I have spent quite a bit of time pondering how to lay out my post on benchwork details and have had several false starts. On one hand, it seems like it should be pretty straightforward….basic shapes with some holes, maybe some pockets, cutaways and bosses…..not a lot to talk about. But on the other hand, the custom details are where we as machine builders add our value. Yes, we use a lot of catalog items like cylinders, slides, bearings, bushings, conveyors, nutrunners, feeder bowls, indexers, etc when designing a piece of automation, but the details that you design specifically for the application are what tie those purchased items together and make them do useful work.

In that light, a short post with a few tips and pointers didn’t seem like it would do justice to something that fundamental to our business, so I have decided to approach this with a series of posts that go through a host of topics about detail work: manufacturing techniques and costs, design practices, interaction between details, and dimensioning (detailing) fundamentals. Because all of those things work in concert to affect both functionality and cost, I don’t think it’s practical or as valuable to discuss the topics independently. Instead, I created an absolutely do-nothing assembly (pictured) that we will dissect and play some “what if” games with to learn how to make the best decisions possible as you are designing. The series won’t be all encompassing……there are no round stock details that require a lathe, no weldments, no interaction with purchased components, and none of the details are even a tiny bit useful, but hopefully, it will cover enough of the basics that future posts on more specific applications can be more focused.

In this series of posts, I will try to subtitle each chapter in a way that helps you track down pertinent information, but reading them in order at least once may be the most beneficial before going back to cherry pick individual tips. Before we go any further, a definition of benchwork: for the purpose of our discussions, these will be the details with maximum envelopes of around 36”L x 12”W x 16”H (with most being considerably smaller) that have historically been made by a skilled toolmaker on a “Bridgeport” style vertical mill, although many details that fall into this category are now made on CNC equipment or even sometimes printed. For the remainder of Chapter 1, I am going to focus on taking you back to your Manufacturing Processes class with a refresher on the equipment used to produce these bench details. Starting out as a designer, it may seem overwhelming enough just to come up with a design that performs the intended function, but your true street cred will come when you also take into account the pain, suffering, and cost of making the detail. The first step in reaching that point is knowing the capabilities of a typical toolroom and the real world impact of certain decisions you make.

Before we get into the specific equipment, just a few general thoughts on what drives costs in a detail:

Setups: This is purely a non-value added, but totally necessary step. To produce any part, you must have it fixured solidly enough to resist the somewhat significant forces generated in material removal and located “square” to the axes of the equipment you are using to at least 2x the most precise requirement listed on the print and then you have to find either an edge of the part or the axis of a hole on another surface also to at least the level of precision called out. So the more precise the detail and the more times you have to turn it to a new surface, the more money gets spent. At a minimum, you can figure 5-10 minutes for even the most basic setup with a vice that’s already been “trammed in” to the mill. More “custom” setups and higher precision requirements can take 20-30. It starts adding up to real time/money in a hurry and should always be on your mind in design.

Material Removal/Milling and Grinding: This is the most expensive value add operation on a detail. Tremendous forces are generated when milling and grinding and those forces have to be supported by adequate fixturing or mitigated by reducing the amount removed in each “pass” of the tool. The rigidity of your detail design and the geometry of the feature you want to create can significantly affect the time it takes to remove the material. I am not a machinist, so this is just a gut feel based on observations and some time spent milling, but I think a decent rule of thumb is to say you can remove roughly one cubic inch of material on a common tool steel in about 6-10 minutes. If it’s just low tolerance clearance, that ratio should be pretty linear, but if you are down at the .002” [.05mm] tolerance range or below, the final “cleanup” passes will add on to that time and sometimes, can even require secondary operations like grinding. And the material has significant effect on any of these times. Plastics mill very quickly, but the heat generated can cause warpage, so that slows things down. You can go maybe 2-3 times faster with aluminum than steel. Low carbon steel is easier than tool steel, even within tool steel, there is a range of toughness, and when you move to stainless steel, it can take more than twice as long to mill than tool steel.

Holes: Holes are the least expensive value add thing you can put in a detail…..kinda….even the most basic hole requires the following: finding two edges or another hole (possibly on a different surface) as a starting point at least once per surface. Then, each hole gets center drilled to make sure the drill bit doesn’t “walk” as it bites into the material. This sounds like I’m being ridiculous as i describe this, but think about the steps. Move the XY axes to position the hole location under the quill. Find the center drill on your bench, chuck it, turn the mill on, lower the quill, make the start of the hole. Then stop the mill, unchuck the center drill, find the right bit, chuck it and drill the hole. Then, unchuck the bit, chuck a countersink, and countersink the hole slightly to break the sharp edge. Simplest, lowest tolerance hole you can make, and we’re already at 3-5 minutes and three ops. Now, is it a precise hole that requires reaming? Does it have a counterbore or countersink? A tap? Repeat the unchuck, search for next tool, rechuck, do the next op. And if it’s a super precise hole, it may even require finishing on a secondary machine, so more setup, more tool changes, etc, etc. The range between easiest to most complex (with secondary op on another machine) is three minutes to over twenty minutes per hole! Even that doesn’t sound too onerous, but think about the number of holes in a machine and it’s a significant expense, so it bears some thought on quantity, precision, and aesthetic choices. And that doesn’t even include “big” holes that you can’t just drill. Those are major time sucks that can cost an hour per hole pretty quickly.

High Precision and Surface Finish Considerations: At some point, the number of zeroes between the decimal point and the significant digit on your tolerance drives you into a secondary operation like grinding. A surface finish callout can also push you into grinding , lapping, honing, or polishing. Anything at or below a 16µ-in [0.4µm] surface finish callout needs ground. You can only really get better than 32µ-in [0.8µm] on a mill when using fly cutters at high speeds or on most CNC machines due to their high spindle speeds, so for a lot of geometries that can’t be fly cut or made on CNC, grinding starts at any callout below 32. At 8µ-in [0.2µm], you are polishing and honing which are very time consuming. Surface finishes are worth knowing a little bit about and this link goes way more in depth. And just grinding on its own is incredibly tedious and more than a little dangerous….if you get too aggressive “kissing off” to find the surface, you can make the wheel fly apart or ruin your detail. Once you do have your starting point, you are removing .002” [.05mm] max and more likely .0005” [.01mm]-.001” [.03mm] of material per pass not to mention all of the stopping to measure to make sure you’re in the tolerance band required. Imagine how quickly the time accumulates to make real dimensional changes to the detail!

With all that as background, now on to the common equipment refresher for bench details that I will reference in later chapters of this series………

The Venerable Vertical Mill or “Bridgeport”

I will go on and on about this piece of equipment for a few reasons. One, it is about the coolest, most versatile metalworking device you will encounter, and I believe still stands as the only machine that can completely reproduce itself (not counting the motor and assuming you have all the gadgets ever made for it). Two, despite the widespread use of CNC equipment today, the manual vertical mill still makes up a large portion of toolmaking capacity in our industry. And finally, just about all of the machining principles, tooling, and methods that are easy to grasp on a manual mill are applicable to much more complex machining centers, so it makes sense to understand it. If you have anyone in your shop that is willing to take the time to teach you to run a mill and make some parts, including setting up the fixtures, etc, I highly recommend doing so. It will give you a much richer perspective while designing. So, here goes…..

A quick anatomy lesson: starting at the top, we have the motor, usually a three phase motor with plenty of power. That feeds a combination gearbox and sheave based belt/pulley system that can be controlled manually for both direction and speed. The pulley drives a quill, which is a high speed shaft/bearing setup. The quill is hollow and has a drawbar that goes through it which you can thread onto collets and then draw the collet up to tighten around various tools. The quill also actuates up and down with a lever much like a simple drill press and can be locked in place for precision operations or milling. The entire head can move out and lock in place in different locations and also rotate and tilt for maximum flexibility. On the bottom half, you have the bed/table where the workpiece is held, which also serves as the X axis. Most X axes nowadays have power feed capability. “Normal” range of motion is about +/- 18” from center. The X axis is mounted to a Y axis that seldom has a power feed due to its reduced +/-6” range of motion. All of that is mounted to a very heavy knee that moves up and down via a large crank. Range of motion is roughly 16”. The only thing I haven’t talked about yet from the diagram to the right is the digital readout. It’s virtually impossible to find a manual mill that doesn’t have glass scales and a readout anymore, and because of that, it has the precision to do just about all hole placement that you will ever need in our industry. Many moons ago, any time you wanted to do dowels or something with super precise spreads, you had to take the parts off the mill and finish them on something called a jig bore. Now that’s basically a museum piece. These mills also come with servo XY tables and control packages that replace the simple readout shown and allow for 2D contour milling and more automated parts making. The precision that can be achieved with a manual vertical mill has a lot to do with the skill of the toolmaker and the time he or she is willing to spend, but realistically, you can hold hole spread tolerances to +/-.0005” [.01mm] and hole depth and surface thickness/parallelism to around +/-.001 [.03mm] on a reasonably well maintained machine with a decently skilled toolmaker.

Now, to make the mill useful, we need to fixture our soon-to-be parts. They make a ton of standard components for this, so I thought I’d share some of the most common. Easily, the one that gets the most use is a good mill vice as shown in the upper left hand corner of the fixturing illustration below. Most have bases that can be rotated and with a good set of parallels to put inside the jaws, you can solidly fixture 80-90% of what needs to be made. For the remaining 10-20%, the other devices shown can be used to support, clamp, and position the detail to be made in just about any orientation, but everything other than the vice does require more setup, time and skill. Finally, we need the actual tooling to produce the parts. As stated above, the tooling is held into the quill by a collet. They come in a range of sizes in a set and are used directly for milling, boring, and fly cutting (a practice that a lot of old time toolmakers think is too hard on the mill). Examples of the collets and the tools used in them can be seen on the left half of the tooling illustration below. What’s left is basically poking holes and making them useful. For that, most of the time, a chuck is inserted into a collet which is put into the mill. The chuck is used in conjunction with drill bits, taps, counterbores, countersinks and reamers to produce the desired result. Examples of all those are on the right half of the tooling illustration.

CNC Machining Centers

I won’t go too deeply into the nuts and bolts of CNC mills because I believe they are probably covered pretty well in most two and four year engineering degree programs since they are used commonly in production plants the world over (plus I will quickly expose my ignorance if I ramble too long). In our industry, their use is a fairly recent (say a decade) addition to the tool kit. Because of high initial purchase prices, cumbersome and time consuming programming, and scarcity of people to program and run them back then, you wouldn’t even consider owning a CNC as a special machine builder and even farming details out to dedicated CNC houses didn’t make sense if the quantity was less than five. But now, the mill prices have come down, the CAD to CAM interface has been improved greatly, and more people coming out of trade schools have been well trained to the point that a CNC can be a very viable choice to make even a single part. And for quantity details, it is incredibly beneficial. High spindle speeds, rapid traverse, 3D path milling, micron level accuracy and a broad range of tool choices make these things the Swiss Army Knives of the toolroom. Automation companies that still have toolrooms will typically have 3 axis machining centers, sometimes vertical spindle, sometimes horizontal, and sometimes with a fourth axis turntable that can greatly reduce setup time and add even more contour milling capabilities. There are two common tool presentation systems….a chain for larger mills and a carousel for small and midsize. They utilize a standard precision tool holder and store anywhere between 10 and maybe 75 of the tools at a time to enable lights out manufacturing of details. They can achieve phenomenal surface finishes and create very complex details. If I have any concern at all it’s that they are such good machines that I think designers worry less about good design for manufacturing practices now that CNCs are so prevalent….if you don’t focus on good practices with a manual mill, it can take a one hour detail and turn it into a two hour detail. If you don’t worry about them on a CNC, it takes a 30 minute detail and turns it into a 40 minute detail, so that drives more of an “it’s not that big of a deal” thinking. The perfectionist in me (or maybe it’s just the old man in me) just feels that we lose an element of professional growth and opportunity to build better relationships with the other departments when we lose track of those little techniques that used to be the difference between a toolmaker having a good day and a bad day just because the manufacturing technology is better now. The pragmatist in me says that hey, it’s still taking 10 minutes longer and enough ten minutes adds up, so we should still worry about the tiny things.

Manual Surface Grinder

Another common machine in most toolrooms is a manual surface grinder. They have a magnetic “chuck” or bed that is used to hold the details directly or to hold other fixturing devices that then hold the details (for non-ferrous materials or setups/details that don’t have enough surface area on the magnet to be safe), and usually have capacities of around 16-18” in X travel, 6-7” in Y travel, and workpiece max height of around 12.” Grinding is done to either hold closer tolerances than you can directly on a mill or to achieve a surface finish that is smoother than a mill finish. Tolerances that can be held with a grinder are down in the .0002” [.005mm] range if it is in good condition and the person running it really takes the time to “sneak up” on the final dimension. It may vary slightly from toolroom to toolroom, but I would say on average, any tolerance you put on a print that is +/-.001” [.03mm] or tighter will get ground, especially if it is a heat treated detail, so be judicious in adding in those close tolerances because grinding could easily add 30-60 minutes to your detail cost. An example of this grinder and a few of the common accessories used with them are pictured to the right.

Jig Grinder

The jig grinder is another piece of toolroom equipment worth mentioning. The one pictured here is a manual jig grinder, but there are also CNC versions. It can be used to create incredibly precise holes and pockets, both diametrically and positionally. It has an XY bed similar to a mill, but with a screw pitch that is much finer and everything is scraped to ultra precision. If the grinder is in good shape and is well maintained, you can actually hold tolerances in the .00005” [.0001mm] range (and no, I didn’t accidentally put one extra zero in there….it really is 50 millionths), but practical tolerances in our business are +/- .0005” [.01mm] for hole spreads and usually no closer than a .0002” [.005mm] tolerance on hole size. The grinder has a high speed pneumatic grinding spindle that “plugs into” a second, lower speed spindle which is capable of oscillating vertically and also has a lower section that can be offset from spindle centerline to give it the capability of grinding holes even smaller than 1/16” and as large as 10” in diameter. You can also disengage the slow speed spindle and rotate it in a partial arc with a hand crank or lock in in place to do more complex pockets and shapes. As I’m typing, I am realizing it’s not a very easy piece of equipment to describe in words, so here is a short Youtube link and a slightly longer Youtube link that show one in operation. As I said above, on non-heat treated parts, even a traditional vertical mill holds close enough tolerances for 95% of what we do and a CNC mill is more than capable of producing all parts. The debate over jig grinding is mostly for heat treated parts. Heat treat causes some change in diameter on holes and some change in spread. Places I’ve worked have always jig ground all of their dowel holes, but I just had a discussion recently with someone who has never worked in a place that grinds them and said he’s never had a problem. It obviously costs money to do a slow, tedious second op like this, so not having to do it is a plus. Luckily, it’s not something you have to call out on your drawings….it’s either standard practice for your company or it’s not….but there are a few hole design practices we’ll talk about in future chapters that make jig grinding easier, so understanding the machine and when it will be utilized when making the details you design is still beneficial.

Hydraulic/Automatic Surface Grinder

The hydraulic surface grinder is a bigger cousin to the manual surface grinder above, and a maybe not found in as many toolrooms, but can still be very valuable. They usually have capacities of more like 30-40” in length and 10-16” in width and use a much wider 2-3” wheel. What’s nice about these grinders is they can be set up to automatically index across the entire table and then have the head index down by a given amount after each sweep and stop when a final height is reached, so they are excellent for grinding multiples of the same detail to a precise height without having to stand there and manually do it all. They usually have built in coolant systems, so that in combination with the big wheel allows them to take off more like .002” [.05mm]-.004” [.10mm] per pass. An example of a fairly large and elaborate one is shown to the left, but there is a pretty big range of sizes and capabilities for these.

Other Equipment

There are certainly more pieces of equipment in a typical toolroom than described here. As I said above, I am not including any of the machines that are for round details like lathes and ID/OD grinders, or any highly specialized machines like wire and conventional EDM’s, hones, and broaches that maybe could have a place in your benchwork details, nor am i covering the big equipment like boring mills and horizontal mills. We’ll save all of those for other posts when talking about designs that require them.

"Benchwork" Details Series: Chapter 1 - Definitions and Manufacturing Processes