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

Balanced CNC Tools Reduce Vibration for High RPM and Feed Rates

CNC balanced tools are used in high speed machining applications to increase feed rates and improve cycle times.

Push Your Program to the Limit with Balanced CNC Tools.

I talk a lot about optimizing programs, some would say too much. I go on about it to lull my children to sleep. Though, I think there are worse subjects to obsess over. So, with that aside, let’s talk a little about tooling – specifically balanced CNC tools.

Balanced CNC tools are used when finishing, deep milling and roughing in high speed machining applications.
Balanced CNC tools are a consideration for Blog author, Dann Demazure, when he optimizes milling programs – particularly for roughing, finishing and deep milling in non-ferrous materials.

If you use a DATRON or any other HSC machine, you may be familiar with our line of single flute end mills. Most traditional machinists would utilize a single flute end mill for cutting soft materials, like thermoplastics or acrylics, but the geniuses at DATRON AG developed a line of single flutes specifically for milling non-ferrous materials, specifically aluminum. Coupled with a high RPM and a fast feed rate, our single flute cutters have a reputation for devouring aluminum at an impressive pace.

With high RPM being the most important feature to accompany a single flute end mill, DATRON had something clever in mind to combat vibration with larger diameter end mills (>6mm). DATRON calls it “Specially Balanced”.

Balanced CNC tools reduce vibration in high speed milling applications that require increased feed rates and material removal.
Balanced CNC tools like this specially balanced single flute end mill help to mitigate vibration.

As you can see in the picture, a healthy amount of material is removed from the backside of the cutting edge to balance the tool. What does this mean for the end user? A couple of key points:

  • Reduced vibrations = reduced chatter marks
  • Balanced tool = Higher RPM and higher feed rates
  • Standard toric cut + Balancing = Long reach milling

For optimizing purposes, this is tremendous, since you can run the same diameter at 50% higher RPM, and therefore a 50% increase in feed rate while maintaining the same chip load. So, if you have a roughing operation in your current program that uses a 6mm single flute end mill, at 32,000 RPM and 2 meters a minute, replace the end mill with a balanced unit of the same size, and you can bump up your RPM and feed rate by 50%.

Just as well, if you have a situation where you need to mill a deep pocket, these tools can be a life-saver. Take this vacuum adapter we made:

This balanced CNC tools sample is an aluminum vacuum adapter with deep pocketing milled with a specially balanced single flute end mill.
This vacuum adapter was made using a specially balanced single flute end mil for deep pocket milling.

At 1.75” deep, a 10mm balanced single flute had no problem removing all material from the inside of the cavity as well as cutting the part out on a vacuum table and left no chatter marks. DATRON offers balanced end mills that go over 3” deep, so you’re not too limited on what you can accomplish.

So, on your next project, consider a balanced end mill for your all your roughing, finishing, or deep milling needs.

 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

5 Tips for Holding Small Parts on a Vacuum Table

Vacuum tables or vacuum chucks can be used to hold sheet materials and small flat workpieces during the CNC machining process.

So, if you’ve been reading this blog, or cruising through our website, then I’m fairly sure you’re aware that we make an extremely capable CNC vacuum table. It’s the must have fixture for many industries – rapid prototyping, signage, front panels, etc. Where the vacuum table can truly shine is holding very small parts.

I once ran a demonstration for a prospective customer that showed that you can cut an entire 12” x 18” sheet of 0.020” thick aluminum into 6mm discs without having any of them fly off the vacuum table. See video below as an example. You can see that the last cut on the perimeter of these small parts goes through the sheet material exposing our VacuCard paper that sits between the sheet stock and the vacuum table – serving as a sacrificial layer that allows you to cut through the workpiece but not into the top of your vacuum table.

With all of this being said, vacuum tables are an excellent workholding solution, but they require a certain approach to get the most out of them.

1) Vacuum Table with Regular or Dense Hole Pattern?

Vacuum table tops in both regular and dense hole pattern to hold very small parts even after they are milled free from the sheet material.
Vacuum Table Tops can be ordered in the standard hole size (right) or in the dense hole pattern (left) which is designed to hold particularly small parts without having them fling off the table when they’re milled free of the sheet material.

The first defining feature of our vacuum tables is the density of the vacuum holes. We have two patterns, regular and dense. The regular pattern is well suited to most of our applications, but when you get down to parts smaller than a square inch, or a more difficult to cut material, a dense hole table is a good choice. The key to the dense hole plate is having more than twice as many holes as a standard plate, thus allowing better suction on smaller parts.

2) Use Vacuum Table Paper

Vacuum table paper called VacuCard is used as a sacrificial layer that allows you to cut completely through the stock without damaging the surface of your vacuum table.
Vacuum table paper known as VacuCard is air permeable but thick enough to allow you to mill through the workpiece without milling into the surface of the vacuum table.

The next step may seem like a no-brainer, but it’s especially important for very small parts. Once a piece of our vacuum table paper (known as VacuCard or VacuFlow) has been cut into, it becomes ineffective for smaller parts. Cuts in the paper allow a path for air to leak by, as well as leave a raised edge that prevents the material from sitting flat on the table.

3) Vacuum Table Strategy

Vacuum table strategy employs both tabbing and onion skinning methods to reduce cutting force so that the part stays fixed to the vacuum table.
Vacuum table strategy includes both onion skinning and tabbing methods to limit cutting force so that the workpiece stays on the vacuum table.

One of the single most important methods of holding small pieces on the vacuum table is your strategy. If you are a little too gung-ho and try to take out a small piece in one pass, you’ll likely have cutting forces too high for the vacuum to overcome. I always recommend two methods; Onion Skinning or Tabbing. Either one works quite well, simply leave a small amount of material at the bottom of your piece to take out at the end of the operation. This will greatly reduce cutting forces and prevent unnecessary scrapping of parts.

4) Tools for Use with a Vacuum Table

Vacuum table tool selection is made based on the required cut but the smaller the better because smaller tools reduce cutting force.
Vacuum Table tool selection obviously is made based on the required process or cut, but in general, the smaller the better … and consider downcut tools for finish cuts.

Use a carefully picked tool in conjunction with step 3 to increase your likelihood of success. My weapon of choice is typically an end mill that is a third the diameter of my original tool, combined with a high RPM and moderate feed rate. With such a small tool, your cutting forces reduce even further to prevent movement of the material. For very stubborn pieces, consider using a down-cutting end mill for finish cuts. Downcut tools push the material down while milling, instead of pulling up, which helps small pieces stay-put.

5) Mill Recessed Areas in Vacuum Table Sacrificial Layer

Vacuum table sacrificial layer like this MagicBoard allows for cavities to be milled to hold parts that are not completely flat or to add side support for flat parts.
Vacuum table sacrificial layer that can be milled with recessed areas so that your part is held in place by vacuum suction as well as physical support on the sides of the workpiece.

So, your part just isn’t holding, you’ve done everything you could, but it’s not happening. Don’t worry. There’s hope. First, to get the part to a state where it will hold on the vacuum table – you may need to leave some material, but that’s OK.  Next, get yourself some MagicBoard, or a porous aluminum. Both have excellent machinability, rigidity, and the ability to let vacuum flow through them. Take either of these materials and mill a cavity into it to retain your part. Now you have physical support on the sides to prevent part movement, which allows you to cut very small parts, very quickly.

So, that’s pretty much it. With a lot of practice and a little patience, using these basic guidelines will find you well on the path to machining some very intricate parts on a very small scale. To learn more about DATRON vacuum tables and other workholding accessories feel free to download this brochure.

Download CNC Workholding Brochure:

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:

AUTODESK Fusion 360 CAM Challenge – DATRON’s Adrian Montero Wins Best Surface Finish

Fusion 360 CAM Challenge won by DATRON's Adrian Montero using a DATRON neo high speed milling machine.

When an Autodesk Fusion 360 Product Manager put out a “key chain challenge” to see who could produce the best quality sample part, many CNC machinists on social media took note and got right to work.

Fusion 360 part being programmed with Autodesk Fusion 360 CAM software by Datron's Adrian Montero.
Fusion 360 Part being programmed by DATRON Application Technician, Adrian Montero.

Appropriately named the AUTODESK Fusion 360 CAM Challenge, participants were asked to produce a Fusion logo made into a key chain.  Autodesk supplied all participants with the same file in their software. There were only 3 requirements to the Autodesk Fusion 360 CAM Challenge:

  • Use Autodesk Fusion 360 to program
  • Take a photo of yourself programming the part
  • Supply a photo of the final end product
Fusion 360 CNC milling performed on DATRON neo high speed machining center.
Fusion 360 CNC milling challenge on DATRON neo, compact high-speed mill.

All participants of the Autodesk Fusion 360 CAM Challenge were given 1 week to complete their sample parts and submit their photos. In that week 56 people participated and tagged 152 photos that were viewed by 129,000 people.

Fusion 360 CNC machining challenge won by Adrian Montero who used a DATRON neo high speed milling machine.
Original Fusion 360 key chain next to the one milled in acrylic on a DATRON neo by Adrian Montero.

DATRON Dynamics Application Technician, Adrian Montero won the Autodesk Fusion 360 CAM Challenge in the Category of Best Surface Finish. His part was machined on the DATRON neo, compact high-speed milling machine.

Learn more DATRON neo download the brochure:

Nameplate Manufacturer Calls DATRON Source of Efficiency

Nameplate milling and engraving at Willington Nameplate is performed with DATRON high speed milling machines

Willington Nameplate in Stafford Springs, CT manufactures metal engraved nameplates and Identification tags for a wide range of customers from aerospace and defense to Gillette Stadium – they actually produced all of the seat tags for “Casa de Brady”. Their metal nameplates and ID tags are made from a range of materials including aluminum, brass and stainless steel.

Willington Nameplate was founded over 50 years ago by Marcel Goepfert and day-to-day operations have been run by his son, Mike Goepfert, since 1990. Since that time, there have been many changes and a lot of growth. This includes a critical decision in 1999 to purchase their first DATRON high-speed milling machine.

Nameplate milling including control panels, data plates and dials is performed at Willington Nameplate on their DATRON high speed machining centers.
Nameplate milling at Willington Nameplate includes control panels, data plates and dials.

Willington Nameplate’s Fabrication Group Leader, Jamie Vale Da Serra, recounts this story saying that, “Prior to installing the DATRON machine we used a manual kick process.” He goes on to say, “We needed to get away from that process because we needed a tolerance higher than .005”. Vale Da Serra refers to the DATRON milling machine as a “set it and forget it” piece of equipment that runs unattended freeing up staff to attend to other tasks.

Nameplate engraving and milling at Willington Nameplate is performed on DATRON high speed milling machines that can run unattended.
Nameplate machining by Willington Nameplate is optimized by DATRON features like vacuum chuck workholding, probing and automatic tool change – resulting in their ability to run this machine unattended.

Quick job setup and the ability of the DATRON machine to run unattended are the result of a number of integrated features – all operating in concert. This starts with integrated vacuum table or vacuum chuck technology that allows the operator to quickly setup the workpiece – for nameplates this is generally sheet material such as aluminum, stainless steel or Metalphoto®.  An integrated probe for part location and measurement also speeds up job setup and enables uniformity by automatically compensating for material irregularities like surface variance. An automatic tool changer with an integrated tool-length sensor provides a full stable (and wide variety) of necessary tooling that can automatically be changed at given intervals and/or when a tool is broken.

Nameplate machining by Willington Nameplate is done with their DATRON CNC mills and produces labels, tags and UID marked nameplates.
Willington’s nameplate machining yields labels, ID tags and UID marked tags.

Vale Da Serra says, “Consistency is there with the DATRONs from the first to the last they all measure the same, whereas with the manual process human error is possible that could give you a deviation.”

The growth at Willington Nameplate is not limited to adding DATRON machines, the company has recently purchased three other companies in New England, thereby expanding sales by 35% in five years. With a staff of more than 80 people, Willington Nameplate has now set their sights on additional acquisitions elsewhere in the United States.

Learn more about Nameplate Production download the White Paper:

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: