CNC Software CNC Software

Subscribe

 

Categories

CNC 4th Axis Basics: What They Can Do

Apr 8, 2013   //   by Bob Warfield   //   Beginner, Blog, Techniques  //  10 Comments

HA5C-First-Model4th Axis machining is an interesting and important sub-part of the CNC milling world.  Haas actually got it’s start building a 4th axis before it ever built entire CNC machines (pictured on the right).  This is an article series to help beginners understand how and why a 4th Axis is used on CNC Mills.  In the first installment, we’ll look at what a 4th axis is used for.  In the second, we’ll look at how they work.

If you’re new to CNC, your first impression may be that the 4th axis is used in the same way a rotary table is used for manual machining.  Indeed, there are many projects out there where someone converted a manual rotab to become a 4th axis.  While there is a grain of truth to this idea, largely it’s incorrect.  Most manual machining 4th axis work is about cutting features along an arc, something that’s hard to do with a manual machine.  With CNC, cutting along an arc is easy–that’s what the G02 and G03 g-codes are for.  There are cases where we do continuous machining with a 4th axis–in other words, we want the cutter to be machining as the 4th axis turns.  But there are also many other applications.  Let’s go over three major categories.

4th Axis Indexing for Access

First thing to talk about is this term “indexing”.  A 4th axis is typically either used in an “indexing” mode or a “continuous” mode.  When indexing, no cutting happens until the 4th axis is stopped (and often locked with a brake of some kind).  In fact, there are some types which are called “indexers” that can only be used to index in fixed degree increments rather than continuously rotating to any desired position.  By contrast, “continuous” means that machining happens as the part is being rotated.  For example, to produce a cam lobe.

You may wonder why you’d ever want anything but continuous machining, but bear with me–there are lots of useful ways to take advantage of indexing.  Also, you’ll need much fancier CAM software to program continous machining.  It’s very powerful, but plenty of work (perhaps even the majority of 4th axis work) is done simply with indexing.

The most obvious case for indexing is to gain better access to the part.  Suppose you’re making something complex, like a gear:

4th Axis Gear Machining

Machining a gear with a 4th axis…

The 4th Axis indexes each tooth into position, stops, and then the cutter makes a pass back and forth until the tooth is done.  They the next tooth is indexed into position.

Gears are kind of an extreme case because it would be hard to imagine how to make one if we couldn’t index the teeth.  But, there are much simpler cases where indexing is also extremely helpful.  Suppose you have a part like a throttle body that has holes on all sides.  You could build fixtures and do a bunch of setups, one for each side.  Or, you could also use a 4th axis to index the sides so more than one can be machined with a single setup.

In a future article, we’ll get into programming 4th axis indexing.

 

4th Axis Indexing for More Parts

They say that Horizontal Machining Centers can be tremendously more productive than Vertical Machining Centers.  One reason is that the chips are easier to keep clear on a Horizontal since gravity is helping rather than forcing them further down into the hole where they’re harder to get at.  But another reason is that almost any Horizontal Mill has a 4th Axis Tombstone arrangement:

4th Axis Tombstone on a Horizontal Mill
A 4th Axis Tombstone on a Horizontal Mill…

Pictured is a great example from our article on a successful manufacturer that is so productive with their Horizontal Mills they only need 2 1/2 machines–it’s a family business.  They load and unload the tombstone (which is the big upright chunk of cast iron the parts are held to while machining) while the machine is busy cutting new parts on a tombstone in the machine.  As you can see, they have things set up so they can even do more than one kind of part on a tombstone.  This is a powerful technique for improving shop productivity, but it’s not strictly limited to Horizontal Mills.  You can stick a tombstone arrangement on a vertical mill too, there’s just less clearance available so you’ll want relatively “flat” parts to use one:

vmc 4th axis tombstone

4th Axis Continuous Machining

Now comes the fancy stuff: 4th Axis Continuous Machining, which may also be referred to as “4th Axis Contouring”.  This video of a turbine blade being machined makes the difference between continuous machining and indexing pretty obvious:

YouTube Preview Image

There are a couple of advantages to Continuous Machining.  First, you can machine shapes that would otherwise be impossible or very difficult.  The closest thing possible without continuous machining would be to index as many positions as possible and use 3D contouring toolpaths to try to get the job done.  This can be surprisingly effective, but is seldom as powerful as true Continuous Machining.

The second advantage comes when profiling with a ballnose cutter.  The ballnose has a weakness, which is that the closer you get to the tip, the slower the flutes are spinning.  It sounds counter-intuitive, but just think of that tip as a series of concentric circles at different heights.  The ones near the tip are smaller circles, their circumference is shorter, yet they’re spinning at exactly the same rpm as the bigger circles up higher.  Hence, the tip moves slower.  Conceptually, the exact tip isn’t really moving at all as it is a circle with zero radius.

This observation leads to a clever technique called “Sturz Milling”.  With this technique, you use the 4th axis to allow the ballnose to be presented to the workpiece at an angle, so the side of the ball is used more than the tip:

Sturz Milling

Not only does this allow faster milling (higher feedrates are possible) but it gives a better surface finish and even improves tool life.

4th Axis “Wrap” Machining or “Wrapping”

I’d be remiss if I didn’t mention the special case of 4th Axis Continous Machining which is called wrapping.  Imagine you want to engrave some text on the side of a cylinder.  You could lay out a 2 1/2D engraving on a flat surface, and then if you had some way to “wrap” that engraving around the cylinder, it would come out right.  It turns out there are ways to do this ranging from software utilities to options in your CAM software, to even the expedient of plugging the Y-axis into your 4th axis and letting the hardware think it’s machining on a flat surface when in fact its doing wrapping on a cylinder.

Conclusion

A 4th Axis can be a powerful addition to your CNC arsenal.  It enables all new kinds of machining and can also make existing jobs run faster and require less setup.  In our next 4th axis installment, I’ll explore the technology of the 4th axis itself a bit more.

 

 

Like what you read on CNCCookbook?

Join 30,000+ Machinists, Designers, Engineers, and Hobbyists!  Get our latest blog posts delivered straight to your email inbox once a week for free. Just enter your email address below:

 

100% Privacy: We will never Spam you!

10 Comments

  • Bob, please also explain when its good to use a 5C 4th axis indexer (such as the HAAS unit) and a 4th axis rotary table and when 3 jaw chucks (sometimes can be used on both). This is timely as I am converting the control on a Dyna DM4400, recently aquired an old stepper driven HAAS 5C indexer and am considering converting a rotab as well. Pros and Cons of both and setup examples would be helpful for everyone.

    • Sure Marty, I’ll try to include an article on 4th axis workholding in the series. Good idea.

      I will have more to say about converting a rotab in the next installment on the mechanicals of a 4th axis. Basically, I’m not a fan–too much backlash in the worm gear arrangement of a manual rotab. It works for a while, but needs constant adjustment and wears out the gear pretty quickly.

  • Yet one more variable for your speed and feed calculator.

    On an Okuma VMC with Kitagawa 4th axis when you run this code:
    G00 X0 Y0 Z1 A0
    G01 X1 A360 F800 ( more than 800 alarms out )

    The tool absolutely does not move at 800 ipm due to some internal syncing between the simultaneous motion of the two axis, it moved at an estimated 20 ipm, when my ball park guess of required ipm was about 80 ipm.

    Nasty stuff.

    • Yep, it will choose the maximum feedrate up to your commanded feedrate that allows all the coordinated axes to arrive at their destination together–Phew!

      I suspect your F800 is being taken as 800 degrees/minute rather than 800 IPM in this case. Otherwise, a much smaller value would let them meet up at 80 IPM.

      • So given that even though machine is set to ipm mode, when you have simultaneous X and A commanded motions the machine overrides into degrees/minute mode.
        That is reasonable, however one still needs to put a value in the F[WORD]
        Depending on the geometry of the part ( thinking pitch of feed screws here ) the effective feed rate is unknown ( with out some serious calculations beyond the realm of a practical machinist ).
        As such I would assume that one must fall back to primitive methods of setting the feed.
        To quote a worker I observed the other day who was cutting a feed screw for a cherry sorting machine when I asked him what he thought the tool was feeding at he said, ” I do not know, but it sounds good!” ;)

  • [...] CNC 4th Axis Basics: What They Can Do [...]

  • [...] CNC 4th Axis Basics: What They Can Do [...]

  • [...] CNC 4th Axis Basics: What They Can Do [...]

  • [...] is the second installment of a series on 4th Axis Milling.  The first talked about why you’d use a 4th Axis.  In this post, I want to talk a little bit about the mechanics of how they work and what’s [...]

  • manual programing a 4th axis cut requires using G93 feed. G93 sets the machine into inverse time feed mode, 1 divided by the time it should take for the machine to make the cut (in minutes). if the machine is still in G94 mode (default) bad things will happen since the actual feed rate will likely be very high.

Leave a comment

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 © 2010-2014, CNCCookbook, Inc.