6 Tips for Holding Tight Tolerances

Holding tight tolerances when CNC machining is a challenge that can be mastered with these tips.

There are few things that a machinist likes more than when they get a print and see this: +/- 0.005”. Holding five thousandths of an inch is child’s play for any good machinist – they might as well mill the part with their eyes closed. But, then there are those jobs that are a bit more demanding. Add another zero, and now you’ve got: 0.0005”. Holding five tenths of a thou is a whole different story. It’s the difference between the thickness of a human hair and a white blood cell. When it comes to holding tight tolerances, here’s a few recommendations that can keep your parts in spec.

Spindle warm up and warming up your CNC machine in all axes helps in holding tight tolerances.
Spindle warm up and a warm up routine can help in holding tight tolerances when machining.

1. Spindle Warm Up for Holding Tight Tolerances

Run a warmup routine – While this is standard procedure with most CNC machines, consider running something a bit more strenuous. A typical procedure will only warm up the spindle, which is critical for spreading grease to prevent premature bearing wear. But, you also need to allow the internal components to reach a steady operating temperature to account for thermal expansion. Now, all of this is fine if you’re only looking to hold tight tolerances in your Z axis, but if you combine the spindle warm up with machine movement in all axis, this will help even further. Allowing the machine to run for 10-20 minutes with all components moving allows for the components to reach an ideal temperature, and will help mitigate the effects of thermal expansion during milling. No matter what, at the end of your warmup, make sure to measure all your tools for absolute precision and holding tight tolerances.

Tool selection can be a factor in holding tight tolerances.
Tool selection can be a factor in holding tight tolerances. Use your roughing tool for the “heavy lifting” so that the finishing tool exhibits less wear and maintains precision.

2. Tool Selection for Holding Tight Tolerances

Choose your tools carefully – When you’re dealing with these unforgiving tolerances, be sure to be accommodating with your tooling. You’ll want to make sure to have specific tools for roughing and finishing, allowing the roughing tool to take the brunt of the wear, while the finishing tool is saved for only the final passes, will ensure a repeatable process for creating accurate parts.

Gauge pins are a handy tool in holding tight tolerances in that you can machine an under sized feature and then dial it in.
Gauge pins can be used measure an under-dimensioned feature before machining it to an exact size.

3. Compensation for Holding Tight Tolerances

Compensate your tools – Tool manufacturers aren’t perfect, so they engineer their tools to be a little forgiving. They know that if you’re going to make something using their tools, you’ll be a lot happier if the feature it cuts comes out under-dimensioned instead of over-dimensioned. Just like a haircut: you can take more off, but you can’t put it back on. Knowing this, you’ll want to make sure the first thing you do when setting up a precise job is to dial in your actual tool diameter. You can do this several ways, but my preferred method is to mill a feature and then use accurate tools to verify the dimension – gage pins or blocks work well for this. It’s easy – if you interpolate a 0.250” hole with a 0.236” tool and only a 0.248” gage pin will fit, then your tool is undersized by 0.001” (use half of the value since it is undersized on each side). You would compensate your size to 0.235” at this point, either through your CAM software or utilizing Tool Comp commands in your cut file.

Temperature sgould be considered if holding tight tolerances is critical in your manufacturing.
Temperature impacts accuracy due to thermal growth. So, be mindful of your environment and machine location.

4. Temperature for Holding Tight Tolerances

Thermally Stabilize – This is one of the most important things on this list for holding tight tolerances because it can make a huge difference and you may not even notice it. Pay attention to where your machine is located. Is it near a window, if so, does the sun shine on it during parts of the day? Does the AC kick on in the afternoon and blow cold air on the machine cabin? Is your material kept a sweltering warehouse, then brought into a chilly 68° environment? These all seem innocent but can create a huge headache in your process. Thermal expansion or contraction of the milling machine or the material you cut can create large variances in your process. Put these all on lockdown – keep your machine and material in a temperature controlled climate, unaffected by sunlight, and you will reap the rewards – consistency in your process.

Ball bar testing and frequent machine calibration help in holding tight tolerances.
Ball bar testing and regular calibration of your machine will help in holding tight tolerances.

5. Calibration for Holding Tight Tolerances

Calibrate your equipment – When you’ve done all of the above but you need it to be just *that* much tighter, consider calling in the manufacturer. After a machine has been built, shipped, dropped off a truck, moved around, leveled, and used for thousands of hours, things will shift and settle. It’s unavoidable. Luckily, there are several pieces of equipment, be it granite squares or the Renishaw Ballbar, that can help pull the reins in on your loosened-up machine to help in holding tight tolerances. We like to perform a ballbar test and make adjustments as part of a yearly maintenance, that way you can keep a tight leash on your machine accuracy. Also, performing these annual services ensures that bearings are tight and lubricated, belts are properly tensioned, and drive motors are healthy – all important factors in having an accurate machine.

Linear scales assist in accuracy and holding tight tolerances.
Linear scales add to a machine’s precision and consistency in holding tight tolerances.

6. Linear Scales for Holding Tight Tolerances

If all else fails, scales! – If you have done everything on this list, and you still struggle, it may be time to consider getting a machine with linear scales. Your typical CNC machine will use the drive motor encoder as the primary method for keeping track of its absolute position, but this can be flawed due to imperfections in the ball screw or thermal discrepancies. Linear scales change all that – typically installed at the factory, they consist of two main components – the scale, and the read head. Put simply – the scale is like a highly accurate ruler that the machine can read, constantly comparing and adjusting for deviations. On our M10Pro, this allows for a 25% tighter positioning tolerance, a 20% improvement in repeatability, and a 85% reduction in backlash..

Use the DATRON M10 Pro to assist in holding tight tolerances in CNC milling applications
The DATRON M10 Pro features linear scales for added precision and accuracy.

Hopefully, these tips will help guide you well down the long, winding, bumpy (but still rewarding!) road of high-precision machining and holding tight tolerances.

Learn More about the DATRON M10 Pro:

Download DATRON M10 Pro Brochure

Slow to Fast Feed Rates for Single Flute End Mill

Feed rates for single flute end mill are detailed in this DATRON Blog.

Machinists ask me all the time, “When do I go fast and when should I go slow with a single flute end mill?” Well, as you can imagine, there are a lot of variables at play regarding feed rates for single flute end mill, but let’s try to break it down.

I’ll use one tool for reference, but the results should be easily scalable amongst the rest of our tools. Let’s say you’re using a DATRON 68806K Single Flute End Mill (aka. 4-in-1 wiper flat) to machine a piece of 6061 aluminum. There is a variety of jobs you can accomplish with this tool, but each will have a different feed for a different reason.

The single flute end mill is very efficient in evacuating chips which allows for very high feed rates.
DATRON Single Flute End Mill: exceptional for efficient chip evacuation and high feed rates.

Slow Feed Rates for Single Flute End Mill

Slow (60″/min) – Finishing – If you need an exceptional quality in the finish of a floor or wall, it helps to slow the machine down to take a fine chip and decrease cutter load/cutter deflection.

Use slower feed rates when using a single flute end mill for finishing especially if great surface finishes on walls and floor are required.
Feed rates for single flute end mill when Finishing: for superior surface finishes on the walls and floor of a pocket, slower feed rates are suggested.

Medium Feed Rates for Single Flute End Mill

Medium (120″/min) – Slotting – Something a single flute does particularly well is slotting, which is a tool path that has 100% of the tool diameter engaged in the material. Using a proper depth cut (25% of tool diameter), you can cruise along at a decent pace without worrying about clogging up on chips.

Medium feed rates are suggested when slotting with a single flute end mill
Feed rates for single flute end mill when Slotting: With 100% of the tool diameter engaged, medium feed rates are beneficial.

Fast Feed Rates for Single Flute End Mill

Fast (180″/min) – Traditional Roughing – When you are using a normal milling strategy, in the range of 33-50% depth of cut (2-3mm) with a 50-70% stepover, you can be fairly safe kicking the speed up, just keep an eye on your spindle load.

When roughing with a single flute end mill you can safely run with fast feed rates.
Feed rates for single flute end mill when Roughing: In the range of 33-50% depth of cut you can dial up the speed.

Very Fast Feed Rates for Single Flute End Mill

Very Fast (240″/min) – Trochoidal Roughing – If you are using Mastercam (Dynamic milling) or Fusion 360 (Adaptive clearing) you may have heard of this strategy before. Instead of going about the traditional method, this method utilizes more of the flute to boost efficiency. For instance, we could use 100-200% depth of cut (6-12mm) with this strategy because our stepover would be decreased to 10-20%. In many cases, this prolongs the life of the tool and puts less strain on the spindle, so you can safely bump the feed rate up.

Very high feed rates can be used when performing dynamic milling using a single flute end mill.
Feed rates for single flute end mill when Trochoidal Roughing: Very fast feed rates can be used when performing dynamic milling.

Extremely Fast Feed Rates for Single Flute End Mill

Extremely Fast (300″/min) – Shallow roughing – If you are taking off less than 10% depth of cut (0.60mm), then you should be safe cranking the feed way up. With such a shallow cut, you won’t have to worry about overloading the tool or spindle.

When shallow roughing at less than 10% depth of cut you're safe to dial up the feed rate.
Feed rates for single flute end mill when Shallow Roughing: If you’re taking less than 10% depth of cut, let ‘er rip!

 Download Cutting Tool Catalog

Drill vs. End Mill? – Some Basic Guidelines.

When to use a drillvs an end mill is a question that machinists often ask. here are some tips/

Question: “Should I use a drill vs. end mill?” DATRON Application Technician, Dann Demazure answers, “It depends on what you’re trying to achieve.

When to Use a Drill vs. End Mill

Drill vs. End Mill is a question asked by many machinists and Application Technician, Kevin Mulhern has some answers.
Drill vs. End Mill? If you need to make a lot of holes a drill is probably the way to go.

If you’re making a very small hole, say, less than 1.5mm in diameter, go with a drill. End mills under 1.5mm become increasingly fragile, and subsequently cannot be run as aggressively, as a drill can be.

If you need to make a very deep hole – in excess of 4x your hole diameter, choose the drill. Past this point, chip evacuation can become very difficult with an end mill, which will quickly wreck your tool and your part.

Are you making a lot of holes? Drilling is probably the way to go. In most instances, a drill will best the fastest time you can achieve with an end mill.

Need to make an extremely precise hole? While milling is typically perfectly acceptable, sometimes the tolerances require a drill and a reamer for the perfect finish.

When to Use an End Mill vs. Drill

However, there’s a lot to be said for using an end mill instead.

Drill vs. End Mill? The End Mill is your choice when you have to make a lot of different size holes.
Drill vs. End Mill? If you need to make a lot of different sized holes, you should probably go with the end mill.

Need to make a big hole? Big holes need big drills and lots of horsepower, this is where helical milling shines. Use an end mill that’s 60-80% the diameter of the hole you’re making to quickly clear out while leaving plenty of room for chips to escape.

Print calls for a flat bottomed hole? Normal drills can’t do that, so you might be better off milling the feature.

Making lots of different size holes? Try to use the end mill, you’ll save time on tool changes and room in your tool changer.

Rapid prototyping? End mills will be appealing for their flexibility. Being adaptable to take on some features that may normally be drilled means you can spend less time CAMing a part and more time making chips.

With either one, there are two simple rules to remember:

Break your chip – don’t try to be a hero and blast through your hole in one go, program a quick retract to get the chip out and let the coolant in.

Turn up the coolant – unless you have through tool coolant, you’re going to want to be sure to turn up the coolant flow and decrease your air pressure. The coolant needs to be able to flow into the hole during your retract.

 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

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:

CNC Milling Laminated Shims

Milling laminated shim with a high speed CNC machining center featuring vacuum workholding and a 40,000 - 60,000 RPM spindle.

Let’s face it, some materials are just no fun. Inconel, hardened steels, ceramics. Everybody likes a material that will cut like a butter, and a typical dread is associated with stuff that doesn’t. So recently, we were presented with a material in the latter category. Milling laminated shims from stainless steel sheet stock.

Everyone we asked had a similar reaction. “Stainless shim stock? That stuff sucks.” And there were many reasons. Delamination during machining, enormous burrs, difficult fixturing. General misery.

Milling laminated shims out of stock like this laminated stainless steel sheet material is best handled using a high speed CNC milling machine with vacuum table workholding.
Milling laminated shims from stock like this laminated stainless steel can present some challenges.

So when addressed with this difficult task, I cringed a bit, and got to work. Luckily for us, DATRON’s technology is a perfect fit for machining shims. But why?

Vacuum Workholding is Ideal for Milling Laminated Shims

Your typical shim machining fixture looks something like this; A base plate, a layer of adhesive, a layer of shim stock, another layer of adhesive, then a sacrificial layer of aluminum on top to prevent delamination. Needless to say, setup takes a long time, and break down takes even longer. With our vacuum table fixturing, the setup is bit more manageable; the vacuum table, a layer of vacuflow sheet, then shim stock. Done. Probe the material and go to town.

CNC milling laminated shims with a high speed machining center equipped with vacuum table workholding for quick setup.
CNC milling laminated shims can be an easier process by using vacuum table workholding. This photo shows how it works.

High RPM Spindles for Reduced Chip Load When Milling Laminated Shims

With a typical VMC, RPM does not get too high. Maybe 10,000 RPM. The issue with this is the cutting forces being applied. Let’s consider a 1.5mm double flute end mill, cutting a part at 10,000 RPM, at 60 inches a minute. That ends up being a 0.003” chip load. That is a problem, and it’s also the reason delamination is so prevalent in shim machining. Cutting forces are too high. Using the same tool at the same feed rate, but at 30,000 RPM, we just reduced our chip load to 0.001”, bringing the cutting force down by 2/3. This is what allows us to cut the shim stock without a sacrificial top layer, thus saving time and aggravation.

Milling laminated shims using a 40,000 - 60,000 RPM spindle helps to reduce chip load which prevents delamination.
Milling laminated shims with reduced chip load is achieved with a 40,000 – 60,000 RPM spindle.

Milling Laminated Shims – Clean and Accurate

There are other methods of cutting shim stock, obviously. Some work better than others. Laser cutting can have issues with welding layers of material together. Waterjet can manage it, but the tolerances aren’t really there, requiring machining after the fact. This is where a DATRON can shine. With high speed machining, edges come out clean and burr free, and tolerances come in within 0.001” (over the work envelope). The benefits here are significant; remachining, cleaning, deburring, can be cut down tremendously, allowing you to move on to the next job.

Now that doesn’t sound so bad, does it? Next time you’re dealing with a problem child like shim stock, give us a call, we can help.

Learn more about vacuum tables – download the data sheet:

Halftone Engraving on a CNC Machine

Halftone engraving of a DATRON M8Cube high speed milling machine that is actually made on the M8Cube milling machine.

When you get to work with a DATRON every day, you get to see some pretty cool things. There are so many cool things to observe, or be involved in, that you can become a little numb to just how cool these things are. So, every once in a while, it’s good to stop and look back at what you’ve been doing and take a second to appreciate it. In this case, it’s halftone engraving.

I thought this might be a unique topic to share with you, the reader, so you too can enjoy the cool things you can do with your CNC machine (hopefully a DATRON!).

What is a Halftone?

First, a little background on our subject. A halftone image, according to Wikipedia, is “the reprographic technique that simulates continuous tone imagery through the use of dots, varying either in size or in spacing, thus generating a gradient like effect.”

Halftone engraving is the simulation of a continuous tone image using dots that vary in size or distance.
Halftone engraving is a reprographic technique simulating a continuous tone image.

Essentially, the trick behind a halftone image is to use varying size dots to create a grey scale image. It’s comparable to some comic book printing or pointillism, but is a bit unique.

Halftone engraving using different size dots milled into the surface of blue sheet material (with a silver surface finish) to create a grayscale.
Halftone engraving on blue sheet material with a silver surface finish requires milling varying size dots to create a grayscale image.

Halftone Engraving Software (Free)

Now, let me introduce you to Halftoner, a free application created by Jason Dorie. It allows you to easily import any image and not only convert to a halftone image, but also apply a tool path to it at the same time. The elegance of this software comes from its simplicity; first, import an image and choose your values for minimum and maximum dot size, dot spacing, dot offset, etc… Then determine your milling values; retract height, minimum depth, feed rate, RPM, and so on. One of the most important values for Halftoner is the tool angle, since it will take the included angle of your tool to determine the necessary depth to make a certain size of dot. It’s really quite intuitive.

Once that’s all done, click “Write GCode” and voila, you’ve got a program ready to go.

Engraving halftone images with a DATRON high speed machining center and a free application called Halftoner.
Engraving halftone images with a high speed CNC milling machine can be done easily with a free application called Halftoner.

I was fortunate enough to get to play with this for a while on a recent project, and the outcome you get for a minimal amount of effort can be very impressive.

Engraving halftone graphics on an engraving machine requires the engraving of different sized dots that reproduce a graphic by simulating a continuous tone image.
Engraving halftone images is quick and fun using a high speed milling and engraving machine like the DATRON M8Cube.

Want more info on engraving? – Download Engraving Brochure

6 Easy Ways to Optimize CNC Program

Optimize CNC Program with tips and directions provided by DATRON Applications Engineer Dann Demazure in this blog.

“Optimize CNC Program” – it’s the instruction you hear in your head when you’ve finished a machining program. And it can be an arduous process that, if you’re like me, you slave over. Typically a bit too much, wasting a lot of time on changes that don’t add up to a substantial improvement. As we all know, time is money, so, I’ll try to relieve you of some of the labor of revamping your program. Here’s a list of quick, easy, and effective tweaks for your DATRON programs.

Optimize CNC program tips and detailed instructions in this blog by Dann Demazure from DATRON Dynamics.
Blog Author and DATRON Applications Engineer, Dann Demazure, optimizing a CNC milling program.


Optimize CNC Program Tip 1 –  Leave the coolant on

It may not sound like much, but this gain can really add up. If you’re using coolant in your program, consider switching it from the Positioning/Cutting feed setting from Cutting <0>, to Travers<1>. You may not easily perceive it, but there is a very brief dwell programmed into the software so that the coolant has time to begin spraying. This change in the command will leave your coolant spraying between positioning movements, thus avoiding the initial dwell. Now, each dwell may only last 1/10th of a second, but if you have 200 retracts in your program, you just shaved 20 seconds of your program, and that’s not nothing.

Optimize CNC program by leaving the coolant running during positioning movements to avoid the initial dwell.
Optimize CNC program by leaving the coolant spraying during positioning movements.


Optimize CNC Program Tip 2 – Ramp

If you’re cutting along a contour, consider changing your method. If you are currently doing depth cuts, try a ramp instead. A ramp keeps the tool engaged in your desired amount of material throughout (except for the very beginning and the very end), and has no retracts. Let’s say again that your part has 200 retracts cutting contours on 20 different features (10 retracts per feature). By ramping, you’d bring that number down from 200 to 20 (final retract), and if each retract takes half a second, you just saved 90 seconds.

Optimize CNC Program Tip 3 – Be smooth

If the devil is in the details, then small contours are your devil. If you’re doing intricate engraving or 3D contouring, then you’ve probably noticed that the machine will slow down to follow all contours tightly. It’s just following orders, but if you have a little leniency in your adhesion to contours, Smoothing can make a huge difference.

Optimize CNC program with smoothing functions to clean up jagged geometry for a tighter milling path.
Optimize CNC programs using Smoothing functions like PerfectCut to smooth jagged geometry. See the results in red above.


Smoothing will take jagged geometry, like what is pictured above (purple), and apply arcs to the contour to create a smooth, more continuous motion (red). Not only does this have benefits for surface finish, but since the machine doesn’t need to slow down nearly as much in an arc as compared to a vector, time savings can be abundant. And utilizing it is as easy as writing the code in your macro, editing the preset values (which work well for most things), and pressing the “Go” button.

Optimize CNC Program Tip 4 – Be dynamic

I’ve talked about dynamics at length before and all the benefits from using them to fine tune a process for speed optimization and ideal surface finish, so why am I mentioning them again? Easy, besides the fact the dynamics settings are one of the easiest ways to reel in cycle time, adjusting them in conjunction with smoothing yields even better results. A high dynamics setting combined with a smoothing filter means that a very minimal amount of deceleration is needed to turn a corner quickly, thus cutting your cycle time even further.

Optimize CNC Program Tip 5 – Get low

This is usually a gimme, but it takes about 10 seconds of your time to change your retract heights from 0.5”, to 0.050” (or lower). Minimizing your retract height won’t save you much time per retract, but think of the big picture. Even if you only saved 5 seconds per part, if you’re making 20,000 parts per year, you just saved over a day of machine time. Every second counts.

Optimize CNC Program Tip 6 – Keep your tools in order

It seems obvious, but try to keep your operations organized so that when a particular tool is done, it never gets used again in the program. Sometimes this is unavoidable, but each tool change will cost you somewhere around 15 seconds of time. Consider using combination tools to cut down on tool changes. Most importantly, if you have parts nested, use tools sequentially rather than by part. If you have to cut 24 parts, and each part uses 4 tools, you’ll either spend 24 minutes changing tools again and again, or 1 minute changing all the tools once.

If you’d like more information on the PerfectCut Smoothing mentioned in Tip 3, Download the Data Sheet by filling out the form below:

Download Optimizing CNC Program Smoothing Tip #3 Data Sheet

How to Save Time and Money with Combination Cutting Tools

Combination cutting tools from DATRON save time through their ability to perform multiple functions with one milling tool.

So, you’re cranking out parts on your machine at a steady rate. The orders are being filled and the boss is happy. Life is good.

But, if you’re like me, you’re still agonizing over the seconds that could be saved. I’ve talked before about the benefits of Dynamic settings to decrease cycle time and increase surface finish quality, but then what? One surefire way to save some time in your process is to decrease tool changes. After you’ve organized the order of your operations to minimize tool changes, things have improved, but what if we could exchange two tools in place of one? Well, luckily, DATRON has the same thing in mind.

Combination Cutting Tool – DATRON Milling Thread Mill

Combination cutting tool that combines milling of holes with threading those holes in a single action with not tool change required.
Combination cutting tool for milling and threading holes.

Meet the Milling Thread Mill. The name may sound redundant, but there is a big reason why. Before the outer flutes take care of the task of cutting the threads, the three flutes at the tip remove all the material in your way. By comparison to standard thread milling, this not only saves you the time of changing the tool from a drill/mill to a thread milling tool, but also the time spent removing that material in the first place.

A combination cutting tool made by DATRON mills holes and threads them in one pass, thereby eliminating a tool change and time associated with drilling holes with one tool and threading them with another.
A combination cutting tool from DATRON cut the hole and thread it in a single pass.

Consider this: This piece above, for example, has ten M6x1.00 threaded holes. Using a 3 mm single flute end mill and a M5-10 thread mill, it is taken care of in 3 minutes and 20 seconds. However, the same part done with the Milling Thread Mill blasts through in just 1 minute and 11 seconds. That’s 20 seconds a hole versus 7 seconds a hole, a 65% improvement! Apply that to your thread-heavy application and you’re looking at a considerable benefit in the long term (especially if you’re hand threading after the fact!).

Not to mention that since you’re not using two tools to accomplish one task you’re saving on tooling cost as well as adding useable life onto other tools. It’s a win-win. Now watch it in action:

Combination Cutting Tool Video (Milling and Threading Holes)

Combination Cutting Tool – DATRON Milling Countersink Tool

Combination cutting tool for producing holes and countersinks at the same time without a tool change.
Combination cutting tool for milling and countersinking in one process … without a tool change!

This combination tool is well suited to front panel applications, but is also handy elsewhere. When many holes need a countersink, this tool combines both operations into one quick operation. With a single flute end mill at the tip and a single angled flute at the shoulder, both operations can be taken care of quickly. It is not limited to just countersinking however, as you can also use it as a chamfer tool to de-burr edges or mill appealing bevels.

Combination cutting tool for milling holes and a countersink in one action to eliminate the need for a tool change which saves time and money.
These holes and the countersinks were made with a single combination cutting tool.

For example; This simple part has 5 countersunk holes and a chamfered perimeter. When cut the typical way, a 3mm single flute end mill clears out the holes, while a 45 degree countersink takes care of the rest. This is accomplished in 1 minute 22 seconds.

When using the combination mill though, the holes and countersink are created at the same time, and the perimeter is beveled without the need for a tool change. Thanks to this small change the cycle time improves the 45 seconds, which is about 45% quicker than before.

So next time you find yourself chasing down seconds, take a look at DATRON tooling, and you might end up saving minutes.

Learn More: Download the DATRON Cutting Tool Catalog:

Cycle Time vs. Surface Finish

Cycle Time vs Surface Finish in CNC milling is a never-ending consideration for machinists and this blog sheds light on dynamics as the means of balancing the two.
Cycle Time Vs. Surface Finish is a deliberation encountered by machinists every time they use a milling machine or machining center to produce a new part. This blog discusses dynamics as a means of balancing the two when using a DATRON high speed CNC milling machine.
The never-ending deliberation … Cycle Time Vs. Surface Finish

For most machinists, it’s a constant quandary, cycle time vs. surface finish? Do I optimize for a perfect surface finish or a minimized cycle time? I know I’ve personally spent hours of programming time in order to shave off precious seconds of cycle time. The reality is that in this day and age, you probably can’t completely sacrifice one for the other (cycle time vs. surface finish) because demand will always be high for both. So, if you’re like me, you’ll ramp up the feed rate, organize the tool changes, minimize retract height and optimize the cut path … and that’s gotten you close … but not close enough. So now what?

Well, good news … dynamics is here!

Ok that may sound a bit boisterous, but there’s good reason for the excitement. To understand why, you have to understand dynamics and we feel that our good friends over at CNCCookbook do a great job of explaining when they say:

“The ability to control the machine’s contour dynamics is a bit like the ride control on a modern high performance car’s suspension: do you want a comfortable ride, sporty, or full race?”

I like to think of it switching from a jackhammer to an exacto-knife, but you get the idea. There’s three main parameters at play in a dynamics adjustment:

Circle resolution: The fineness of movements in an arc.

Acceleration: The change of velocity over time.

Jerk: The rate of change of acceleration.

So using a DATRON high speed milling machine as an example – dialing down these values in Dynamic 1 within the control software, we get the most precise movements with the most gentle acceleration ramp, which leads to the best surface finish possible. First, however, you need to rough out that part and this is where Dynamic 5 shines. At over 4 times greater values than in Dynamic 1, the time advantage you can gain is significant.

I’ll illustrate the range between Dynamic 1 and Dynamic 5 by milling the part below.

Cycle Time vs Surface Finish balanced using dynamics settings in the CNC machine program to achieve optimal results.
Aluminum part programmed to illustrate the difference between dynamics settings.

On Dynamic 1 you can mill one of these parts every 8 minutes 40 seconds Not bad, but on Dynamic 5, each part is milled in 6 minutes 3 seconds. In both instances, the spindle speed is 40,000 RPM and the feed rates are 4 m/min. with a 6mm single flute end mill and 3 m/min. with a 3mm single flute end mill. So the only variable is the Dynamic setting.

What is really great is that unlike the more time consuming portions of program optimization, adjusting these settings is as simple as typing “dynamics” in your editor and selecting 1-5.

So, if you’re perplexed by the cycle time vs. surface finish dilemma it’s time to consider Dynamics. Dial it in and enjoy the best possible of both worlds.