G-Wizard User Guide

Calculator

Feeds and Speeds

Cut Optimizer

Geometry

Threads

Quick Reference

Setup

Tips and Goodies

Troubleshooting

User's Club

G-Wizard Change Log

G-Wizard Install

GWizardE Peek!

G-Wizard Machinist's Calculator: Feeds and Speeds

G-Wizard's feeds and speeds calculator is designed to help you determine the best feeds and speeds for particular machining operations. To use the Feeds and Speeds calculator, simply start filling in the form from left to right, top to bottom:

Machine

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, iIt's worth your time to set up the basic machine parameters using the Setup tab. This will ensure G-Wizard 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 the Tool Crib for later.

Material

The next choice is the type of material you will be cutting. G-Wizard supports the following materials:

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.

Tool

The last choice on the top row is the type of tool you will be using. G-Wizard supports the following tooling:

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 facemill.

The first row below the tool specification asks for (depending on tool type):

- Cutter 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.

Cut Specifications

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 slot width.

Optimizer

Hold that thought. We're going to describe the Cut Optimizer on its own page. For now, just ignore it until you get the basics down!

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.

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 Limit specified.

- 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 tool.

- 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 endmills.

A lot of machinists focus on maximizing MRR as a way of running their machines for optimal productivity.

Something else 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.

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.

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...

Lathe Surface Finish

For turning operations, you can pop up a surface finish box to determine feedrates based on desired surface finish given a particular cutter nose radius.

Parameter 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 tweaking.

What is Chip Thinning?

Chip thinning 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 Case 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 Calculator.

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 twist drill.

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 called for!

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.