G-Wizard's feed and speed
calculator is designed to help you determine the best feeds and speeds
for particular machining operations. Getting the best feed and speed for your particular tooling and cutting situation is one of the most important steps to ensure maximum material removal rates, best surface finishes, and better tool life. The Feeds and Speeds calculator considers many additional variables that simple lookup tables and the SFM and chipload math every machinist knows by heart don't. Considerations such as radial chip thinning, and when it's better to climb versus conventional mill are very important to getting the best results.
If you're wondering why you'd care about all that, here is a quick course in Feeds and Speeds that fills in the blanks:
It's a 10 minute video that covers things like chip thinning, relationship of cutter edge radius to chip thickness for best tool life, ballnose cutter compensation, and a number of other topics associated with feed and speed calculation. And, in the spirit that a picture is worth 1000 words, here is an in-depth demonstration of the G-Wizard Feed and Speed Calculator:
To use the Feed and Speed calculator is simple. Just start filling in the form from left to right, top to bottom and your answer comes out at the bottom:
First, you select
your machine, the material, and the tool.
You can set up each machine in your shop with information such
as the type of machine, machine's rpm limit, maximum feedrate, horsepower
of the spindle, and even what tooling is set up with the machine in the Tool Crib. If you haven't already done so, it's worth your time to set up the basic machine parameters using the Setup tab. This will ensure the G-Wizard Feeds and Speeds Calculator doesn't suggest a spindle speed or feedrate that are faster than your machine can handle, or a cut that takes more horsepower than your machine has available. Save creating a custom Tool Crib for later, after you're familiar with the basics of G-Wizard.
The next choice
is the type of material you will be cutting. G-Wizard supports the following
aluminum alloys, Hardness of 50-150 BHN. 1000, 1100, 1200, 1300 series.
2011 through 2024 series. 300 series. High-silicon aluminum: 4000,
5000, 6000, and 7000 series.
malleable cast irons, Hardness 140-260 BHN: Nodular/ductile, ferritic/pearlitic,
and pearlitic martenistic.
irons, Hardness 135-340 BHN.
Composite: Fiberglass/PC Board
Use this for any resin impregnated glass cloth, e.g. fiberglass or PC boards. Won't work for carbon fiber or exotic stuff like Kevlar though!
Harder woods such as Maple, Wenge, African Pedauk, Hickory/Pecan, Purpleheart, Jarrah, Merbau, Santos Mahogany, Mesquite, Brazillian Cherry, Brazillian Ebony
Particle board and similar materials
Softer woods such as Douglas Fir, So. Yellow Pine, Black Cherry, Teak, Black Walnut, Heart Pine, Yellow Birch, Red Oak, American Beech, Ash, White Oak, Australian Cypress
For a more detailed list, consult the product.
There are two ways to enter a material. First is to use the Material list. Second is to use the Material Database, which is accessed via the "More" button next to the Material list. The Material DB brings up a much more detailed list of materials that includes alloy and condition. Here is a typical example after selecting low carbon steel from the Materials list:
Materials Database is organized by Family, Alloy, and Condition...
You can access any family from within the Materials Database with the "Family" pulldown. Pick the alloy you want and its condition. This determines the Hardness that G-Wizard will use to adjust the cutting parameters. If you know the hardness of your material, all you need is the correct family and enter your own hardness.
When in doubt about which material to select (because you don't see your particular alloy on the list), choose one from the same family and similar hardness. By family, I mean Aluminum, Cast Iron, Stainless, Steel, etc. Use the Hardness conversion table in the Quick Reference if your hardness units are different than the BHN units listed above. While the match is not exact, most tooling manufacturers make recommendations exactly this way and don't list recommendations for the thousands of different possible alloys that are out there. G-Wizard lists the hardness range for the current material right under the material selection menu.
If you don't make a choice from the Materials DB, G-Wizard will assume an alloy and condition that falls in the middle of the range. This works most of the time and there is enough conservatism built into GW that you're unlikely to damage a tool unless you're working on very hard material. The purpose of the Materials DB is twofold. First, it is to help you in identifying the material more precisely. Maybe you're not sure which family to choose, but if you can find it on the list, then you know. Second, it provides a little fine tuning of the surface speed which may increase your performance if the material is softer than the average or decrease and thereby increase tool life if the material is harder.
If you're working with a material that isn't on the list, send us an email or bring it up on the User's Club. We'll be happy to add your material.
The last choice
on the top row is the type of tool you will be using. The G-Wizard Feed and Speed Calculator supports
the following tooling:
HSS Spot Drill
HP HSS Endmill
denotes a higher performance version. Perhaps it has a coating, or
for HSS, maybe it uses a Cobalt alloy. A high helix endmill is an
HP HSS Twist
End / Facemill
Both indexable endmills and facemills use this category.
So you can
find the proper SFM and feedrate when tapping. BTW, check out Field Operators so you can do math in the lead field to convert TPI.
If you have set up your Tool Crib to reflect the tools you have on hand (or are in your toolchanger), you can click the crib checkbox and the menu will show the entries from the current Tool Crib. Note that when you select from the Tool Crib, the Tool Size and Shape Options will be greyed out. You can see what they are for the selected tool, but to change them you will have to go to the Tool Crib.
Tool Size and Shape Options
Depending on which
tool type you select, the remaining options may change. For example, if
you select one of the Twist Drills, you will be given the option of specifying
Parabolic flutes, which are useful for deep holes. You do not need to
specify how many flutes your Twist Drill has because G-Wizard assumes
they're always 2 flute. If you select an Endmill, you will have options
for Ballnose Cutters. If you select an Indexable End / Facemill, you have
the added option of specifying a lead angle, for example for a 45 degree
The first row
below the tool specification asks for (depending on tool type):
diameter and number of flutes.
- The drill chart
will let you enter a standard twist drill size for the cutter diameter.
- The Ballnose
Cutter checkbox does compensation for Ballnose cutters. Activating the
Ballnose Cutter checkbox will reveal more information about your ballnosed
cutter at the bottom of the Feeds and Speeds calculator. Speeds and feeds
differ because depth of cut changes the effective diameter of the cutter
on a ballnose.
- The Rougher
checkbox tells G-Wizard you have a "Corncob" rougher. These
are endmills that have a serrated edge. They can take a higher chipload
because they chop up the chips and make them a lot smaller.
- The Lead Angle
on Face Mills is the angle of the shoulder that would be cut. A straight
square shoulder is a 90 degree lead angle. Lead Angle also affects your
speeds and fees. You can feed a 45 degree Lead Angle cutter faster than
a 90 degree, and it will generally produce a nicer surface finish.
- Twist Drills
have a "Parabolic" checkbox that specifies whether the drill
has parabolic flutes.
- Taps have a "Carbide" and "Form Tap" checkbox that lets you specifies those options so you can get feeds and speeds for carbide taps and thread forming taps (form taps).
Now you've fully
specified what sort of cutter you're using, and it is time to specify
the cut. Parameters relating to the cut appear on the next row down:
- Enter the cut
depth and the cut width.
- Cut Width and
Cut Depth are also expressed as a percentage of tool diameter: Axial Engagement
is lengthwise along the cutter. Radial Engagement is hole diameter or
If you're wondering how to choose the best Cut Width and Cut Depth, welcome to the party. Many machinists are brought up on rules of thumb, trial and error, and what has worked in the past. G-Wizard introduces the Cut Optimizer to help calculate more optimal depths and widths of cut based on an analysis of tool deflection. It's possible to get much more scientific about your choice of width and depth of cut, and hence way better at choosing. But hold that thought. We're going to describe the Cut Optimizer on its own page.
Check out the Cut Optimizer after you've read through the basics of the Feeds and Speeds calculator.
The "Gas Pedal"
The Gas Pedal gives you finer control over what you want to accomplish with a cut:
The Gas Pedal is at the bottom, outlined in red...
The Gas Pedal is calibrated from Conservative to Aggressive in 4 steps. The conservative end emphasizes Tool Life and Surface Finish. The aggressive end emphasizes Material Removal Rates. The Gas Pedal always comes up in position "3", 1 notch below most aggressive, because that's how G-Wizard was calibrated before the Gas Pedal was introduced.
If you're a beginner, crank the Gas Pedal over to the conservative side until you're comfortable you've come up to speed. You might consider coming up a notch at a time.
If you're experienced, use the Gas Pedal to emphasize the difference between roughing and finishing. Or, to give a job a little more safety margin. For example, if you're down to your last cutter of a certain size and the job has to get done that day, be a little more conservative. If you want to emphasize a finer surface finish, be a little more conservative. If you are working on a job that's been going on for 2 weeks and would be expensive to start over on, be a little more conservative.
Feeds and Speeds
This is what its all about: G-Wizard has calculated your feeds and speeds by telling you the RPM and Feedrate you should be using.
Advanced Cutting Parameters
There is a lot more information available to help you understand what's going on and potentially fine tune further. You get the additional information by pressing the "Advanced" button. Most of the time, you have everything you need already, so all that extra stuff is hidden so it won't be distracting.
Note that if you are hitting the limits of your machine in some way, the Feedrate or RPM will change colors. Clicking the Advanced button will lead you to the reason because the appropriate parameters under Advanced will also change color.
Advanced Cutting Parameters
After pressing the Advanced button, you can read
off a number of additional parameters about your cut as shown in the screen shot. Any of the indicators
that have that little padlock to the right are ones you have overridden
from the recommended settings. Be sure to take a look at G-Wizard's recommendations before you try to override anything! To make the Advanced Cutting Parameters go away, just press the "Simplify" button, which is in the same place the "Advanced" button was before.
Machine Limits Column
The first column
in this section is related to your machine limits. They're set up based on which machine you have selected. You can override them here, or you can set up a machine profile in the Setup Tab that matches your machine. Here is what you'll find in this column:
- HP Limit: The
maximum number of horsepower for your spindle motor. Note that not all
spindles can make their full horsepower at all rpms even though G-Wizard
assumes they will! When a cut is specified that would exceed the HP Limit,
G-Wizard scales back the feedrate until the operation is within the HP
- RPM Limit: That
maximum RPM your spindle is limited to.
- Spindle %: The percentage of the available rpm you are using.
- Feed Limit:
The maximum feedrate your machine can manage.
- Feed %: The percentage of the available feedrate you are using.
Keep in mind, not all machines can offer their full HP over the entire RPM range. You may need to be conservative about approaching your machine's HP limit. I "derate" my HP by specifying a little less in the machine profile. Also, some machines become less accurate at higher feedrates, and should only use the higher feedrates for rapids. So you may want to derate the feedrate as well.
Cutting Parameters Column
The second column
in this section is related to a deeper analysis of the cutting parameters:
- Surface Speed
(SFM or SMM in Metric): This is a measure of how fast the tool is moving
relative to the material being cut. SFM is "Surface Feet per Minute"
and "SMM is Surface Meters per Minute". If the tool were a wheel
rolling along the workpiece, that's how fast it would be rolling. SFM
is largely what determines tool life. If you exceed the recommended SFM,
you will wear out the tool much faster. If you run more slowly than recommended
SFM, you may extend the tool life.
- IPT: Inches
Per Tooth, also called Chipload. For metric, this is mm per tooth. To
maximize tool life, cut as close to the recommended chipload as possible
without going over. Exceeding the chipload will eventually break the tool.
Excessive SFM burns or wears out the tool, excessive chipload breaks the
- IPR: Inches
per revolution, or mm per revolution for metric. During the time it takes
for the spindle to make one revolution, this how far the workpiece must
move relative to the spindle to maintain the chipload given the number
of cutting flutes on the tool.
- Chip Thinning
and AFPT: That business of "Chip Thinning" and "AFPT"
on the mill cutter screens is a High Speed Machining concept, but it matters
no matter what speed you are machining at. When you use less than half
of the total cutter diameter for your radial engagement, it turns out
you're not cutting full chip thickness. Hence the chip is "thinned".
The idea behind these settings is to bump up the feed rate until you're
cutting full thickness chips again. Use the "Chip Thinning"
checkbox to turn this on and off. "AFPT" is the actual chip
thickness if you weren't using a chip thinning feedrate. Remember, cutting
a chip that is too thin will prematurely wear your cutter. Try to approach
the recommended chiploads by bumping up your feed. Chip
Thinning and AFPT also come into play if you are using a high lead angle
cutter. Similar geometric effects make the high lead angle (I don't know
why 45 is a "high" lead angle and 90 is not!) cutters require
more feed to maintain the recommended chipload.
Material Removal Rates and HP Column
Once the feeds
and speeds are determined, G-Wizard can estimate you material removal
rate (MRR) in cubic inches per minute (cubic mm/min for metric), how much
horsepower will be required, what % of your available maximum feedrate
and spindle speed are being used, and the recommended plunge rate for
A lot of machinists
focus on maximizing MRR as a way of running their machines for optimal
to think about: not all machines are equal in rigidity. Not even all setups
are equal. HP is a pretty good indicator of how much energy is being transferred
into the workpiece from a cutting operation. Since every action has an
equal and opposite reaction, that force is transferred back into the machine,
and the machine's rigidity has to fight to hold it in check. HP can be
a useful way to tell how stressful a cut is going to be. When you get
a feel for how many HP your machine can successfully transfer into a cut
for certain operations, you may want to use the HP Limit to scale back
a cut so that it is more in line with your machine's comfort zone.
And speaking of rigidity, you can see the predicted tool deflection for your cut (only for endmills and indexables) as well.
Time Estimator Column
The Time Estimator
attempts to determine how long it will take to complete the machining
operation. It needs a few extra parameters:
- Pass Length:
Pass length in inches or mm (for metric).
- XY Clearance:
Use this parameter to specify the distance the cutter must move while
not cutting, for example, to position for the next pass.
- Passes: The
number of passes that will be made.
In exchange, it
will estimate how many minutes per pass are needed and how long the total
specified number of passes will take.
"HSM" refers to "High Speed Machining", a collection of modern techniques designed to wring maximum performance out of CNC machine tools.
The HSM section provides several tools for dealing with the effects of Tool Engagement Angles (also called Cutter Engagement Angles). The TEA provides a means of measuring how hard a cut is working the cutter. Think of it as the angle of the cutter that is actually engaged in cutting. For example, when slotting, a full 180 degrees is engaged. This is the maximum, except during plunging, when a full 360 degrees may engage. TEA changes as a function of corners the cutter may be forced to negotiate in a complex toolpath for CNC. If you don't use CNC, the TEA functions are probably not important to your work.
This portion of the G-Wizard Calculator enables you to do the following:
- Calculate the straightline TEA based on tool diameter and cut width. To do so, just press the "Const. TEA" button and you'll see it come up. For example, a 1/2" endmill cutting 0.015" width of cut has a TEA of 19 degrees--much less than the 180 degrees when full slotting!
- Estimate the TEA of a toolpath based on tool diameter, cut width, and the sharpest angled corner in the path. To bring up the TEA Estimator, press the "Est. TEA" button. Here is our 1/2" endmill, 0.015" cut width example with a 90 degree corner:
Estimating the TEA of a 1/2" EM with a 0.015" width of cut in a 90 degree corner...
When estimating TEA's, you're stuck using the worst case corner since you presumably have a conventional toolpath and not a constant TEA toolpath. You'll be surprised at how much corners increase your TEA. The example cut went from a paltry 19 degrees all the way to 109 degrees in a 90 degree corner, for example. The estimator will show you a scale drawing of the cutter and the corner to help visualize what's happening.
- Estimate how much you'd need to slow down in a 90 degree corner versus "straight line" performance. Any machinist has seen cases where corners cause problems with chatter or perhaps even breaking or chipping a corner. The "Corner Adjust" number tells you how much slower you'd have to go through a 90 degree corner versus straightline with a given tool diameter and cut width. To determine the slowdown, press "Const. TEA" first so you have a straightline TEA, and then look at the "Corner Adjust". For our example, we'd have to slow a path optimized for straight line to just 17% of the MRR of the straight line path.
- Calculate how much faster a constant engagement angle toolpath (HSM) can run than a "standard" toolpath. Calculate the standard feeds and speeds as you always would, press "Const. TEA", and read off the "HSM Adjust". Like "Corner Adjust", this is an increase in MRR. Press the "Show HSM Feeds and Speeds" checkbox to update RPM and IPM accordingly. Our light TEA angle example (1/2" EM, 0.015" cut width) goes from a speed of 3805 rpm and 76.5 IPM to a blistering 6946 rpm and 382 IPM with an HSM toolpath because the MRR went up 500% Now you know why they can charge more for that feature in a CAM program!
The "RPM Factor" and "Feedrate Factor" tell you how much you're exceeding the non-HSM toolpath spindle speed and feedrates, respectively. For example, "1.19" means you're going 1.19 times faster.
People are always passing along tips: "Use a parabolic drill if your length to hole diameter ratio is more than X." G-Wizard has a lot of tips too, and it presents them in the Tips are near the bottom of the screen so you don't have to try to remember them. These tips include the following:
Hole Too Deep: Not Recommended!
The length to diameter ratio is too great. Drilling a hole that deep in that diameter is not recommended.
Use a parabolic flute drill for best results. Parabolics are more effective at chip evacuation in deep holes.
Use Peck Drilling
The hole is deep enough to benefit from peck drilling.
Drill a pilot hole 2xD deep
On some deep holes, it is advantageous to drill a pilot hole that is 2xD deep. The pilot should be a slightly smaller diameter than the main hole. The pilot is important because the long shank needed for the deep hole makes the tool less rigid. The pilot ensures it gets started properly and is supported by the hole with reduced cutting force before it has to really dig in.
Use Conventional Milling
Some cutting conditions result in negative rake geometry when climb milling. When this happens use Conventional Milling.
Use Climb Milling
If your machine is capable of it, climb milling will produce a better finish. Make sure your machine has no backlash before attempting climb milling.
Avoid the centerline of your cutter by using more or less cut width
Centerline cutting is hard on the cutter and hard on the workpiece. You'll get a better result if you use either more or less cut width.
Ballnose Compensation and Surface Finish
The feeds and
speeds calculator also does calculations for ballnosed cutters. These
cutters are unique because their diameter depends on how far down the
ball you are cutting, which complicates the feed and speed calculation.
Simply click the "Ballnose Cutter" checkbox to turn on ballnose
compensation. It's located next to where you enter the number of flutes
and only appears for tool types that could be ball nosed. Turning on this
option will display some additional values near the bottom of the calculator
that tell you the effective diameter of the tool for a given depth of
cut and that also let you calculate what stepover to use to get a certain
scallop height. When 3D profiling, the scallop height gives you some idea
of the smoothness of the surface. Note that this calculation assumes a
flat surface. You may be profiling a wall at an angle, which will result
in a different value. I need to set the calculator up to deal with that,
but haven't gotten around to it yet. The computation simply involves multiplying
the values given by the cosine of the angle of the material. Of course
the cosine of 0 degrees is "1", hence this calculation is right
for flat horizontal surfaces.
Ballnose information appears below the RPM and Feedrate when the "Ballnose Cutter" choice is checked. It provides the effective diameter based on depth of cut and for a given scallop height will tell you the RA/RMS Surface Finish and required stepover...
G-Wizard's feeds and speeds
calculator has a set of functions called "Mini-Calcs" that are little popup feeds and speeds calculators for special situations:
- Surface Finish: Turning surface finish
- Interpolate: Circular and Helical Interpolation of holes and bosses
- Ramp: Feeds and Speeds for ramping into a cut
- Plunge: Plunge Roughing speeds and feeds
The Mini-Calcs are accessed directly under the Tool Definition (where you specify tool diameter, flutes, and so on). For more information, see the Mini-Calcs Doc Page.
Locking and Overrides
Many of the parameters
sometimes have a little padlock next to them, for example there is one
next to the Surface Speed parameter. The padlock only appears when the
parameter has been overridden by the user. Let's say G-Wizard is recommending
400 SFM for your Surface Speed, and you think that's too fast. You can
simply type "200" into that field and override the recommendation.
Once you've overridden, the field stays overridden until you click the
padlock, press the "Reset to Defaults" button (which resets
all padlocks), or restart G-Wizard.
Note that there
are some good reasons not to leave parameters locked for very long. Many
of them interact with one another. For example, let's say you want to
look at the MRR and HP for various sized cutters. You decide to override
SFM because you prefer a lower value. However, G-Wizard tweaks SFM depending
on cut depth and cut width relative to cutter diameter. So as you're playing
with larger and smaller endmill diameters, you're missing out on that
Using the Cut Knowledge Base
The Cut Knowledge Base (Cut KB) is a powerful feature normally only found in high end CAM packages where it is often referred to under the heading of "knowledge based programming". The idea behind the Cut KB is to facilitate the gathering and organization of your shop's best practices around cutting to create a Knowledge Base (similar to a database) that captures that experience.
is the tendency for the chips to get thinner when you cut less than half
the cutter's diameter depth of cut at a particular feedrate (more detail on my chip thinning page).
Consider a cutter
that is 1/2" in diameter edge milling a 1/4" deep depth of cut.
Further, let's say it is spinning at 2700 rpm at a recommended feedrate
of 16 IPM. So, for 1/2 of a revolution, a tooth is engaged in the cut.
That 1/2 revolution takes 0.000185 minutes. During that time, the 16 IPM
feedrate moves the cutter 0.003", which is the recommended chipload
for the cutter.
Now let's try
less depth of cut. Instead of 1/4" deep, let's go 1/8" deep,
half as much cut. We can use the chord calculator in G-Wizard to see how
much engagement we have. The arc length is 0.5236", and the overall
circumference of the cutter is 1.5708", so we are engaging only 1/3
of the total circumference instead of the 1/2 with the deeper cut. So
the cutter now has even less time to peel of a chip, hence it has a lower
chipload. The actual chipload is now than what it should be. Hence, we
can speed up the feedrate quite a bit to restore the recommended chipload.
G-Wizards's "AFPT" is the "Adjusted Feed Per Tooth",
and it is the chipload at this faster feedrate.
Note that G-Wizard's
Chip Thinning compensation is radial chip thinning. Axial chip thinning
is also possible, but is based on the cutter's profile being something
other than vertical. For example, button cutters are like face mills that
have round inserts. The ballnosed cutter compensation compensates for
the round profile of a ballnosed cutter, but assumes a semicircle rather
than the radius of a button cutter. Certain insert types (high feed inserts)
also use this kind of geometry to allow extremely high feedrates.
The danger when running light cuts and feeds and speeds that don't take chip thinning into account is that your cutter will "rub", which drastically reduces tool life!
for Parabolic Drills and Some New G-Wizard Functionality
It is always hard to drill
deep holes, where deep is defined by a hole that is many diameters of
the drill bit deep. I recently came across a
question on CNCZone that started me doing some research on the topic
of parabolic drills. Parabolic-style drills were developed in the early
1980s. They use a heavier web to create higher rigidity and increased
flute area for chip removal on deep-hole drilling operations.
Precision Twist Drill has a
nice discussion on their site of how to vary feeds and speeds to accomodate
deep holes when using regular and parabolic twist drills. I was so taken
by the CNCZoner's question and that nice discussion that I wound up adding
a bunch of functionality to my G-Wizard Machinist's
The new functionality is both
to implement the feeds and speeds adjustments recommended by Precision
Twist for deep holes, but also to give recommendations based on the hole
depth. For example, it suggests when you need to use a peck drilling cycle
(where you drill down a little ways and then retract to clear chips) as
well as when you should be considering a parabolic bit instead of a regular
The question the CNCZoner raised
was what feeds and speeds to use when drilling a 0.201" hole 3.5"
deep. That's over 17x the diameter in depth, so a parabolic drill is definitely
Here is what G-Wizard shows
when you enter those parameters:
Note the box for
Parabolic is checked, which tells G-Wizard we want to use a parabolic
drill. Also, it is recommending a peck drilling cycle (DUH!) for this
17.412x Diameter hole depth. If we enter a less severe hole depth, 0.2",
it recommends 3800 rpm and a feed of 16.85, whereas you can see from the
diagram it has compensated for hole depth and slowed down both the feeds
and speeds. The feed is slowed as a result of the spindle rpm. Parabolics
don't need further slowing. A regular twist drill would also get feedrate
reduction on top of that.
When to Climb Versus Conventional Mill
Many CNC'ers are
brought up on the notion that you should always Climb mill because it
leaves a better surface finish, requires less energy, and is less likely
to deflect the cutter. Conversely, manual machinists are often taught
never to climb mill because it's dangerous to do on a machine that has
backlash. The truth is somewhere in the middle. ABTools, makers of the
popular AlumaHog and ShearHog cutters, point out some
worthwhile rules of thumb:
- One cutting
half the cutter diameter or less, you should definitely climb mill (assuming
your machine has low or no backlash and it is safe to do so!).
- Up to 3/4 of
the cutter diameter, it doesn't matter which way you cut.
- When cutting
from 3/4 to 1x the cutter diameter, you should prefer conventional milling.
The reason is
that cutter geometry forces the equivalent of negative rake cutting for
those heavy 3/4 to 1x diameter cuts. It seems that Dapra corporation first
discussed this phenomenon way back in 1971. G-Wizard now reminds you with
a little hint which one you should prefer:
Just to the
right of Radial Engagement it says, "Use Climb Milling"...
If you choose
to climb mill, do make sure your machine is up to it from the standpoint
of having low or no backlash, lest your cutter dig in and suddenly jump
very deeply into the cut due to the backlash.
Exploring Ramping and Interpolated Holes with G-Wizard's New Mini-Calcs
I've just finished adding a new feature to the G-Wizard Calculator that I call "Mini-Calcs" for release 1.040. Mini-Calcs are little popup feeds and speeds calculators for special situations. We already had one popup for calculating ballnose cutter stepover to achieve a particular surface finish. I've just added two more--one is all about interpolated holes and the other is about ramping. Both are common CNC operations that may be used to get a cutter down into a pocket or in the case of interpolation, this is an effective way to use an endmill to create a hole of a particular size. There are a lot of trade-offs around making holes with interpolation, but more on those in a moment.
The Mini-Calcs are accessed directly under the Tool Definition (where you specify tool diameter, flutes, and so on):
The three Mini-Calc buttons are right under where you specify Tool Diameter and Flutes...
Let's start with the Ramping Mini-Calc. From the screen shot above you can see I've set up an aggressive machining scenario in 6061 aluminum. I've got a 1/2" 3-flute TiAlN Endmill selected and it's a serrated "corncob" rougher to boot. I want to set up my CAM program to cut a pocket on a part, and I've decided my entry to the pocket will be via ramp. I'll show how to use the Ramp Mini-Calc to solve a couple of interesting problems.
First, let's say I just plan to ramp down at some "standard" rate, say a 3 degree angle. What should my feeds and speeds be on that ramp? You should adjust your feeds and speeds slightly when ramping because its harder than making a level cut. Let's say we'll be cutting our pocket at a 1/2" depth. Set up for a full slot cut, because the ramp will be descending into bare metal. Let's also set the depth of cut to be the maximum depth of the ramp in one pass. If we need to go deeper to get down to full cut depth, the ramp will zig zag back and forth. I'll use a 1/2" depth of cut at full ramp. Here is the Ramp Mini-Calc with all that keyed in:
Ramping the Cut Down 3 Degrees...
As you can see, with a 3 degree ramp, the adjustment in feedrate is pretty minor, from 108.6'ish IPM down to 106. No biggie, in fact we could probably just choose to ignore it unless we're running a really max'ed out feedrate we've determined through trial and error to be right at the ragged edge.
What if we want to see what angle is needed to get all the way down the ramp in say 2" of travel? No problem. Set your depth of cut as before to the bottom of the ramp, bring up the Ramp Mini-Calc and press "From Cut Depth". You'll see a new control appear that wants to know the travel length. We're trying to get there in 2", so fill that in:
You need a 14 degree angle to ramp down 1/2" in a 2" pass...
The Ramping Mini-Calc figures the ramp angle at 14 degrees. This is more aggressive than the 3 degrees we had earlier, so we have to cut our feedrate from 108.6 IPM down to about 97 IPM. That's starting to be worth worrying about in the CAM program. You can just click "Adjust Feedrate" and the Mini-Calc will override G-Wizard's default calculated feedrate based on the new information on ramp angle.
This is a probably a good time to mention the warning you see there. Not all cutters can tolerate arbitrary ramp angles. For example, let's say we had a 90 degree ramp angle. That would be a straight plunge. Obviously if you don't have a center-cutting endmill, that's a no-no!
Insertable tooling will have a ramp angle limitation that you can find in the manufacturer's catalog. It's often pretty limiting, so be sure you don't find out the hard way you have exceeded it!
What about the Interpolation Mini-Calc? Let's check it out:
Suppose you want to use the same basic setup to interpolate a 2" hole. Click on the Interpolate Mini-Calc and here's what you'll see:
The Helical and Circular Interpolation Mini-Calc...
There's quite a bit more going on here as you can see. First, you'll need to specify whether you're machining a hole or a boss. This determines whether the endmill is going around an ID or an OD diameter. In addition, the checkbox tells whether Tool Comp is in use, in which case the toolpath is the cutting edge rather than center of tool. We also need to tell whether we will be doing a Helical Interpolation (going down the hole in a spiral) or a Circular Interpolation (just machine from center out without changing the Z depth). Lastly, we enter our Feature Diameter, which we said would be a 2" hole.
Now the Mini-Calc displays a series of intermediate results:
- The raw unadjusted feedrate coming in from G-Wizard is 108.6 IPM again.
- Since we're doing a Helical Interpolation, there is a ramp angle. We figured it out from the Cut Depth parameter. You could also have used the ramp calculator to go from degrees to cut depth.
- We need to adjust for the geometry of both the ramp and the fact that unless we have tool comp on, our feedrate is based on a radius that is either larger (boss) or smaller (hole) than our feature. As we can see, the geometry adjust feedrate is signicantly different in this case, coming in at 77.8 IPM.
What's all this business of acceleration? Thought you'd never ask!
Not long ago I was chatting with a moldmaker about the pros and cons of interpolation versus a honking indexable drill to open up a hole before pocketing. He wasn't having any of it because he needed a bunch of hole sizes in his molds and he needed them to be done accurately via interpolation. And, he wanted G-Wizard to do the interpolation calculations, and BTW, the feedrates it was giving him were too fast for his machine to interpolate accurately (I related the story in more detail in a prior blog post). After thinking about the issue for quite some while, I finally realized the answer to the accuracy issue was in figuring out the acceleration required for the op and making sure it was within the machine's capabilities.
As you can see, the operation depicted by the screen shot requires 0.03 g's of acceleration, which is 4034.5 inches per minute per minute. That's not very challenging for most machines. A high-end machine purpose-built for HSM with linear servos may be able to do 5 g's of acceleration. The vast majority of machines are only capable of a tiny fraction of that kind of performance. You can check your manufacturer's specifications, but I have more bad news--the exact acceleration capabilities can vary fairly significantly from one machine to the next, particularly if they're not right off the assembly line.
The thing to do if you want to be able to interpolate holes and other features accurately is to measure your machine's capability in this regard. Mastercam has a document out that walks through how to go about this with their software. Or, you can use G-Wizard's Interpolation Mini-Calc to figure it out. Here's how:
1. Pick a test diameter. Smaller is better because its easier to generate higher accelerations going round and round real fast in a little hole!
2. Set up the Interpolation Mini-Calc for circular interpolation on your small hole.
3. Now go run tests on your machine until you've figured out the fastest feedrate that interpolates that hole accurately. Plug that feedrate into the Mini-Calc and it'll tell you how many g's that was. Write that down! Eventually I will add a field to the Machine Profiles in G-Wizard so it'll remember it for future interpolation calculations.
Just as an example, let's say we machine 1/2" bosses with a 1/4" EM. I like bosses for these tests because we can get a micrometer on one to accurately measure it. Holes are more trouble. Given a Cut Depth of 0.2" and a 15% of diameter Cut Width for that boss, G-Wizard has us going round and round at 178 IPM on our 7500 rpm limited spindle. That gives us an acceleration of 0.3 g's. Believe it or not, that's probably heading into the pain threshold for an older VMC that doesn't have the swiftest rapids in the Wild West. So let's say we wind up having to slow it down to 120 IPM before we hit our tolerances. With just a little fiddling in G-Wizard around the Interpolation Calculator, we discover that means our limit is 0.15 g's.
If you're just hogging a hole to get a pocket started, don't sweat the acceleration limits. There is a checkbox to turn the feature off.
Incidentally, going around a corner on a toolpath will be subject to the same kinds of acceleration limits. You'll want to map these limits out for a couple of hole sizes to see how stable they are for your machine. Keep careful notes, they'll come in handy when you're trying to dial in that high dollar job.
Okay. You've now seen how we can use the Ramping and Interpolation Mini-Calcs in G-Wizard to solve some interesting machining problems. Go forth, be fruitful, and make some chips!