Mechanical Fabrication of Printed Circuit Boards (PCB)
Fabricating printed circuit boards (PCBs) using electrochemical imaging / etching techniques is a well understood, and reasonably straight forward process. Surprisingly complex and precise ciruits can be made with relatively inexpensive equipment and consumables. The problem, of course, is that most of the chemicals involved are pretty nasty and are difficult to dispose of (unless you live in California, where they are impossible to dispose of). This is where mechanically etching PCBs comes in.
With mechanical etching, there are no nasty chemicals to handle and dispose of. No need for darkrooms, UV exposure systems, or negative film printers. Basically, all that is needed is a computer controlled (CNC) router, speciliazed layout software and the right set of tools. Although mechanical etching cannot yet make printed circuits as complex as conventional processes, advances in low-cost CNC systems, design software and solid carbide cutting tools have extended the capabilities of this technology to the point that, in our estimation, it is finally ready for primetime.
In spite of the advances, making PCBs by cutting away areas of unwanted copper can be surprisingly difficult and downright frustrating. This is due in part to the copperclad boards that comprise the feedstock of the process. Copperclad, when properly made, is a precision laminated structure with a fiberglass (or ceramic, or teflon, or paper phenolic, or ...) core coated on one, or both, side with a thin layer of annealed electrolytic copper foil. The first problem that you encounter is that, for some unholy reason, all of the best substrate materials seem custom made to destroy even the best made tools. Forget about high speed (HSS) and cobalt steels . To achieve any kind of decent life expectancy, tools have to be made of carbide, diamond, or some combination of the two. The second major hurdle is that, annealed copper loves to smear and/or tear when it is being cut. It is also very abrasive and requires properly designed and fabricated tools to machine it without leaving a myriad of tiny, and not so tiny, "hairs" that all conspire to create nearly invisible shorts in the worse possible places in your circuit design. The bottom line is that, to make a reliable circuit, in an acceptable amount of time without descending into psychoses, you have to use tools designed specifically for the task, not bargain basement drills and cutters found in the dark recesses of the web. That is not to say that there are not some good deals out there. There very definitely are! You just have to know what you are buying and how to recognize a good tool when you see one.
And that, in a nutshell, is why we have written the following. Click below for information on each proces / tool type.
True spiral 2-flute "V" point mechanical etching bits offer an optimum combination of high resolution cutting and tip strength. The plunge style tip geometry insures reliable copper removal at all isolation widths. Both coated and uncoated bits are available from stock. Compatible with LPKF, T-Tech,MITS, and AccurateCNC desktop PCB prototyping machines.
Which engraving tool should you be using? Good question, so I will address some common scenarios and misconceptions that will hopefully help answer this question.
First, one of the most common misconceptions: You do not get a sharper or better cutting tool with a sharper angle. Each of our engraving tools has true cutting flutes, which are what determine the quality of the cut.
We have family of engraving tools that are designed for PCB work, each with a different angle and different flute geometries. This tutorial will largely deal with our V-Tip Micro-engraving tools. Choosing between them is a compromise as you have 2 competing forces at work: the strength of the tool, and the cutting width of the tool at a given depth. The sharper the angle, the narrower the cut at the same depth (for more info on this see "Cutting Width" above). However, at the same time, your tool becomes weaker and its sweet spot slower. Let’s take a couple examples to help illustrate where each type is useful.
First let's say you have a machine that is made for making PCBs. It has a vacuum table, and a pressure foot to control your plunge depth. With this kind of setup, your plunge depth is very well controlled and you can be sure you are plunging the tool a constant depth throughout your cut. Unless special requirements are necessary, a 90° or 60° tool is recommended for life, feedrates, and cut quality.
Now let's say you have a hobby level machine. You probably have some variance in your gantry height, no vacuum table, and no pressure foot. In this scenario, you will not have perfect control of your plunge depth and will need to compensate (see “Common Issues” above for some tips). One of the things you can do is choose a tool with a sharper angle. The sharper the angle of the tool, the more slowly cut width increases in relation to tool depth. So in this scenario, we would go with a 45° or 60° cutter. This will allow you to plunge a little deeper without picking up a lot of extra cutting width. The trade-off, however, is a slower feedrate and a more fragile tool.
You may have noticed I listed the 60° cutter in both examples. In most cases the 60° tool is a good middle ground, allowing for work with both types of machines (or those somewhere between). It doesn’t mean that the other tools do not have a place, but if I were forced to pick just one tool to recommend, the 60° would be it. So if you still don't know which tool to get, your safest bet is to go with a 60° tool.
One of the most common questions we get for these tools is “If I plunge the tool to 'X' depth, how wide will my cut be?” or “How far do I need to plunge the tool to get a cut width of 'X'?”. Here I will attempt to answer these questions.
First we will need some data, so here’s a breakdown of the plunge depth to cutting width.
Tool Angle |
Width increased for every .001" plunged |
Increased in depth required for a increase of .001" in cutting width. |
90° |
0.00200" |
0.00050" |
60° |
0.00115" |
0.00087" |
45° |
0.00083" |
0.00120" |
So let's use this in an example. Let's say we plunge a cutter 0.005" into our copper clad. Using the above table, we can determine what the increase in our cutting width will be. Taking the width increase for each 0.001" plunged and multiplying it by 5 (for the 0.005" we are plunging) will give us our increase in cut width.
90°: 0.00200"*5=0.01000"
60°: 0.00115"*5=0.00575"
45°: 0.00083"*5=0.00415"
Now we know what our INCREASE in width will be. To determine our TOTAL cutting width we have to add the tip size of 0.005".
Now let's say we want a TOTAL cutting width of 0.015". We can use the same table above to give us our necessary plunging depth. Since we know that the tip of the tool is 0.005", we know we need to increase the cutting width by 0.010". So we take the "increase in depth required" number above and multiply it by 10.
90°: 0.00050"*10=0.0050"
60°: 0.00087"*10=0.0087"
45°: 0.00120"*10=0.0120"
It is always recommended that you run your own sweet spot test. It will help you ensure that you are running correctly for YOUR material, machine, and setup. Here we will show you some of our test pieces to help you pick a sweet spot on your own. Copper clad is a very easy material to pick a sweet spot in as it will quite easily create a burr of copper when you exceed the tool's ability to cut (see below).
(Click here for high res image)
Here we see one of our tests with a 60° cutter. You can easily see the burr at the start of the cut caused by a lack of tool engagement. As we move up, you can see the clean smooth cut of the sweet spot. Moving up again, we see where the tool's ability is exceeded and we form an obvious copper burr. Where in the sweet spot should you pick? That is a much harder question to answer. It will largely depend on your own preferences. You could choose the highest feedrate within the sweet spot. This would give you better cut times but as the tools dull, you will no longer have a clean cut. You could pick the slowest feedrate and get the longest tool life out of the tools, but you would sacrifice cut time. You could pick a feedrate in the middle and (obviously) be in the middle of these two extremes. Another possibility is to run the tools at the higher feed initially, and as they dull, retire them to slower feedrates or to other tasks.
Engraving Tool Feeds and Speeds in 1oz Copper Clad
| Angle | Depth / Pass | Speed (RPM) |
Feed (IPM) | Infeed / Plunge (IPM) |
| 45° | 0.005" (0.125mm) | 24,000* | 20 | 5-10 |
| 45° | 0.010" (0.250mm) | 24,000* | 30-50 | 5-10 |
| 60° | 0.005" (0.125mm) | 24,000* | 20-30 | 5-10 |
| 60° | 0.010" (0.250mm) | 24,000* | 30-70 | 5-10 |
| 90° | 0.005" (0.125mm) | 24,000* | 20-45 | 5-10 |
| 90° | 0.010" (0.250mm) | 24,000* | 30-85 | 5-10 |
*Please note that our max spindle RPM is 24k. These tools are quite capable of running at much higher RPMs.
Surface Height (If you have a machine with a pressure foot and a true, flat vacuum table skip this section)
Plunge depth is critical to proper use of the engraving tools. You are going to be cutting THOUSANDTHS of an inch into your copper clad. This is not to be taken lightly. If your board is a few thousandths of an inch different in height from one side to the other you will either wind up cutting on one end and not on the other, or cutting one depth (and width) at one end and much deeper/shallower (and wider/narrower) on the other. Neither of these is desirable and it can be very frustrating and may result in a ruined or inconsistant product.
There are a few things you can do to prevent this problem.
- You can true and/or level your table and spindle. This can be quite challenging and may change as your machine moves and ages. We will not cover this here as the process differs for every set of machine and equipment.
- You can adjust your PCB design to allow you to make a deeper cut, basically adjusting for the fact that you will be getting varying depths and widths of cut across the PCB. Using a sharper angled tool will reduce the variation in cut width as a result of the inconsistant depth. This, however, is obviously not an ideal solution.
- You can machine a sacrificial material to mount your board to. This is quite easy and is explained in this section. After completing the below you will have a surface that may not be level, but will be true to your spindle head, eliminating one variable of the plunge equation.
- Find a piece of sacrificial material that is larger then your board.
- Mount it to your machine in a secure way that allows you to still machine the area that the board will be touching.
- Take a large cutter and machine the area the copper clad will be mounted on. Be sure that you go deep enough that at least a small amount of material is removed from the ENTIRE surface of the area where you will mount the copper clad.
Runout
Runout, for lack of an easier explanation, is the wobble of your tool. For a more complete explanation see “Total Indicated Runout (TIR)”, and to determine your runout, see “Measuring spindle runout”). The problem is that these tools can be very sensitive to runout. If you have excessive runout, you will end up with a cut that smears the copper and leaves a nasty burr. If the runout is high enough, it will even break your cutter. For these reasons, it is highly recommended that youknow what your runout is, both for these tools, and in general.
Broken Tools
This may seem obvious, but a broken tool is not going to cut well. These tools have a 0.005” tip, and as such, it is possible to break them without realising it. This is usually a result of an impact on the tips of the tools, commonly either by being dropped during tool changes or by plunging too fast. Unfortunately, without a microscope there is no easy way to tell if you have a broken tip except by the cut quality. To minimize breakage, insure that you are plunging at a proper feedrate and be very careful with tools when inserting them into and removing them from the spindle.