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

Toolpath Secret Weapon: Complete Guide to Plunge Roughing / Milling

Oct 5, 2016   //   by Bob Warfield   //   Blog, FeedsSpeeds, Software, Techniques  //  5 Comments

Have you got a tough job ahead, either because your machine is too lightweight or because of challenging geometry on the part (deep pockets, for example)?

If so, maybe Plunge Roughing (also called Plunge Milling ) is the answer.

What is Plunge Roughing?

Let’s start by taking a look at what Plunge Roughing is.  The idea, is to rough out a pocket, profile, or 3D surface by plunging either a twist drill, an endmill, or a special-purpose tool straight down into the material.  Here’s a typical example:

Plunge Roughing Milling a Pocket

Plunge Roughing a Pocket – Image courtesy of BobCAD

The graphic shows a typical plunge roughing operation for a square pocket, courtesy of BobCAD.  As you can see, a chain of holes are plunged vertically with the tool to rough out most of the pocket area.  A subsequent finish pass will complete the pocket.

What are Plunge Roughing’s Advantages?

I called Plunge Roughing a “Secret Weapon” above because it can really save your bacon in some situations.  It is designed to take advantage of two important properties:

  • Twist drills often have much higher material removal rates than endmills.
  • Most CNC Machines have Z as their stiffest axis.  By changing forces from side forces (XY plane) to axial (Z) up and down forces, we get much more rigid cutting.

Taken together, it’s pretty easy to see where Plunge Roughing could turn into your Secret Weapon.

Perhaps you have a relatively lightweight or less rigid machine.  By taking advantage of the greater rigidity your machine will have in the Z direction, you may be able to get higher Material Removal Rates.  Or, you may be able to overcome a chatter problem that’s due to a lack of rigidity.

Older (or cheaper) CNC milling machines that have more slop in the XY axes, less precise interpolation, or slower spindle speeds may also benefit from exercising the Z-axis more via Plunge Roughing.  Plunge Roughing seems tailor-made for the limited rigidity and performance of Hobby CNC machines too, for example.

And speaking of a lack of rigidity, Plunge Roughing can be ideal for those really deep pockets where side forces are causing so much tool deflection you can hardly make progress at all.  Sandvik says Plunge Roughing is advantageous any time overall Tool Stick out is more than 4 x Tool Diameter.

How about a Mill-Turn situation where your live tooling is not nearly as rigid as on a pure milling machine?  Here again, you may find Plunge Roughing is just the ticket.

Plunge Roughing can also be just the ticket when your machine’s spindle power is limited, according to Sandvik.

5 Axis Plunge Roughing Hypermill

Talk about a lack of rigidity–long reach and thin walls make Plunge Roughing a natural for this 5-axis turbine application.  Image courtesy of Hypermill.

How about machining a tall thin wall?  This is a notoriously chatter-prone situation that may be partially amenable to Plunge Roughing.  It’s not a total cure, because you’ll still have to manage a finish pass that removes the scallops, but it might allow higher Material Removal Rates without chatter for the roughing pass.

In fact, consider Plunge Roughing any time chatter becomes a big problem on a job.

One last special case for Plunge Roughing would be corner clearing.  When the depth of the corner is greater than about 4 x the cutter diameter that fits into the corner, rigidity issues develop.

Plunge Roughing can be applied to help maintain rigidity in these difficult cases:

Plunge Roughing Corners

Plunge Roughing Corners.  Image courtesy of Sandvik.

One could imagine doing most of the roughing with an HSM Toolpath and an endmill that is much to large in diameter to get into the corners.  Depending on pocket shape, this can clear most of the material without leaving much scalloping.

As part of the final finish or an intermediate Semi-Finish pass, we use a much smaller diameter endmill to clear the area of the corner and then we can make an overall finish pass of the entire wall of the pocket or profile.

What are the Disadvantages?

Plunge Roughing Scallops

Plunge Milling leaves scalloped edges which may take a fair amount of cleanup or a semi-finishing pass before a true finish pass can be applied.  Image courtesy of Sandvik-Coromant.

  • Scalloped Edges:  Plunge cutting leaves a scalloped edge (see diagram above) that will have to be cleaned up by a finish pass.  Depending on your X and Y stepover amounts, the amount of scallop to be removed could be significant.  If it’s more than a single finish pass can remove, an optional semi-roughing pass will be needed to clean up the scallops before the final finish pass can be applied.
  • Center Cut:  The tool used must either be center cutting (leaves out many types of indexable endmill) or the toolpath must allow for a ramp or helix entry to create enough space to start taking partial plunge cuts.  If the tool isn’t center cutting, it also can’t cut on a down slope where the feature gets deeper in some places.
  • 2D vs 3D Plunge Roughing:  Some Plunge Roughing toolpaths only support 2D features where the floor is at the same Z, while others can do full 3D Profiling via Plunge Roughing.

3D Plunge Roughing

3D Plunge Roughing.  Image courtesy of SprutCAM.

  • Conventional Twist Drills:  The point angle on conventional twist drills makes them wander when plunge roughing if the holes overlap too much.  You also wind up with a scalloped floor, which is less desirable.  This may require flat-bottom tooling such as endmills or twist drills that are specially made for Plunge Roughing.
  • Not the Best Under Favorable Conditions:  Plunge Roughing is not a general-purpose strategy that replaces all other strategies.  It’s best use is when you need Plunge Roughing’s advantages: more rigidity and less power required. If those are not problems you need to solve, then Plunge Roughing is probably less optimal than other Roughing Strategies such as a High Speed Machining (HSM) Toolpath.

What about Plunge Roughing Feeds and Speeds?

Our first task is to decide on the X and Y stepovers.

Sandvik recommends starting with a stepover (Cut Width in G-Wizard) of 80% of cutter diameter for the sideways motion of a single pass.

The stepover to move deeper into the material for the next pass is limited by the insert diameter or the maximum Cut Width of any non-center cutting tool.  80% of that value is a good choice as well.  Keep an eye out so there’s no skinny stalks sticking up in the corners between the holes.  If you see stalks, you need less stepover in one dimension or the other.

Now we need Feeds and Speeds.  Our G-Wizard Feeds and Speeds Calculator has special features to help with Plunge Roughing.

Let’s work through an example that shows the strengths of Plunge Roughing.  Suppose we are handed the task of roughing out a pocket that has 1/8″ corner radii, which dictates and endmill no larger than 1/4″ in diameter.  Next, suppose that pocket is 1 1/2″ deep.

I can already hear the groans out there in the audience–a pocket that deep with such a small endmill is likely to be a bear!

Just to keep things simple, I’m going to choose X and Y stepovers of 0.0625″ for this job. Let’s check Feeds and Speeds with G-Wizard and assume we want to use an HSM roughing strategy like Adaptive Clearing or Volumill:

plungegwiz1

MRR isn’t bad at 3 cubic inches/min, but deflection is way too high…

The MRR isn’t bad at 3 cubic inches/min, but deflection is way too high.  This approach is going to chew up tools very quickly with almost 3 thousandths of deflection.

We can use G-Wizard’s Cut Optimizer to see how much stepover is allowable to keep things within deflection allowances:

plungegwiz2

Cut is almost impossible without too much deflection…

A quick click on the “Cut Width” label has Cut Optimizer taking us all the way down to a Cut Width of only 1.4 thousandths and there’s still a bit too much deflection.  We could probably live with that, but MRR is down to a lousy 1.1 cubic inches a minute.

We’re going to lose our shirts on this job if we don’t find another way.  What about Plunge Roughing?

Click the “Plunge” button to bring up the Plunge Roughing Mini-Calc:

Plunge Roughing Calculator

G-Wizard’s Plunge Roughing Calculator…

G-Wizard’s Plunge Roughing Calculator let’s us enter a Step Up (amount to move into material at start of each pass) and a Step Over (amount to move laterally from prior hole on the same pass) and adjusts the feedrate based on those parameters.

Here is the result:

Plunge Roughing Feeds and Speeds

Here’s a case where Plunge Roughing shines…

Here’s a case where Plunge Roughing shines: our MRR is back in the 3 cubes a minute territory of the original HSM scenario, and while the Deflection error is still red, we can ignore it because we’re plunging and there will be no significant deflection while doing that.

Problem solved!

Which CAM Packages have Plunge Roughing?

Here is a list of the most popular software from our last CAM Package Survey that shows whether each package has Plunge Roughing or not:

camplunge

As far as differences in Plunge Roughing toolpath quality, it’s worth checking on whether your CAM package supports two capabilities.

First, does it do true 3D or just 2D Plunge Roughing?  3D is obviously much more general while 2D will only work for flat-bottomed features.

Second does the plunge cycle retract away from the wall during the overall retract?  This reduces chatter and increases tool life when machining tough materials. Here’s the Plunge Rough retract style jointly developed by WorkNC and Ingersoll:

Plunge Roughing Retract Tool Life

Retracting from the Wall slightly during Plunge Rough…

Retracting from the Wall slightly during each Plunge Rough stroke can improve tool life by 10 to 15 percent, according to the developers of the technique.

What Can I do if my CAM Software won’t Plunge Rough?

Normally if your CAM software doesn’t support a particular kind of toolpath, you’re just out of luck.  But Plunge Roughing may be different, depending on how adventurous you are.  A basic strategy for creating your own Plunge Roughing toolpath works like this:

  1. Use your CAD Software to generate a grid of holes (circles or whatever you like) within the contours of the pocket or other feature’s outline.  Be sure to leave some finish allowance, so you may need to inset the outline by the finish allowance.  Depending on how easy it is to keep the circles entirely within the outline, you may have to inset further to leave enough allowance.  Your CAD software does most of the work, so you’re relying on its sophistication to pull off the creation of the hole grid.  Even if the package is a bit weak in this area, most of them should be able to lay down a grid within a rectangular region or perhaps in a line so you can Plunge Mill a slot.
  2. Given the grid of circles, you create a g-code program to plunge the cutter at each circle’s coordinates.  This can be as simple as taking a canned drilling cycle and feeding it the list of circle coordinates.

There are certainly embellishments.  For example, you could do the fancy wall retract move with a little bit more hand coding.  You may also need to deal with entering the pocket, though you could use just have your CAM package generate its entry and then cut and paste that gcode to create a starting point for your Plunge Roughing routine.

With a little bit of gcode programming familiarity and some decent chops with your CAD software, this is not hard nor does it need to take very long.

Here’s an example I partially worked through in Rhino3D:

  1. Start with the outline of your pocket.  Inset that outline by a finish allowance.  Here is the contour with an inset:

Plunge Rough Hand Programming

The contour of a pocket wall with an inset for a Finish Allowance…

2. Drop a circle of the endmill’s diameter down and make it tangent to somewhere convenient on the inset contour:

cadplunge2

3. Create an array of the circles with the X and Y stepover you want to use:

cadplunge3

I didn’t get the grid quite large enough!

4.  Trim any excess circles that extend too far out-of-bounds:

cadplunge4

5. Adjust remaining circles at the edges so they’re tangent to any inset contour edges they intersect:

cadplunge5

That’s about all there is to it.  You now have a CAD drawing that shows where the holes for the plunge strokes need to go.

Import it into your CAM package and treat just like trying to drill all those holes.  It’ll generate the gcode which you can then further tweak as needed.

I didn’t finish with the CAM part, but the CAD work only took 10 minutes and I didn’t use any shortcuts.  It’s not hard to do if you want to play with Plunge Roughing a bit. Programming something like this to clear a corner or two would be even easier.

I want to know more!

Like I said, Plunge Roughing can be a powerful secret weapon in your CNC arsenal.  We’ve seen its advantages graphically via G-Wizard in the case of a pocket that’s too deep relative to tool diameter.

Take advantage of our free 30-day G-Wizard Trial so you can work on your own scenarios too!

To learn more about Plunge Roughing, try these articles:

Do you use Plunge Roughing?  Tell us your experiences and thoughts on Plunge Roughing in the comments.

 

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

5 Comments

  • I’m using SprutCam 10 and I’m not aware of any Plunge Roughing Operations.

    I’m I missing something?

    • Mark, just click the link by the photo. It leads to the page in the Sprut docs where the photo came from.

  • Drills do not like it when side brake into other hole, End mills have no problem.
    If drilling should leave 1/16 inch web and then use end mill to remove web.

  • I’m trying to figure out by visualizing in my head, why would plunge milling be an improvement over milling in layers on the Z-axis (aka contour milling or topographic milling)? It seems to me, and correct me if I’m wrong, but the time would be about the same, but contour milling would wear down the tip of the bit faster than the rest of the bit and you would still get some deflection along the x and y axes. With plunge milling, the only deflection would be along the Z-axis.

    Also, it seems like plunging is fine for roughing only because of scalloping, but which method do you think would make the smoothest result for the final pass? There’s just so many options! (I’m new to CNCing if you can’t tell).

    • Jason, plunge milling is advantageous only when rigidity is a problem due to either the machine being a bit too lightweight, or the required tool diameter being too small relative to the cut depth. That’s really the point of the article is to spell out when it is a better bet.

      Plunging is only suitable for roughing, and if you’re leaving a reasonable finish allowance, the roughing method shouldn’t affect the quality of the finish from the final pass.

      I suppose it is possible to imagine a situation where the rigidity problems are so challenging that they continue to exist during the finish pass and that the scalloping could potentially make that worse, but in the end, I think it only means there will be multiple finish passes required.

      If rigidity is not an issue, other methods, such as HSM style toolpaths will achieve higher material removal rates and efficiencies.

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.