CNC Machinist Trial and Error: An Unfortunate Reality

Trial and error is sometimes a requirement for CNC machinists to dial in their program, minimize their cycle time and perfect their finished parts.

So here we are.  You have read all of my eloquent, informative, and groundbreaking (perhaps a minor exaggeration) blogs.  You are ready.  You have a pencil behind your ear and a calculator on your desk and you’re going to trust in the numbers!  Slow down there cowboy, because the most important thing to remember is the numbers, formulas, and suggestions are just that – suggestions.  They give you a reasonable starting point. They get you in the neighborhood but some good old CNC machinist trial and error might be in order.  I know, if you bought an expensive GPS unit for your car (who buys those anymore?) and it GUARANTEED to get you within ten blocks of your destination and left the rest up to you then you might wonder why you bothered.  Well my friend, if that building you were driving to was constantly moving and changing based on the simplest of variables then ten blocks isn’t too shabby.  Besides, you got my Shop Math formulae for free.  Stop complaining.

CNC machinist trial and error is often a necessary part of optimizing milling performance.
CNC machinist trial and error is often a necessary process even when using the most bullet-proof machining program.

Control the Variables

The point is, no matter how sophisticated your CNC machine, software, tooling, or ego is you will always have to make adjustments.  Sometimes minor, sometimes major.  It all depends on what you are doing and how you are doing it.  There are an endless number of variables involved with machining so I won’t even attempt to touch on all of them.  The name of the game is eliminating or at the very least CONTROLLING those variables to get consistent results every time.  Let’s say you set up a new job on Monday morning.  This job uses eight tools and takes approximately two hours.  The tools do well all day Monday and when you come in Tuesday morning the second shift guy tells you he had to look busy so he swapped out all the tools.  When you ask if they were worn out he replies “I dunno.”  You would think they would be smart enough to put a competent human being on second shift since there is far less supervision, but trust me I know how that goes.  Anyway, you have many issues now.  Judging by Gomer’s attitude and general work ethic you can assume that none of the new tools were properly measured before he put them in.  So it’s time to get to work – measure all your tools, check your zero points, make sure your speeds and feeds are good.  Should be all set, you say?  Guess again.  Same program, same machine, right tools, everything looks good.  That doesn’t mean it will cut the same as it did yesterday.  Or even two parts ago.  Depending on the tolerance you are working with something as simple as the ambient temperature and humidity can affect the final result.  This is where some CNC machinist trial and error comes in.

Warming up the spindle before machining prevents thermal expansion of the spindle.
Warming up the spindle helps to eliminate thermal expansion of the spindle as one of the variable.

Warm Up the Spindle

Before you decide a program is ready for production and release it to Gomer, you need to make some determinations.  First off, make sure no matter what that you always warm up the spindle.  If you warm up the spindle properly before running your first job of the day then you will ensure that thermal expansion in the spindle will not become one of your variables.  That way the fifth part will come off just like the first.  Also, any time your machine is going to sit more than a couple hours it is a good idea to do a warm up, especially if you are working with tight tolerances.

Standardizing tool libraries helps to control variables so that trial and error is kept to a minimum.
Standardizing tool libraries helps to minimize variables and maximize efficiency.

Know Your Tools & Standardize Your Tool Library

Another consideration when preparing a job for production is tool life, so you can avoid the problem mentioned above.  By testing and running through some “CNC machinist trial and error” you will learn a lot about tool life and be able to compile some simple information and expectations.  You will find that the more you do this, the faster and easier it will become.  You will reach a point (especially if you followed my advice from my previous blogs and set up a standard tool library) that the information will just be there and suddenly your reference material will be right off the top of your head.  Once you know your tool life you can be much more proactive in your approach to shift change and work flow.

Feeds and speeds can be tested through trial and error to optimize the cut and cycle time.
Guideline feeds and speeds can be fine tuned through trial and error to maximize performance and cycle times.

Trial and Error with Feeds and Speeds

CNC machinist trial and error also comes into play when efficiency and productivity are the goals (when are they not?).  So my suggested speeds and feeds get the part done in twenty minutes, but if I take a 10% lighter cut and increase my feed 20% then the part is off the machine faster, and my tool will last for eight parts rather than five.  I have cut time, increased tool life and made the boss happy.  What about QC?  Are they still happy?  OK, so my surface finish suffered a little, but it’s still within specifications so we are good.  Success!

Trial and error with tools can result in breaking a tool in order to understand the full potential of that tool.
Trial and error with tools sometimes means pushing the envelope or even breaking a tool.

Don’t be Afraid to Push the Envelope … or Break a Tool

If there is one thing for you to remember it’s that ERROR is half of trial and error.  The best machinists I ever worked with broke tools on a regular basis, just because they wanted to see what they could do.  A little bit of CNC machinist trial and error, pushing the envelope, will get you farther than you may think.  You will discover very quickly that the envelope is far more expansive than you imagined.

Learn More: Download the High Speed Machining White Paper:

Tool Deflection in CNC Machining

Have you ever wondered why after milling a hole or pocket that it measures larger at the top of the cut than at the bottom?  Or why your gauge pin fits nice and snug in the beginning of the hole but won’t quite make it all the way through?  The simple answer is tool deflection.  Everything bends.  And I mean everything.  Tool deflection is an omnipresent yet little understood problem.  Worry not my fellow machinists, because it is not your fault!  There is no eliminating tool deflection, only controlling and minimizing it.  Knowledge is power, and hopefully by the end of this post you will have a working knowledge of the causes of tool deflection and potential solutions.

Simply put, tool deflection is the bending of the tool.  When you cut a feature, for this example we’ll say a deep pocket.  While cutting you are applying forces to the tool and the material.  The material gives, which is why you get chips.  However, it does not go down without a fight.  When the material pushes back it forces the end of the tool in the opposite direction of the forces being applied to the material.  The farther the tool sticks out, the farther the end of the tool will move.

It is possible to calculate tool deflection, but the math involved is quite complicated.  If you spend any significant time in a machine shop then you know how often optimization is achieved with your eyes and ears – I consider those two things the most important tools a good machinist can have.  However, if you would like to calculate some numbers for tool deflection there are multiple calculators available online.  For the purposes of today’s post we will rely on our trusty eyes ears and little bit of that common sense.

Tool deflection is reduced by using tools with a larger diameter shank and less flutes when possible.
Tool deflection can be reduced by using the largest diameter and lowest number of flutes possible.

Rigidity is the most important factor.  As you increase the distance your tool sticks out of your tool holder the rigidity decreases exponentially.  There are situations when you need the length, in which case, your best course of action is to use the largest diameter with the least number of flutes.  As you decrease the diameter of your tool you also decrease the amount of force required to make it bend.  Also, every flute on your cutter reduces the rigidity of your tool.  If you are cutting a deep feature, you want to make sure that you are using the largest diameter the print will allow in order to optimize tool performance. Even if you need to rough with a larger diameter tool, and finish with a smaller tool in order to meet specification on your corner radii that’s OK. You also want a tool with the least number of flutes, and only stick the tool out as much as you truly need to.  When researching tools, you will find that there are tools for which rigidity is a major concern and many “micro” tools come with a tapered shank to increase rigidity.

Carbide Tools vs. High Speed Steel Tools to Reduce Tool Deflection

If you think tool deflection is an issue, or you are performing cuts aggressive enough that it is causing you problems, then one thing you should always consider is carbide tooling.  Aside from the benefits like higher SFPM and better tool life, carbide is about three times more rigid than high speed steel.  Keep in mind however, that carbide is extremely brittle – that is not a good combination when talking about tool deflection. It takes more to deflect it, but if you provide enough force the tool is not as forgiving and will break, so beware.

As discussed in my “Climb Milling vs. Conventional Milling” blog post, cutting strategy can affect tool deflection. Utilizing dynamic toolpath strategies (see my blog post “Dynamic Milling”) can assist in minimizing tool deflection due to the light radial cut. If you rough the feature using a dynamic toolpath and make sure you are climb milling then you should be happy with your results.  As discussed in these other posts, for the finish you have a couple options – either climb mill the finish or conventional mill a spring pass, or conventional mill a light finish pass with lubrication and you will be very happy with your results.

 Download Cutting Tool Catalog

Threads – Tapping and Thread Milling

Hey folks, today we are going to talk about threading in multiple forms. For the most part I am going to discuss my experiences with the different types of thread cutting/forming, so if you are looking for tons of technical information I apologize, but there are so many variables when it comes to the threading –perhaps I can write a more technical blog on each type of thread forming. For now, we are going to give a general overview of cutting threads based on my experiences and opinions. I know, opinions are like… well, you get it, just stay with me and hopefully I can provide some insight.

First and foremost we have cut taps. In my experience cut taps are the most widely used across most industries. Cut taps are reasonably cheap and very versatile. You have all seen the drill charts that give you the tap drill sizes required for different threads. Pretty straight forward – drill the hole to the right size and depth, countersink the hole, then tap it. Cut taps can be used by hand, on a drill press with a tapping head, on a knee mill, or rigid tapping on a CNC machine.

Creating Threads in Through Holes with a Cut Tap

Threads can be produced using a standard cut tap like this with a CNC machining center.
Standard tap for creating threads with a CNC milling machine.

When determining which tap you need you should pay attention to the type of hole you are tapping. When tapping a through hole you can use a standard cut tap which has a lead on it. The lead is the tapered portion on the end of the tap that essentially centers the tap in the hole when engaging.

When tapping a through hole you need to make sure you go deep enough to cut threads all the way through the hole – the length of the lead will depend on the size of the thread. The larger the thread the longer the lead.

Threading a Blind Hole with a Bottoming Tap

Bottoming taps are used to thread deeper in blind holes.
This bottoming tap has little or no lead and allows you to thread deeper into a blind hole.

However, if you are tapping a blind hole you would be wise to consider a bottoming tap. A bottoming tap has the lead almost completely ground off. This allows you to engage the tap deeper into a blind hole. These are used when there is a tighter tolerance on the depth of the hole, in situations where a hole too deep will break through into a feature. This is due to the main problem with cut taps … CHIPS. When using cut taps in a blind hole, regardless of standard tap or bottoming tap, you need to make room for chips. As the tap engages the hole it is cutting the thread geometry out of the material, therefore creating chips. Since you are engaging from above the chips are forced down in the hole along with the tap. If you do not provide enough room at the bottom of your hole, then you will break your tap. Simple as that. That is why bottoming taps are so helpful in blind holes – with a very short lead you do not have to drill as deep to form full threads to a certain depth. Keep in mind, there are taps available with helical geometry with the goal of lifting chips up out of the hole. In my experience, I have gotten mixed results. The complex geometry ultimately weakens the tap, so if you are tapping a tough material be careful. Just make sure you do your homework.

The Strength of a Roll Form Tap

Roll form taps require more torque but are more durable than cut taps and are harder to break.
Roll form taps like this are stronger than cut taps and forms threads rather than cutting them.

Next, we have roll form taps. When I first discovered roll form taps, I was in heaven.  It was after a particularly frustrating week of broken taps and bad parts. Chances are if you are reading this then you have had some of those weeks.  We all have.  Roll form taps are much stronger than cut taps, and the geometry is completely different. The one drawback to roll form taps, and a major reason most shops I have worked for never adopted them completely is because the standard tap drill size no longer applies.  Most standard drill charts (the large ones you put on the wall in the shop) now have standard tap, roll form tap, metric tap and STI tap drill sizes all listed separately. However, after years of using standard taps many of us don’t reference the chart as much as we should, and since the hole for a roll form tap is significantly larger than that for a cut tap, bad things can happen. A roll form tap does exactly as the name hints – it forms the threads rather than cutting them. When the tap engages the hole rather than cutting material away it changes the form of it, and shapes it into the thread geometry. If you have ever done any work for a defense contractor, this is why most prints will have a note that all threads must be formed by a cut tap. The military generally frowns upon operations that change the structure of the material, at least in my experience. They also frown upon castings as opposed to solid plates for complex parts – too much unknown in what you can’t see. Anyway, roll form taps are great.  They are difficult to break (no, that’s not a challenge) but they also require a bit more torque. I have really only used roll form taps in aluminum and other soft materials, rarely in cold rolled steel. I am not sure how they perform in harder materials, but most shops don’t like the idea of two sets of drills for the same size thread, which is why they are not more widespread.

The Versatility of Making Threads with a Thread Mill

Threadmills are used to thread previously drilled or bored holes.
Helical boring rather than drilling combined with thread milling allows you to produce a multitude of different sized threaded holes with just two tools.

The final type of thread cutting is thread milling. Thread milling is a great operation that seems scary at first, but once you get it down it is truly amazing. There are many different types of thread mills, which I will get into in a different blog post. For now, I will discuss a single point thread mill. With a single point thread mill, you have great versatility, with most thread mills cutting a wide range of threads. You can create custom pitch threads, right hand or left hand, inside threads or outside threads all with one tool. Since I have recently started using helical boring for my holes rather than drilling, you can accomplish many different holes, with many different threads all with two tools. You bore a hole to the minor diameter of the thread, send the thread mill in to cut the threads, and you can use the thread mill itself to chamfer the top of the hole, as long as it doesn’t have to be a ninety-degree countersink, since most thread mills will be somewhere between thirty and sixty degrees. Due to the geometry of the tool, the only distance you need to make up for is from the outside edge (cutting edge, or point) of the tool to the flat tip, which is generally less than .02” on the smaller thread mills. The real benefit here is that once you mill the hole, you can send the thread mill to the bottom of the hole and mill from the bottom up, rather than top down. By doing this you are avoiding any concern of the tool running into chips at the bottom of the hole since you are moving away from the bottom of the hole. Looking at the thread mills you may not believe at first that it is going to do what it is supposed to. I know when I used one for the first time I was sure it was going to break – but it didn’t.  Thread milling is the most versatile and efficient of thread forming strategies, and it is going to be my go-to from here on out unless there is a good reason I can’t do it.

Mill a Hole and Thread it with the Same Tool

More Info. on Thread Milling vs. Tapping

Do your homework, know your tools and your materials and approach anything you do in the machine shop with a good understanding and clear head.  This doesn’t change when you are threading holes.  Trust the numbers, and in this case, don’t be afraid of trying new things. I always scoffed at thread milling – I only wish I had found it sooner.  Stay safe folks.

 Download Cutting Tool Catalog

Dynamic Toolpaths to Optimize CNC Machining

Dynamic tools paths help to extend tool life and the life of your machining spindle.

If you have spent any considerable time in a machine shop I am sure you have heard the term “dynamic milling.” There are many other names out there depending on the CAM software you use – Edgecam calls it “Waveform” while Surfcam calls it “TrueMill.”  Solidcam calls it “iMachining” while Mastercam calls it “Dynamic Milling.” You get the point. Every CAM package will claim theirs is the best, and while they may approach certain cuts differently, they are all based on a simple principle that in practice will give you amazing results.  I have been a machinist and CNC programmer for ten years, and my first experience with dynamic toolpaths had me speechless. Today I hope to open that same door for you.

Each CAM package calls their dynamic milling function by a different name ... and most of them will give you very favorable results.
Each CAM package calls their dynamic milling function by a different name … and most of them will give you very favorable results.

Dynamic toolpaths are not a new concept by any means. There is a very good reason many machinists have long used light depth (axial) cuts with heavy side (radial) cuts to achieve their machining goals. Any machinist who has been in the industry more than 25 years remembers a day when CNC was the minority. Current CAM software allows for significantly more complex and lengthy programs and precision. When you are turning handles on a Bridgeport maintaining a 10% step or a specific chip load would be impossible with dynamic motion involved. Can you imagine hand writing and punching tape for a 600,000-line G-code program? It’s been done, but it certainly can’t be called efficient. So it’s not for a lack of knowledge, simply a lack of technology that dynamic toolpaths are not standard practice … yet.

Maximize Tool and Spindle Life with Dynamic Toolpaths

Dynamic strategies have a very simple principle – maintain a constant chip load throughout the entire cut utilizing a full depth (axial) cut and very light side (radial) cut. The benefits you will see from this type of cut include longer tool life, longer spindle life, improved surface finish, greater efficiency and awesome rooster tails. No really though, I’m not joking. You are going to have people standing there watching the machine run just because of how the chips are flying.

Both tool and spindle life are extended with dynamic toolpaths.
Dynamic toolpaths help to extend the life of your machining spindle as well as your cutting tools.

First and foremost is tool life. I will also throw spindle life in with tool life because they really go hand in hand. You get multiple benefits for both your tool and spindle if you properly apply dynamic strategies.  If you are cutting a pocket or any internal feature that doesn’t allow an approach from outside the material, then entry into the cut is not only the first consideration, but one of the more important.  I always use a helical entry motion with a 1%-3% helix angle, or entry angle. You want to use an entry diameter that is somewhere between 120% and 150% of your tool diameter – be careful, sometimes the CAM software asks for a radius rather than a diameter and that information makes a huge difference.  Once you are at depth the real fun begins. Due to the light radial cut you can really be aggressive with your feed rate.  Depending on the limits of the spindle RPM, use the tooling manufacturers specifications on chip load and surface feet per minute (check my blog on shop math). In my first experience with a dynamic toolpath I was running a 3-flute .500” end mill with a 1.5” flute length. The cut was 1.375” deep, with a 10% (.05”) step over with a feed rate of 144 inches per minute.  I used a high helix end mill to assist in chip evacuation which created a “rooster tail” of chips trailing the cut. It was a thing of beauty. Even though the cut was so fast and seemingly aggressively deep, the tool lasted through 32 parts and gave the same finish on part 32 that it had given on part 1. The full depth cut means that you are wearing the entire flute length evenly, therefore you are not going to get lines on your finish. The light radial cut reduces the cutting forces, thereby reducing overall wear on both the tool and the spindle.

Dynamic toolpaths result in optimal chipload and chip evacuation that produces rooter tails.
Dynamic toolpaths help to extend tool life, spindle life, improve surface finish, maximize efficiency and create awesome rooster tails.

Efficiency is also a significant benefit. Pretend for a moment that you are cutting a 1.375” deep pocket with features at 4 different depths. Using a standard toolpath and a light depth with a heavy step over you will cut from the top of your part down. Depending on how aggressive you are with your step down you will cut many passes on each depth, with the deepest being the most time consuming. Utilizing a dynamic strategy you will cut from the bottom up, meaning each depth will consist of one pass, with all previous passes having already cleared out other material at that depth. Therefore, at each depth you are only cutting the remaining material, essentially creating a “rest rough” toolpath that minimizes total machining time.

With dynamic toolpath strategies you will not only improve tool life, spindle life and surface finish but also overall cycle time and cost efficiency. Not to mention you will impress the boss and anybody else who happens to walk by. Do me a favor, and give it a shot.  You won’t be sorry you did.

 Download Cutting Tool Catalog

Minimize Burrs in CNC Machining Applications

Burr free milling is possible if you use very sharp tools.

This may seem like a strange topic for a blog post.  Burrs, really?  Snorefest, am I right?  I understand, trust me.  Let me ask you one question before you move on to the next post, what do you do to your parts after they come off the machine?  Depending on your coolant you wash them, then are they ready to go to inspection?  No sir, nine times out of ten they are not.  When the part comes off the machine there is almost always some form of deburring operation.  Unless of course the programmer includes small chamfers on your part as a deburring operation inside the program.  Either way, when you spend as much time as you do performing a single omnipresent function, how could it be as trivial as everyone seems to think?  I have worked from prints dating as far back as 1938, and even that print had a note on it requiring all sharp edges and burrs be removed.  This post is intended to shed some light on the often ignored topic of burrs, and perhaps teach you a bit in search of strategies aimed at eliminating, or at the very least minimizing burring on your machined parts.

Burrs are a concern for multiple reasons.  First and foremost, they can cause dimensional issues or fit issues. The dimension on your part may be right on, but if there is a burr on the edge then subsequent parts may not fit.  Along those same lines, depending on the location of your burr you could have a part that is in fact within tolerance, but measures out of spec because of burring.  Another major concern when dealing with burrs is cost.  Deburring, like inspection, is not a productive operation – you are not producing parts, simply making the parts that you already produced meet requirements.  Since the operation itself is not making money, it must be costing money.  You know how it works – if it costs money, do less of it.  It doesn’t matter how unreasonable the request may be, just do the same thing you’ve always done.  Only, do it faster.  And for less money.  And with no overtime.  I digress – deburring operations can be reduced, which will make you more efficient and your department more profitable.  Many studies have been done on the causes of burring, and one of the reports I read was somewhat eye opening.  On a part of medium complexity it is estimated that deburring accounts for 14% of the total manufacturing cost. 

Sharp tools reduce burrs and monitoring tool life will help to minimize burrs and produce consistent quality parts.
Sharp tools reduce burrs and for that reason it is a good idea to use a different tool for finishing than the one used for roughing.

There is a lot of money to be made by optimizing strategies and tooling selection.  One of the more common culprits is the tool you are using.  Always make sure your tools are sharp, since a dull tool can cause serious burrs even with the optimal tool path.  In fact, watching for burrs is one of the best ways to monitor tool life, at least until you have a good understanding of how your go-to tools are going to perform.  Also, this is one reason it’s a good idea to use a different tool for finishing than you do for roughing – that way you ensure the best finish and also limit burring.

Minimize Burrs in CNC Drilling Applications

Burrs when drilling can be avoided by drilling deep enough (through the material) to account for the angled tip of the drill.
Burrs when drilling can occur because you haven’t drilled deep enough to account for the angled tip.

When it comes to drilling, many of the same rules apply.  A dull drill is going to give you larger burrs on the bottom of your part when you drill through – fresh drills will help with that.  One of the simpler causes of burrs when drilling is not drilling deep enough.  When you are drilling through your part you need to make sure you make up for the angled tip – the larger your drill diameter the deeper you will need to go.  Drilling too shallow will result in what almost looks like a cap on the bottom of your part, not to mention a taper at the bottom of your hole.  If you drill deep enough with a good, sharp drill you should be good to go.

Burr free drilling requires sharp tools and making sure you drill completely through the material to account for the angled tool tip.
Burr free drilling can be achieved by maintaining sharp tools and accounting for the angled drill tip when drilling through holes.

Burrs are a frustrating, time consuming problem that you will always deal with on some level.  Just take care of your tools, mind your feeds and speeds and make sure you are drilling deep enough.  It can be more efficient to utilize your CNC machine to deburr in process, just keep in mind there will always be geometry that you will need to deburr by hand.  Get next to it folks, cause it’s never going away.  Just keep it under control.  Until next time, be safe and mind the numbers.

 Download Cutting Tool Catalog

Job Setup Sheets and Documentation for the Machine Shop

Job set up sheet in a file folder for documenting all aspects of a CNC machining job.

If you visit ten machine shops you will more than likely find ten drastically different approaches to setup sheets and documentation procedures.  Every one of them is the best.  Just ask.  Proper and organized documentation and setup sheets are vital to the efficient operation of any shop, and adding multiple shifts and operators or programmers running multiple machines multiplies the necessity exponentially.  As with literally almost everything you do in the machine shop, there is no black and white.  I’m not going to tell you which way is the best, because there are too many variables.  I am simply going to make some suggestions based on my experiences.  I’m not going to lie, as I’m sure you have experienced firsthand, change is never easy.  Especially when you are dealing with the old salt that’s been doing this for 50 years.  You know the guy – same denim apron every day, same bologna and cheese sandwich for lunch (always at 11:45 instead of 12, just to be difficult), coffee at 9 and bathroom at 9:30.  You get the point.  It’s going to be an uphill battle, but it will be worth it.  If not, just wait until he retires.  It has to happen someday.

Before starting with job setup sheets, try to standardize tools in the same positions on all CNC machines in the shop.
If possible, standardize tools keeping them in the same position from one machine to the next and leaving two open “variable” spots in the tool changer.

My first suggestion is standardizing tools.  This is mainly a concern in CNC shops since you are manually loading tools on your manual machines anyway.  The first step in standardizing your tools is accomplished in your CAM software.  The tool database needs to be created.  I would always suggest starting from scratch.  As you program jobs and figure out which tools are the most common the picture will become clear.  Make a tool database that only holds the tools you use – it makes programming much simpler rather than having to play with filters and tool types.  It may take time to decide what works best for your shop but if Tool 1 is a 6mm single flute end mill on machine 1 it should be the same on all of your milling machines.  The last machine shop I worked in ran tools in numerical order for each job.  I would run anywhere from two to six jobs a day, and each job used a different set of tools.  Every job started at Tool 1, and unless it was a lucky day that tool was different from the last Tool 1.  Some of these jobs used upwards of twelve tools.  On a busy day (six jobs, twelve tools each) you are loading seventy-two tools by hand.  That doesn’t include any tools that needed to be changed in the holder.  Very inefficient.  Now let’s say we standardized our tools.  In every machine in our shop Tools 1-10 are the same, and we will leave two positions open for variables.  Tool 1 here is the same as Tool 1 over there.  Got it?  OK, now on that same busy day with six jobs, each using twelve tools you are loading up to twelve variable tools by hand.  Twelve is more efficient than seventy-two (you can refer to my blog on shop math if necessary, but I think you see my point).  You will have so much time to research sleepers in your fantasy football league that you are a shoe-in for the championship.  You’re welcome.

Setup sheet in a standard file folder using pencil to mark up changes and revisions as you complete the CNC milling job.
Setup sheets can be as simple as a file folder or manila envelope detailing everything in pencil so that you can make revisions as you go.

The next topic to discuss is the actual setup sheet.  This is a sheet that should accompany the job on some level.  To be honest my preferred method for this has always been a filing cabinet with manila folders.  I know, digital age and all that.  There is a place for that, but especially when you are trying to assimilate old guys who still aren’t quite sure how to check their email sometimes relying on digital paperwork can be difficult.  If the other programmer saves a file in the wrong location or makes changes without telling you then the whole system can fall apart.  Program a job, take a PENCIL (no pens!) and document the details.  My setup sheets always included the part number, fixture location, tooling list, and a brief description of the setup including the X, Y and Z zero points and any pertinent information on fixture location or operation.  Using a pencil was always an important aspect for me because not only can you modify what you write but you will be able to see if somebody else made a change and “forgot” to tell you.  The old guys get nostalgic with pencils too.  It puts them at ease, makes them a little more docile and cooperative.  I’ve experienced mixed results with that last point, so be wary.  Anyway, the point here is that you get a work order and you can go to your filing cabinet to pull that job number.  You can write the current revision level on the folder itself or the setup sheet to keep compliance happy, and when the job is done it goes back into the filing cabinet.  You can most definitely make an argument for doing this all digitally, and if you have a good system it is probably the way to go.  With a digital system you don’t have as much paper floating around, you don’t have to worry about physical damage (losing documentation in a fire for example) as long as you back everything up, preferably on an off-site server.  Digital documentation management is also more efficient since you are pulling the document off the same server you are pulling your program, all at the same time.  I have yet to use a digital system that didn’t have problems, hence my preference for the old filing cabinet but if you can manage a digital system and avoid any major headaches you are ahead of the game.

Job setup sheets let other CNC machinists know exactly how the job has been approached.
Notate everything in your job setup sheets and documentation so that other machinists who may step into a job know exactly what has been done.

Finally, I will talk about documentation.  This one is easy.  You will be using the folder and setup sheet that we already talked about, which has all of the information on it that we already talked about.  The point here is document everything.  While you were running the job on third shift Tool 2 was chattering a lot so you changed out the tool and slowed your feed rate.  They lost power briefly on first shift so they had to reload the program.  How will they know what changes they need to make?  I’ll tell you!  When the first shift operator came in this morning you were drooling on yourself so much he couldn’t understand any of the words coming out of your mouth, but he’s too nice to say anything.  Instead, he checked the setup sheet and saw the detailed note you left about the issue you had and how you fixed it.  Good work!  Now just in case you never updated the server he can make the change permanent and we’re done.  See?  I was able to teach you something after all.  DOCUMENT EVERYTHING, no matter how small or insignificant it may seem.  As I have stated before, it’s usually the small stuff that makes the difference.  There is always a different way to do things and the people who can recognize where their process is lacking are already ahead of the game.

 Download Cutting Tool Catalog

Absolute vs. Incremental Movement – What’s the Difference?

Absolute vs incremental movement is discussed in this machinist's blog detailing the use of each method.

Absolute vs. Incremental Movement? These are two terms that you will hear or use in the machine shop, and there are many people who don’t really understand the difference.  When I am in a customer’s shop training them on their new machine, it’s a little surprising to me how many people don’t know what the distinction is. Don’t get me wrong, there is nothing wrong with not knowing – after all, if you already knew then you wouldn’t be reading this right now and then my existence would be meaningless.

Absolute vs. Incremental Movement

In my experience there are a couple ways to convey the difference between absolute movement and incremental movement. When it comes to machine movement, simply put:

An ABSOLUTE movement moves TO A COORDINATE based on your ZERO POINT.

An INCREMENTAL movement moves A DISTANCE based on your CURRENT POSITION.  An incremental movement does not take your part zero point into consideration.

Absolute movement tells the CNC machine to move to a coordinate based on your zero point.
Absolute Movement – used to move the machine from a random location at the back of the work area to the zero point (in this case, top of the left front corner on the workpiece).

Let’s run through an example.  We will work on the assumption that you have a fixture and work piece set up on your machine, and your zero point is the front left corner, with top of stock being Z zero.  You just finished setting up your tools so you are located near the back of your table at some random coordinate.  We will pretend that your program starts from X0 Y0 Z0.5.  So here is your dilemma – you are currently at X6.753 Y14.265 Z2.37 and you need to get to X0 Y0 Z0.5. How will you do it?

Absolute vs. Incremental?

Well, technically you can use either absolute movement or incremental movement. To make this incremental movement you would enter X -6.753 Y-14.265 and then you do some math. You are currently at Z 2.37 and need to reach Z 0.5.  2.37 – 0.5 = 1.87.  So for your Z input you would enter Z -1.87.  This would get you to X0 Y0 Z0.5.  On the flip side, if you make an absolute movement your input will be X0 Y0 Z0.5.  You are telling the machine “I want to move the X axis to 0, I want to move the Y axis to 0, and I want to move the Z axis to 0.5.”  This is where the real benefit of an absolute movement comes in.  When you are moving TO A POINT absolute is the much simpler way to go.

Incremental movement is telling your CNC machine to move a distance away from your current position
Incremental Movement – used after milling a hole in a part and needing to mill another feature 6″ away.

On the other side of this argument, is the situation where you have drilled a hole or pocket in your part, and you know that you need another feature six inches away.  Now, if your first feature is at X0 Y0 then it’s really not a concern, since both absolute movement and incremental movement would be the same. However, if you are not at zero, then suddenly your absolute movement becomes more difficult as you need to determine a point in relation to your zero point, rather than a distance from your current position.  Let’s use the same numbers as before. You drilled a hole at X6.753 Y14.265.  You need a second hole six inches away in the X axis.  In order to use an absolute movement your XY input would be X12.735 (6.753 + 6.000) Y14.265.  Not too complicated, but certainly there’s a possibility for error.  On the other hand, if you choose to do an incremental movement your XY input is X6 Y0.  You are telling the machine “I want to move the X axis 6 inches in the positive direction, and I want to move the Y 0 inches.” With incremental movement you are telling the machine A DISTANCE.

It is altogether possible that I just made this more confusing for you. This is not an easy thing to understand at first, and as I have found in my training of others, it is not always an easy thing to teach.  Hopefully what I said makes sense – if not feel free to comment and ask any questions you may have.  Understanding the difference between absolute and incremental can make your job a whole lot easier and more efficient.

Download White Paper
Learn About High Speed Machining:

Shop Safety for CNC Machinists

Shop safety includes the use of personal protective equipment (PPE) as well as lockout tagout policies.

Shop Safety? Go ahead. Roll your eyes. Get it out of the way now. We have all seen the cheesy safety movies with terrible acting and fake blood. Don’t worry though, this isn’t like that – I’m a terrific actor. Seriously though, I took classes.

All joking aside, I know how easy it is to laugh it off and ignore the safety rules. Let’s be honest, a lot of those safety rules make all of our lives in the shop more difficult. I had one safety officer (any of you working for a large corporation will know exactly the type I am talking about) who required us to make Plexiglas covers for every moving part on all of our machines. Try setting a gear hobbing machine through three levels of six year old plexi. You get the point. However, one thing I learned very fast was that those safety rules were not created to make you less productive. They were created and enforced to – get this – KEEP US SAFE! One close call is usually all it takes (that’s all it took me) to start taking those rules a little more seriously and my goal today is to prevent the close call and maybe just speak some sense into you. If I manage to save a finger or two, or even a pint of blood, then I have achieved my goal!

Shop Safety PPE or personal protective equipment can include a wide range of items, but should always start with proper eye and ear protection.
Shop Safety PPE – Personal Protective Equipment starts with eye and ear protection.

Why don’t we start with my favorite basic rule – If you don’t do it while you’re driving, don’t do it while you’re machining. Don’t sleep, eat, consume alcoholic beverages, use drugs, call Grandma, text your buddies, or make unsafe lane changes while running your machine. Whether it is a high end CNC or an engine lathe it requires your full and undivided attention at all times. All of these machines are incredibly powerful tools that don’t have brains – don’t argue, even your half million dollar five-axis VMC doesn’t think for you. Machines do what you tell them to do, make sure you are aware of what you’re telling them. Common sense is not a part of the final sale, you have to bring that with you. Respect the equipment, it deserves it.

Personal Protective Equipment (PPE) for Shop Safety

Personal Protective Equipment (PPE) is a very important aspect of shop safety. This includes everything from safety glasses to gloves, earplugs and aprons. I have worked in shops that required hard hats because of a 20 ton overhead crane, as well as shops that would send you home if your sleeves were loose or long, or long hair wasn’t pulled back. On the opposite end of that spectrum I have worked in shops where sneakers and flip flops were more common than steel toe boots and safety glasses. Just because your company may not enforce the rules does not mean you shouldn’t follow them. If you ever need the safety glasses you will be glad you have them on. Always be your own advocate when it comes to safety, because even if you have that annoying safety guy always sneaking around to write you up for not putting your earplugs in he can’t be there all the time, and all it takes is a split second for things to go wrong.

Shop Safety Gloves can protect your hands when moving sharp material but could harm them if caught in moving parts of a CNC machine so know when to wear them and when not to.
Shop Safety Gloves – know when to wear them and when not to.

Shop Safety – Gloves … when to wear them and when NOT to!

Gloves are a tricky piece of PPE, because depending on what you are doing and which machine you are running they can be either helpful or harmful. Very harmful. If you are going over to the stock rack to grab a plate of steel a thick pair of leather work gloves will protect you from any sharp edges while you carry that stock. However if you are running ANY machine with a running spindle DO NOT wear gloves. Whether it is a CNC machine, a lathe, a knee mill, or a drill press wearing gloves near a rotating spindle and spell disaster. A lot of folks think they can get a better grip on their part while running the drill press if they were a heavy pair of gloves and the sharp edges won’t cut them. I can tell you first-hand how disastrous this can be – it is very easy for the drill or material to grab right onto that drill, and I will let your imagination take you from there. Assuming safety features haven’t been disabled (again, the common sense thing) then most CNC machines will not allow you to put your hand near the spindle while it is running. However, on the off chance you have both the chance and opportunity – DON’T! The only times that I ever suggest wearing gloves when running a CNC are either when fingerprints need to be avoided or when the coolant tank is full of month old flood coolant and your company hasn’t invested in anti-microbial/anti-bacterial additives. I have seen some pretty nasty skin infections from old coolant, so make sure you keep that in mind. In these cases wear latex nitrile gloves – tight fitting non leather gloves that will break with minimal force if necessary.

Avoid “Danglers” for Shop Safety

When running manual machines especially it is very important to keep any “danglers” in mind. Long sleeves, pony tails, baggy shirts, jewelry, etc. Anything that hangs off of your body – keep it to a minimum. Again, all of the above could spell disaster. I know you want to be the best dressed guy in the shop, but I would rather be the guy with all his limbs and digits. Just my personal preference.

Shop Safety Lockout Tagout is extremely important in the machine shop and when working around CNC milling machines.
Shop Safety Lockout Tagout is often overlooked but is critical when working around CNC machining centers.

Lockout/Tagout – take it seriously!

Finally I want to discuss Lockout/Tagout. The number of people whom I witness not following this procedure enough (myself included at times) is alarming. Lockout/Tagout for anybody who is not familiar is the process of powering down the machine and locking the power switch with a lock that only the service technician has the key for. The purpose here is to prevent anybody but the service tech from doing ANYTHING with the machine. Every time you service that machine without powering down and locking it out you are inviting accidents. Especially when dealing with CNC machines the consequences of this mistake could be fatal- it’s not worth the extra thirty seconds.

Safety is absolutely no joke. PPE can be uncomfortable, inconvenient and cumbersome. Safety procedures can be time consuming. Plain and simple, you never want to be in a position where you finally understand why they enact all these rules – just trust in them and follow your common sense. It is the most useful tool you will have with you in the machine shop. Stay safe friends.

Micro drilling: An incredible (and Incredibly Frustrating) Adventure

Micro drilling using drills far smaller than a human hair requires experience, research and the right milling machine.

So micro drilling has never been my forte.  I have done a lot of drilling but never anything much smaller than 1/64th or so.  Well friends, if you were a part of that club too then there is a whole other world of drilling that you have never experienced, and there are some pretty amazing things going on.  Some of the more recent research I have done on micro drilling has been very eye opening, and the project I am currently working on has been one of the most challenging in my career – all to drill holes slightly larger than a human hair.  We will discuss many of the things to watch out for and some basic parameters to start some of your own research projects.

Much like anything else in the machining world, the numbers don’t lie.  Many of the same formulae apply.  However, there is MUCH less room for error.  Everything from the length of your flute to the geometry on the tip of your drill needs to be scrutinized, and with micro drilling there is no easy answer for anything.  Tooling manufacturers will be your best resource for parameters to start with, since they are the experts on their own tools.  I am not a tool salesman, so I am not going to promote one brand over the other.  That, friends, needs to be part of your research.

Step 1 in Micro Drilling – Research the Material

Micro drilling stainless is shown in these impressive Xrays of a 0.004" hole drilled 0.040" deep in stainless steel rods.
Micro drilling stainless: Xrays of a 0.004″ hole drilled 0.040″ deep in stainless rods.

That brings me to step one of your micro drilling adventure.  Research.  You need to know your machine, you need to know your material, you need to know your coolant and coolant system, and you need to know your tools.  When I say you need to “know” I don’t mean a basic knowledge.  Research it, become as much of an expert as you can on everything you are doing before you even consider cutting metal.  When it comes to micro drilling in general there is a lot of research out there, and much of it provides conflicting or confusing information.  Arm yourself with the knowledge to fight through it and you will be OK. Research different coolants, research different drills.  Drill suppliers and coolant suppliers should both have people that you can talk to over the phone for more information – most importantly specific information about your material.

Micro drilling plastic like these tiny holes drilled in small cavities on a Delrin part.
Micro drilling plastic – this shows small holes drilled through circular cups (or cavities) in a Delrin part.

Currently I am drilling .008” holes into 15-5 PH stainless.  The first thing I did was learn as much as possible about 15-5 stainless.  It’s an interesting material because it is considered a stainless steel, but it acts like a die steel.  Because I knew that before doing my research I was able to navigate my way through the tooling manufacturers’ charts, skip right by stainless steel and take the parameters from the die steel section.  I avoided many headaches, because the parameters were very different – much slower spindle speed for the stainless.  My point is, material knowledge is key.  Know that first.

Step 2 in Micro Drilling – Understand the Coolant

Micro drilling of rounded surfaces like the one shown in this photo requires a 4th axis solution.
Micro drilling requires research to understand the material being drilled and the available coolants.

The second step, after you do your homework and figure out the specifics on the material you are running, the coolant you are going to use and narrow it down to two or three drill manufacturers is to look at your program.  First and foremost, when you are programming a micro drilling operation is the drill cycle itself.  There is varying information available on the most successful strategy, but one thing everyone agrees on is that it has to be a pecking cycle.  A chip break cycle (where the drill does not retract fully out of the hole, only enough to break the chip) is generally ineffective because it leaves chips in the hole. On a standard drill the flute is carrying those chips up and out of the hole. Technically, micro drills will do the same, except you really don’t want them to.  Drills that small (.008” in my case) DO NOT like re-cutting chips and will eventually break because of it.  A full retract on every peck is the strategy I choose, and while it may take a little more time it is the best way to ensure the longest life of your drill. There are machinists (and tooling manufacturers) who will suggest a “chip break, chip break, full peck” strategy, which will be faster but I would only apply this at the upper end of the “micro drilling” scale.  This scale by the way is another point of contention.  A micro-drilled hole is generally considered any hole smaller than .1”, but you will always have people who disagree.  Call it what you will, it’s small.  Anyway, back on track.  Strategy is very important.  You want to make sure that the tool clears the hole with enough distance and time to clear the chip and receive some coolant.

Optimal Coolant for Micro Drilling

Micro drilling coolant shown cooling a micro drill (in comparison to a pencil tip).
In micro drilling coolant is a key consideration. Here a spray mist (minimum quantity coolant) sprays on a micro drill (shown in comparison with a pencil tip). Yes, we drilled the pencil tip … because we can!

Coolant.  It’s an interesting term – true to life, since it is actually cooling the tool, or at least acting as a vehicle for heat transfer.  However, in micro drilling the more important aspect is the lubrication.  Water-soluble coolants do a very funny thing that most people don’t realize when you’re drilling.  When the bottom of your hole fills with coolant and the tool enters the hole, it actually becomes pressurized.  Under normal circumstances this is not a concern, but with micro drills being so fragile it can easily be enough to overpower the tool.  I am using a misting system for my operation, along with a thin oil that flows well.  What happens is the oil pools on top of the part, so no matter what the drill passes through the coolant and lubrication before contacting the part. The only problem this presents is chips.  As you machine holes you notice chips building around the completed holes.  Due to the fact that the oil is not flowing like a flood coolant, it doesn’t carry the chips away.  This is currently a problem I am trying to remedy, but again it’s a very time consuming process that involves much patience … and frustration.  You will be OK.  Plan to break a few drills, and plan to try different things.  Just don’t plan on drilling a hundred holes in ten minutes.  Micro drilling is not, and should not be considered a high-speed machining operation.  It takes care and precision.

Optimal Tools for Micro Drilling

Micro Drilling Tools can be as small as this 0.0015" drill shown in comparison to a penny.
Micro drilling tools like this 0.0015″ drill (in comparison to a penny) require research, experience and the right CNC machine to use effectively.

Finally, I’m going to discuss a little about the actual tools.  There are many tooling companies that provide micro drills.  In your research you will find that many of them have very specific information on the geometry they use for their cutters and the coatings and every other bell and whistle you can imagine.  Do yourself a favor and pay attention.  Some of it may seem like fluff, which it may be, but some of it is very important.  If you have read any of my other blogs then you know that sometimes seemingly small things make all the difference.  Such is the case here.  These tools need to be precision ground and incredibly sharp.  As is the case with most aspects of micro drilling, there are differing opinions on the tooling material – carbide or high-speed steel.  While carbide offers better rigidity and longer sustainability of the cutting edge, high-speed steel offers more flexibility. Carbide is brittle and will break as soon as it’s dull – high-speed steel is more forgiving and lower cost.  It all comes down to the workpiece material.  This is another situation where I hand it off to the true experts – the ones who make the tools.  One last bit of advice on the tooling – don’t go cheap.  If you do your research and you find that you can achieve your goals with a $15 drill that’s fantastic. Just don’t shy away from a drill just because it costs $75.  The name of the game is value, and be sure to explain to your finance department that the best value doesn’t mean the cheapest drill.  If “Drill A” costs $15 and drills 100 holes, and “Drill B” costs $75 but drills 1,000 holes then the better value is Drill B, even at five times the cost.

I would give you an idea of some of the parameters I am running but that would essentially defeat the purpose of my post.  Do your research, find your numbers and run with it.  I have been very impressed with the success of the base parameters I have received from tooling companies, so always remember – trust in the numbers.

Download a Real-World Micro Drilling Case Study:

Machine Shop Math – Common Formulas and Strategies

Machine shop math blog detailing feeds, speeds and formulas associated with CNC machining and milling machines.

One of the more common problems I have seen in my years in the machine shop is a general lack of readily available and handy information on machine shop math – specifically on feeds, speeds and related formulae.

Machine shop math for feeds, speeds and other important aspects of CNC machining and milling applications.
Machine shop math is an important consideration for CNC programmers and machinists.

Whether you are programming a 5-axis CNC machine or turning handles on a 60 year old knee mill the numbers don’t lie.  However, one very important lesson I have learned is to respect the variables.  Any common formula you are going to use in the machine shop will provide you with the information you need to approach the cut appropriately but remember to always treat that number as a starting point.  There are an immeasurable number of variables with any cut, all the way down to the atmospheric conditions in the shop.  Tooling manufacturers will provide you with suggested numbers whether it be surface feet per minute, chip load per tooth, revolutions per minute, inches per minute or any combination of those and more.  It can all get very confusing and overwhelming but don’t quit on me now.  I am hoping this post can serve as go-to information for you and your shop, and hopefully I can make some sense of it for you.

Machine shop math formula for RPM, SFPM, Feed Rate and Chip Load per Tooth to help machinists and operators of CNC milling machines.
Machine shop math formula for SFPM, RPM, Feed Rate and Chip Load per Tooth.

As you can see in the above formulae in order to calculate any of these you need to already know some of the other data to input.  This is where the tooling manufacturers come in.  They can provide information to you for their specific tools and applications.  However there is some basic information based on the material you are cutting that I will provide to you right now.  Keep in mind that these are starting points, the best judge will be your eyes and ears.  The following is a list of suggested SFPM for common materials:

Machine Shop Math – SFPM for Common Materials:

Surface feet per minute parameters associated with particular millable materials.
Surface Feet Per Minute (SFM) parameters based on material.

So let’s say we are using a .500” solid carbide end mill cutting aluminum.  Looking at our chart the suggested SFPM is 800.  In order to determine our suggested RPM we use the above formula SFPM x 3.82 / Tool Diameter:

Machine shop math formula for calculating revolutions per minute (RPM) can be used by CNC machine programmers and machining center operators.
Machine shop math to calculate RPM (revolutions per minute).

I will give you another example, this time with a significantly smaller tool.  We are going to use the same material but this time with a .125” solid carbide end mill.

In machine shop math SFPM or surface feet per minute can be calculated using this formula.
In machine shop math SFPM is surface feet per minute and can be calculated with this formula .

You can clearly see where the tool diameter drastically changes the suggested parameters, and where a high RPM spindle is a valuable factor.  This table can be used for these common materials however the manufacturer of the tools you choose will most likely have specific information on the tools you purchased which should always be used when available.

Are you still with me?  I know, you feel like you are in high school algebra again.  All of these numbers will make more sense when you start applying them to jobs in YOUR shop on YOUR machine, until then stick with me!  I promise it will be worth your time.  We are going to move on to Inches per Minute.  If you reference the formula above Feed Rate (inches per minute) = RPM x Chip Load per Tooth x Number of Flutes you see that in order to calculate this you need tool information.  Chip Load per Tooth is the amount of material a tooth, or flute, of the tool is removing in one revolution.  Most tooling manufacturers have suggested chip load information available, but you can also use your own knowledge and expertise to make a suggestion.

In this example we are going to be using a .500” solid carbide end mill with three flutes to cut aluminum.  Since we already know from the first example that the suggested RPM is 6,112 all we need is the chip load per tooth.  The manufacturer suggests .005” per tooth chip load on this tool, so we have all of the information we need to calculate our feed rate.

Machine shop math inches per minute formula used by CNC machine programmers and operators.
Machine shop math inches per minute formula.

See?  That is not as confusing as it looked.  However, here is where some of variables come into play.  Serious consideration needs to be made for the type of cut you are performing.  If you are milling a slot with full tool engagement then you need to be more conservative.  However, if you are utilizing a dynamic strategy (as discussed in another blog post) then you could potentially be more aggressive.  As I stated in the beginning, these numbers are starting points.

Finally, we will discuss how to calculate Chip Load per Tooth.  This is a useful formula for both preparing for a cut or programming and analyzing an existing cut.  You can easily look at your program while trying to optimize either surface finish, cycle time, or tool life and this will be a good indicator of proper tool utilization.  Let’s say we were running that last example at 4,000 RPM instead of the suggested 6,112.  We also ran it at 120 IPM rather than 91.68 IPM.  Our results weren’t great and Quality Control wants answers… NOW!  I know!  Let’s check the numbers!


This is double the manufacturers suggestion, therefore a very good place to start looking for problems.  Using the formula that you have now mastered, you know that you either need to bring your feed rate down or your RPM up to meet the requirements.

Now that you are armed with a basic understanding of these formulae and the knowledge that NONE of this is set in stone, you are ready to start applying it to your everyday work.  You will be amazed how quickly you won’t need to reference any charts or websites to be confident in your numbers and the job of programming a very expensive CNC machine will become a little less stressful.

If you want to put these formulas to work using the best cutting tools of the market, just download the DATRON Cutting Tools Catalog by filling out the following form.

Download Cutting Tool Catalog: