CNC Router Feeds and Speeds - The Adam's Guide

Feeds and speeds, the deal maker or breaker of CNC machining. I field weekly phone calls from customers asking for advice on the best feeds and speeds. This guide is gives you a head start or to help you adjust your technique.

This guide is divided into three parts:

• Explanation of the Adam’s Bits calculator
• Considerations and Limitations of the calculator
• Frequently asked questions

Where I have not explained enough on a certain value, there is a good chance I will elaborate in the Considerations and Limitations section and FAQs

Let’s start with the Adam’s Bits Feeds and Speeds calculator:

feeds.endmill.com.au

For steel, V bits and other situations not covered by this calculator, check out FSWizard

Start by selecting your material

Choose the material that best represents what you are cutting

The materials listed are not limited to what you can cut but it’s a great start. Do your best to match the type of material. Just remember that balsa wood is regarded as a hardwood but would better be selected as a softwood.

Chip Load %

The material selects the appropriate chip load %.

Don’t get hung up on what the exact value but it’s important to the calculation to the correct feed rate. For example, hardwood has a chip load value of 2% and softwood 4%. That means that you will be able to cut softwood 2x faster than hardwood. Sounds about right!

Diameter of bit

The diameter of the bit is measured at the tip in millimetres.

This calculator can only calculate straight cutters, not V bits or tapered bits. When looking at the label of an Adam’s Bits, it’ll be the first set of numbers.

Select a cutter profile

The cutter profile is defined by the direction of the flute/s of the cutter.

UP cut bits will pull material up and can leave a top edge burr. Down cut will push material down and if cutting through will leave a bottom edge burr. A COMPRESSION bit will have both up cut and down cut components. A straight cut will leave a slight burr to both top and bottom.

Select a coating

Is your bit coated with Diamond like Carbon (DLC) or uncoated?

Diamond Like Carbon (DLC) is the new kid on the block when it comes to coatings. DLC coatings have the characteristics of hardness, lubricity and abrasion resistance which is what you need when it comes to CNC router bits. If there is no coating, choose “uncoated”.

Flutes

The number of cutting edges.

Typically, you’d use a 1 flute for plastics and aluminium (soft metals) and 2 flute for timbers. Remember to choose the correct 1 flute for soft metals. Bits made for soft metals have a different cobalt % and are therefore harder, but not sharper. You can use 1 flute for soft metals on plastics, especially DLC coated that give a great finish and cutter longevity. If you are cutting plastics and soft metal with the same profile bit, use two sets and keep them separate. Any deposit of soft metals on a bit that is later used on plastics will result in a suboptimal finish.

Cut length

The length of the effective flute/cutting edge length.

When looking at the label of an Adam’s Bits, it’ll be the third set of numbers.

Cutter natural length

The length in mm that if you just used chip load % x RPM x diameter fits perfectly

This is a concept that makes the most sense to me but do not get hung up on it. Each bit has its sweet spot in cut length when feed rate = chip load % x RPM x diameter. The natural length is used as the baseline to calculate the final feed rate. In essence, if speed/feed is the key, the shorter the bit the better. For every 5mm longer the natural length, you will have a feed rate reduction of 20% and times -20% for every 5mm. The opposite happens when you use a shorter bit than the natural length. In other words, if you want to push your CNC and achieve a higher production throughput, you'd want the shortest and thickest diameter.

Depth per pass

Depth per pass is how deep your machine cuts down into your material at each pass

There is no real “general rule” on setting depth per pass contrary to many articles and YouTube videos. The only exception is a compression bit where the up-cut component of a compression bit is 1 X D. You will therefore need a depth per pass greater than 1 x D in the first pass as a minimum. Depth per pass does effect the MRR Material Removal Rate which could overload your stepper motors which will be explained later.

Spindle speed (RPMs)

The revolutions of your spindle/trimmer per minute

A good start is to use

• 12,000-16,000 RPM for plastics and timbers
• 18,000 -24,000RPM for soft metals

Lower / Middle / Upper

Feed rate per mm/min

Your results have arrived and before you commit, it is best to sense check the numbers. Play around with your setting with different combinations to match yours and the machines capability. More will be explained in considerations and limitations.

Check your Machine Capability

If your CNC has a feed rate limitation, tinker with the depth per pass value or RPMS to reduce the feed rate below your CNCs maximum. You can use the following calculation addendum to assign your CNCs maximum feed rate and have it calculate the new feed rate.

Your Max Feed Rate

If your feed rate is limited in the calculated result, input your machines max feed rate

New RPM Value

A new RPM value will be calculated that can be used to override the value that you used in the calculation

Considerations and limitations

The calculator does not guarantee your desired results

The calculator strikes a balance between cut quality and bit longevity. Operating at the ideal speed will not necessarily mean that you will get a perfect burr free finish and will not guarantee that your bit will last. There is an inverse relationship between cut quality and longevity, and you will have to determine which you would prefer.

This calculator does not consider your machines maximum MRR Material Removal Rate aka machine rigidity

Calculated as:

• MRR = feed rate x diameter tip x depth per pass

(Example 64cm3/min = 4,000mm/min x 2mm diameter tip x 2mm depth per pass)

The MRR of each CNC will be different and will dictate the maximum diameter, feed rate and overall carve/cut time. It is one of two questions I ask when being asked for recommendations on bits. There is no point on suggesting a 6mm bit for a 3018 CNC, no matter how fast the customer would like to cut their project. 

My rough estimations on the following machines and their capability for softwoods

• Small 3018 style CNCs – 2,000mm/min x 2mm x 2mm = 8cm3/min
• Belt driven – 4,000 x 4 x 4 = 64cm3/min
• Lead screw and linear rails – 6,000 x 6 x 6 = 216cm3/min
• Ball screw driven – 8 x 8 x 8 = 512cm3/min
• Industrial CNC – 12.7 x 12.7 x 12.7 = 2048cm3/min and up

By asking what CNC the customer is using, I can at least place a ceiling to the bit diameter suggested. Encroaching on the machines maximum MRR will result in gantry chatter leading to a suboptimal finish. If they are insistent on using the larger diameter bit, a lower feed rate or depth per cut would lower the MRR. Funny how if you are experiencing chatter that forums suggest lower the feed rate or the depth of cut but they do not suggest using a smaller bit!

The values stated are for softwoods and soft plastics with a value of 1. For hardwood and acrylic x 0.5 and soft metals x 0.1.

For example, a belt driven CNC with an upper limit of 64cm3/min MRR for softwood, would have an upper limit of 32cm3/min for hardwood. You would therefore limit yourself to 3.175mm/min with a 3.175mm diameter bit at 3.175mm depth per cut = 32mm3/min

The calculator does not take into account hold down strength

When you start increasing the MRR, you run the risk of lifting the material you are cutting or potentially ripping the material out of the holds. If you are worried about the integrity of your material hold down method, decrease the MRR e.g. reduce the bit size.

An example of where you would reduce the diameter of your bit would be cutting thin aluminium over a large sheet. Where you have the greatest vacuum is in the centre of the material, gradually dissipating towards the edges. A 6mm cutter would fair well in the centre of the material but when travelling along the edges, the material will pull up the material and inevitably snap the cutter. This would happen regardless of what the size of the vacuum. By reducing the cutter diameter, you will reduce the MRR and there is a lower chance your material will lift.

If the numbers are way higher than you are used to or are uncertain about how your CNC will handle it, just reduce the depth per pass! It’s good to know what your limits are and slowly increasing your depth per pass is one way to do that. Keep the feed rate and RPMs the same as the calculator.

Plunge rates are not calculated

Plunge rate is a bit of a tricky one to determine. Your plunge rate is determined by the rigidity of your spindle and Z axis. You can plunge at 800mm/min for timber and plastic and 400mm/min for aluminium. The smaller the bit, the lower the plunge rate. You do not want to go too slow of a plunge rate with high RPMs.

Where possible and capable, use the ramp in feature to minimise dwell in one spot. In lieu of ramping in, reduce the RPMs especially when cutting multiple holes or parts. This applies especially with compression bits as this will create high friction and burn your bits.

The calculator does not take into account your experience

Another question I ask a customer is what’s their experience in using a CNC router. In my head I have presumed a MRR value, not of the machine but of what the customer has the experience in using. For example, there is no point in suggesting a 12.7mm 3 flute compression bit for a customer new to CNC whose CNC would easily handle the size. The potential for the bit to break, burn or give a suboptimal finish is extremely high due to the shear MRR needed. Having the customer start with instead a 6 or 8mm diameter bit eases the customer into the world of CNC by building their confidence. The chances of breaking or burning the bit is much lower and gives a much better chance of a successful cut. I don’t know of any other bits supplier that does this, and I know of many that do not take the customers experience into account, but I think it’s just good business ethics.

Did you notice that there is no provision for shank diameter? 

That’s done on purpose because a shank diameter does not add strength to your bit. Your bit should be inserted about 3mm above the start of the cutting edge/flute and this is factored into the calculator. Any additional stick out will reduce the calculated feed rate the same way a cut length of 5mm greater than the natural length reduces the feed rate by 20%. How are Youtubers getting away with such a long stick out in their videos? The answer is that their videos are sped up and/or depth per pass is shallow.

The shallower the depth per pass, the faster you can go

You will need to balance depth per pass and feed rate to achieve your desired carve time. You will need to consider your CNCs rigidity (MRR) in setting the depth. Even though solid carbide will break before it bends, it will still flex while cutting. You can hear this when you are cutting by listening to see if your CNC is "struggling". The "struggling" sound is a combination of your Z axis chattering and bit reverberating. If your carving is very loud, the finish you are producing will be suboptimal. To get your time back in profile cutting, divide the full depth of cut by the number of passes and see if you can reduce a pass or level out passes without increasing MRR too much. For example, if your material is 10mm, try to cut 3.4mm per pass instead of 4 + 4 + 2 where your feed rate is calculated at the 4mm depth of pass value.

Diamond Like Carbon DLC coating is the new kid on the block

DLC coatings have the characteristics of hardness, lubricity and abrasion resistance which is what you need when it comes to CNC router bits. The special qualities of a 1 flute DLC coated bit for Aluminium bit allows for harder cutting in softer aluminium’s like 5005 while also reducing the need for coolants. Coolants are still good to use but what you will find is that you will not need as much in malleable metals and potentially not have the need to use it on 5083. A bonus of a 1 flute DLC coated bit is that you can use the bit on plastics and get a really good side finish.

Low / ideal / high is just an arbitrary guide

You will find that if you aim for the low, you will achieve a better cut finish while if you use high values, you will get more life out of your bit.

Calculating ball nose feeds and speeds for 3D carving

You can use the calculator to determine the appropriate feed rate for ball nose bits. The calculator assumes that WOC or width of cut is 100%. Typically when programming a ball nose step over, you will be using between 5% and 15%. The calculation to use

• Choose 2 flute up cut uncoated
• Input the bit diameter (not radius) and cut length
• Determine the max depth of cut
• Choose 16,000RPMs as a start for timbers
• You will see that your feed rate is very low and that is ok. Divide 100% by your step over, multiply that by the calculated feed rate. The new value is the feed rate to use for carving and pocketing.
• If your carve starts with a deep initial plunge, you will need to adjust your feed rate to a WOC of 100%.

The calculator assumes your bits are new and sharp

Bits will stay sharp for a fair while but will degrade sharply due to the following factors:

• Unsuitability of the bit to the material
• Low carbide quality with large carbide grain size
• No coating or poor-quality coatings
• Chipped tips and edges
• Worn or burnt bits

The width of cut assumed in the calculator is 100%

If you are removing product through pocketing and will only be engaging a portion the of the diameter of the bit, you can divide 100% by the step over % to get a new feed rate number.

Using a Makita RT0700 and its variants, the following RPM values apply

A Makita trimmer starts at 10,000RPMs at 1 and increases in increments of 4,000RPMs to a maximum of 30,000RPMs

1 – 10,000

2 - 14,000

3 – 18,000

4 – 22,000

5 – 26,000

6 – 30,000

Relationship of feed rate to RPM and how to maximise productivity and reduce cycle times

So you have read the guide and determined that both you and your CNC are ready to up your game. Considering the feed rate has a direct relation to RPMs, by increasing your federate by 20% as an example, you will want to increase the RPMs by the same percentage. Another way to squeeze that bit more feed rate, increase your feed rate while cutting and listen to how the bit is behaving. Once the bit sounds to be struggling, start increasing the feed rate and RPMs at the same rate. When you hit the maximum travel speed of your CNC or spindle speed, you can now start to increase the depth per cut.

FAQ

If you want to save yourself time and would like the TLDR (too long didn’t read) version, here it is.

• Pick the correct bit for the job
• Use optimal feeds for both bit and CNC
• Reduce the amount of time a bit dwells at high RPMs in a single spot
• Replace the bit once worn

If you want my experiences and anecdotes, here it is in the form of a FAQ

Why isn’t there any speeds and feeds for V bits, surfacing bits, router bits etc?

I haven’t worked out an appropriate and accurate feed rate calculator for V bits yet. The issue is that it’s very hard to determine the tip strength and the effect on your material at certain depths.

To get you started though, for bits 45deg and below, start at 2m/min and go shallow at about 1mm at 12,000RPMs. If you are not sensing any struggle on your CNC and the cut quality is acceptable, start to increase the depth and feed rate. For bits above 45deg, try 3m/min. A V bit with a small tip diameter and sharper angle will snap easier. If you are unhappy with the finish, find that you have a low of furries or you have step over markers, rerun the job at full depth and drop the Z by a few 0.1mm. That will reduce sanding and post processing.W

Why am I getting crazy numbers for a surfacing bit?

That is the calculator doing it’s thing, but it does not mean that you should run it at those numbers. It assumes that you are running a 22mm solid carbide bit with a 22mm shank, not a 6.35mm HSS shank.

For a 22mm surfacing bit, start at 4m/min at 1mm depth at 12,000RPMs and either increase feed rate or increase depth.

I am using a 6mm bit on my hobby CNC. I am getting burrs, my bit isn’t lasting and I’m getting heavy chattering, what am I doing wrong?

The most efficient your bit will cut at is 90.00deg perpendicular to the material, optimal bit settings with zero chatter. It is hard to achieve all three factors with a large cutter on a hobby CNC. A sign your CNC is not running optimally is by listening to it while cutting. If your CNC sounds like it’s struggling, you are generating sound which translates to a bad finish. The way to reduce this is my reducing the diameter of your end mill or reducing the length of your bit.

My cuts start off great then starts to degrade after a few minutes in. If I use a slower RPM, my cuts don’t come out perfect. What’s the go?

Sounds like the RPMs are way too high for the feed rate and you are using a less suitable bit. Your bit is burning up and wearing fast. Switch to a more appropriate bit and use the calculator to determine the optimal feeds and speeds. If you are still not achieving an acceptable result, it could be the material you are cutting. Soft materials will produce furrier cuts and chip out easily.

More flutes means better finish right?

No! It all comes down to chip evacuation and sometimes using less flutes will produce a better cut. For example a 1 flute up cut for plastics is excellent on hardwood timbers by producing a quieter cut. It is the go-to for people with smaller less rigid CNCs. Only a 1 flute should be used to profile cut plastics and aluminium. Using bits with multiple flutes will heat up the material and cause gumming, sometimes instant. The only occasion 3 flute router bits make since is high production where every second counts.

Why is the colour of my bit black and can I clean it off?

Black material forming on your cutter is a sign that you have burnt your bit. The material, usually timber has deposited back onto the cutter and will degrade faster to the point of being completely blunt. High RPMs as a ratio of feed rate or high RPMs with a toolpath of a lot of 90deg corners will start to burn the timber and deposit residue. Reducing the RPMs or the number of flutes used will reduce burning. A situation where there is almost very high chance of burning is a 3 flute compression cutter. The extra flute over a 2 flute means you have to run the feed rate 50% higher or reduce the RPMs by 33%. There have been many occasions where I have suggested to swap to using a 2 flute over a 3 flute and not adjusting the feed rate or RPMs.

Can I sharpen/regrind my CNC router bits?

There are limited situations where you would find it economically viable to regrind router bits. It would be true that larger diameter end mills would be a suitable candidate for regrinding because of the generic cutting tip. With CNC router bits it’s not that easy and the price of the regrinding would be half to the full cost of a new bit.

My feeds and speeds are correct, why am I breaking bits?

Material and or waste-board is not levelled

By far my favorite cause of all time! Just like with depth per cut, if you plunge into your material at an aggressive depth, it will break. Same goes when you are thinking that you are cutting at X, but now X + a millimetre or two. 

Your board should be levelled each time you install a new board. You will would be surprised the effect of moisture and humidity has effect on your boards level. Also, using screws to hold your material down creates nice 0.5mm to 1mm craters. Use screws sparingly and if you do use them, level them out with a sander or chisel before the next carve. Using plywood as a waste-board is not advisable. They tend to warp easily so stick to a thick 18mm+ MDF board

Hitting something it shouldn’t

Yes an obvious one and one that we have all experienced, hitting a screw, clamp or piece of material just after being cut out. Avoiding the use of screws and clamps is one way to avoid a breakage. There are holding methods best described in this article holding it down. Allow for a higher safety height when travelling. There is a reason why Easel uses 3.8mm as a safety height. Going any lower is “tickling the dragon's tail” so maybe get some experience before you try. Holding your material down with tape or tabs is advised as it’ll stop the part you cut out from wanting to pop out. Using a down cut router bit mitigates this. Holding your material down sufficiently is another consideration. If there is even a slight vibration, this will lead to early deterioration of your bit

Tool run out

Now we are moving into the more obscure causes. Tool run out is where your bit is not rotating on its axis perfectly. If a bit is jiggling or not tightened correctly, it’ll start to cut it’s own path and make all sorts of mess. Using the right sized collet sounds obvious but sometimes overlooked. Using a 6.35mm collet for example for a 6mm bit is not advisable, no matter how tempting. Sitting the bit in just above the flute cutting length is not only good for achieving a higher feed rate, but also increases rigidity substantially. I aim for 3mm above where the flute stops. Collet maintenance is also another good practice to instil. After and before each time you install a new bit, ensure the slits are free of material and there is integrity in the collet

Your machine has something loose or NQR

Checking to see that your CNC is in good shape is not only a good thing to do, but also another cause of breakages. If your CNC is vibrating, that is a sign there is something loose. Check that the following are tightened:

• Wheels and eccentric spacers
• Belts
• Spindle holders
• Nuts and bolts

One story that comes to mind was the shop that had a $400k CNC of which they could not return the ⅛” bit to the same hole and blamed it on the bit. The other was that they were breaking a 3mm 2 flute for aluminum constantly. I suggested a list of items but ended up refunding their unused bits. 3 months later I got a call from the owner saying that the spindle had busted bearings and was the cause for all their issues

Compromised material

A less obvious one is foreign matter in your material. I have heard of customers buying cheap ply from overseas only to realise that there were staples and rocks pitted all throughout the material. Same goes for recycled material like pallet boards regarding forgotten nails.