the Cut Depth that keeps deflection under control.  That’s what G-Wizard’s Cut Optimizer is designed to do.  Just click the little speedometer next to Cut Depth (since that’s what we want to calculate–there’s another little speedo next to cut width if you prefer to change that) and it’ll pop up with the answer:

CutOptimizerFTW

With one click, Cut Optimizer determines the best depth of cut would be 0.2485″

With one mouse click, Cut Optimizer determines the best depth of cut would be 0.2485″, and you can save that back to Feeds and Speeds.  Done!

GW Calculator also has a feature called CADCAM Wizard that will suggest the optimum tool, stickout, hints for designers (based on that Design for Manufacturing stuff), cut depth, cut width, and feeds and speeds all while controlling tool deflection.  There is no more complete solution for Tool Deflection problems available anywhere.

If you haven’t played with G-Wizard Calculator yet, try a 30-day free trial.  You’ll be surprised at what all it can do for you.

 

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!

Who is Afraid of Tool Deflection?
Rate this post

1 Comment

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.