Blog Archives

Index

Current

The CNC Cookbook Blog

2/8/10

Neat Bandsaw Tricks

Cleaned out some of my notes and consolidated them onto my mini-bandsaw page. There's some good tricks in there to get more from your mini-bandsaw. Every time I think mine is done because I got some better saw, I wind up making a little mod to it and bringing it back into service. The last rumor of its demise was due to my DeWalt Multicutter carbide chop saw. I will admit, it took me a couple years to bring it back, but I finally did. I mounted it on a nice cart so it was more stable and at a better work height, and I added a little table to it. I used it mostly in vertical mode at that stage. Handy to pop it on to cut little pieces quickly. A lot less drama than the chop saw too.

The latest rumor of its demise is due to the hulking big 20" (thought it was an 18", but got to doing some research and checking the nameplates and it is a model 28-365 Delta/rockwell 20" Bandsaw, woohoo!) bandsaw I got. It is not yet operational. Spent some time tinkering this weekend to get it going. Motor just hums, so I'll have to suss that out. My brother will likely be invaluable as he helped me get my big compressor with a similar issue going.

We'll see whether I can come up with a good use for the little guy, but meanwhile, the updated page should help others with a saw like this.

At the moment, the other tool I almost never use and need to upgrade to make it more useful or get rid of is my drill press. Of course I have a drill press page full of potential upgades too!

2/6/10

Try a Corncob Rougher to Stop Chatter

Corncob roughers are great. They're those endmills that have the serrated edges. They cut through most materials much more freely than conventional endmills, but my friend Pete says they are da bomb when dealing with chatter, and particularly if you're fighting a small machine's rigidity limitations.

I'll have to try one out the next time I'm having a problem.

Making Cool Fasteners

I like cool and offbeat fasteners. Call it a fetish, but I got hooked on weird fasteners working on cars. They can be very decorative and aesthetically pleasing. Take this shopmade example for a folding knife that I saw recently on the awesome HSM Shopmade Tooling thread:

The "bolt" looks great on the knife, doesn't it? The tool would be a real nuisance to make manually, but very straightforward with CNC. I'll have to try something like this at some point. It needs to wait for my CNC lathe to be finished though.

2/4/10

Armadillo Way Covers

Or at least that's what someone called this style and I liked it:

Cutting Steel on a Sieg X2

I recently had a G-Wizard user contact me about cutting steel on his Sieg X2. He was not happy with the results he was getting and couldn't go near as fast as G-Wizard was telling him to. I wanted to pen some thoughts for this fellow and others who are in the same boat. Sorry for the long post, but it touches on some of the seminal issues that have to be understood right from the start of your machining learning curve.

First, the difference between working steel and aluminum is almost like night and day. Hoss remarked recently on CNCZone that he bought an RF-45 mill so he could work steel and that he had only really been happy working Aluminum on his Sieg X2. I can tell you that even with the RF-45, steel is more challenging to get good results with.

This fellow was trying to square some ¼" angle iron to make some vise clamps. As he put it:

The angle iron was very wavy and needed some squaring. But when cutting, the mill sounded like I was shaking it to pieces if I tried side milling at .030 DOC and around 800 RPM using a 1/2" HSS endmill. The faster I fed the more it shook.

What's up with that?

I remember manual milling steel on my RF-45, a much stouter mill, before I CNC'd it and got G-Wizard. At the time, it would've been rare for me to take more than about 40 thousandths depth of cut turning the handwheels in steel. It just seemed too gnarly and I was in no great hurry. Trying to cut 30 thou on a much lighter mill might be the issue right there. I've since gotten a lot bolder with the CNC, but let's look this situation over carefully.

First up, there are actually three issues to be concerned with. One is what the recommended feeds and speeds might be and how to go about administering those manually. Two is what the machine can actually handle. Three is the possibility of chatter. Let's consider each one in turn.

What are the Recommended Feeds and Speeds?

For a side milling cut of ¼" angle iron at 0.030 depth of cut with a ½" 4 flute HSS Endmill, G-Wizard gives back 1015 rpm @ 37.278 IPM. For a gearbox machine, you'll have to take the nearest spindle rpm and override G-Wizard with that value. In this case, he says 800 rpm, which drops the feed to 29.394 IPM. Keep in mind that recommendations are just the starting point. It's up to the skills of the machinist to take it forward from there.

Next problem is how to manually feed at such a rate? I always converted to handscrew turns/second or seconds/handscrew turn (if it was a slow feed) and then just counted them off-it'll be close enough. In this case, the handscrews are likely 100 thousandths per turn, 10 turns an inch, so we need 290 turns a minute. That's about 5 turns a second, pretty quick!. Faster than a manual machinist will likely be comfortable feeding.

But in this case, the mill is shaking like crazy with a feed that is probably much slower. Let's say 1/5 of that (1 turn a second). So he was going maybe 5 or 6 IPM at best and no way would the mill go faster without shaking apart. Time to consider:

What Can the Mill Actually Handle?

This brings us to issue number two: can this mill actually handle the recommended feeds and speeds? Note that this is a fairly complex question. A less than completely rigid setup, a small mill, and a cheap cutter can combine to make it really hard to hit recommended feeds and speeds.

Let's analyze the symptoms of two problem areas:

- Cutter is getting burned and dulled very rapidly. Lots of heat in the cut. The cutter may be discolored. This is a sign of too much SFM. Need to cut back spindle rpms. Many hobby mills have such low maximum spindle rpm we don't see this one too much. Look at the chip color on steel. Blue will kill HSS cutters. Straw is about right, and silver will give you longest life. Carbide is capable of amazingly faster spindle rpms.

- You are breaking endmills. This can be the sign of too much chipload. Need to feed more slowly. OTOH, this can also be a sign of inadequate chip clearance too. If chips are packing into the cut the endmill's job is tremendously more difficult. Make sure they're being rapidly cleared.

This individual reports the cutter is raising a burr and acting dull as well as there being a ton of vibration. The cutter may have started out pretty dull or low quality, so that is something to keep in mind. The vibration may be chatter, which is a harmonic vibration affected by speeds and feeds, but not a feeds and speeds problem per se. I lean to the theory that this is chatter, BTW. Chatter is a bad combination of rigidity and resonances in the machine.

Let's put the chatter theory aside for later and look at whether the mill can handle the cut.

In this case, G-Wizard assumes a chipload of 0.0022. We may want to take that down some if dealing with cutters that are well used and/or not name brand. A low end value might be as low as say 6 or 7 tenths of chipload. FWIW, that's actually 6.5 IPM on the handle. Too little chipload, BTW, can lead to as much trouble as too much, so don't arbitrarily assume you want to always crank it down. If you want to always reduce it, you can always enter a chipload adjustment in G-Wizard's machine profile. For a Sieg X2, I would be tempted to enter at least some reduction in chipload from the recommended values.

In terms of how difficult that cut is, I like to use HP as a measure. G-Wizard tells us this cut is 0.15 HP if you follow recommended feeds and speeds. So 0.15HP is being fed into the workpiece, your setup, and the mill, and it must resist that force successfully to do the job. FWIW, the same feedrate in 6061 aluminum requires about 1/3 as much HP. That's a decent rule of thumb-the same cuts in steel are 3x more demanding than aluminum. Put another way, whatever your mill could do in aluminum, you can do 1/3 that much in steel, and we're talking the mildest steel, not tool steel or stainless!

Let's turn it around. Is the desired cut, 1/4" deep, 0.030" wide, the sort of cut one would make in aluminum on this machine? I suspect it is. But if steel is 3x more difficult, would the machine be happy cutting say 0.090" wide? Probably a lot less happy.

On my IH mill, I set a 1 HP limit on G-Wizard that I've learned from experience is a good number. That's half the rated 2 HP of the motor because I know if I start to get north of 1 HP I am working my mill pretty hard. I can do it, but I need to take extra care with every aspect of the setup. That's not to say the mill is incapable of doing more, just that I, as the machinist, will have to work harder to ensure success above that level.

I don't know the limits of the Sieg, but I wouldn't be surprised if 0.15HP are very close to equivalent to 1HP on my mill. So, we have both a chatter-prone situation as I will discuss shortly, and we are at the edge of prudence.

What about Chatter?

Okay, let's now go back and focus on chatter. Since it is a resonant effect, you can change feeds and speeds to get away from it or you can increase the rigidity of your machine, tooling, or setup to help resist the vibration.

I said before I suspect chatter, but why? First, one of the big symptoms is lots of vibration and often a sharp sound (hence the name "chatter"). Second, The X2's have a notoriously weak column, which will be prone to chatter. Think attaching your spindle to a tuning fork. Making one of the column mods to stiffen it would really help a lot. Also, the writer mentions that the part was in the vise and "sticking out like a diving board." That's a sure recipe for chatter and low rigidity. Thin plates love to vibrate like tuning forks, which makes me lean even harder to the theory this problem is chatter.

What to do about the chatter? If you want to vary feed or speed, try faster first according to a lot of the sources I have read (Kennametal, for example). In fact, you can systematically map the resonance character of your machine with each cutter, but that's a topic for another post.

Changing feeds and speeds is quick and easy, but it won't always work. The next step would be to find ways to hold the angle iron much more securely and with as little sticking out as possible. I recently built a very stout set of vise jaws (my Vise Jaws of "Doom") to get away from some chatter problems in surface finish. This was while trying to engrave ¼" 6061 aluminimum in a 6" vise. I had maybe 2" sticking out on either side of the vise and no chatter was audible, but you sure could see it in the cut with even the lightest face milling passes.

Here are some ideas for how to systematically deal with chatter:

1) Vary speed and/or feed to get outside the resonance zone. Try increasing feed, then decreasing, then try increasing followed by decreasing speed.

2) Change axial or radial depth of cut. There is a large body of literature on chatter that suggests the resonant frequency of chatter varies with axial and radial depth of cut for a given machine and tool, but regardless of material or workpiece. Changing the axial or radial depth of cut may move you out of the zone of resonance.

3) Make the setup more rigid. Leave as little of the workpiece as possible unsupported. Add more clamps. Etc.

4) Make the tooling more rigid. Use a larger diameter endmill. Reduce the length and "stick out" of the cutter.

5) Make the mill more rigid: Lock every axis but the one that has to move. Tighten the gibs as tight as you can while still being able to move the handwheels smoothly. Make sure the ways are well lubed so you can run your gibs even tighter. I even went to the trouble of doing an epoxy/granite fill on my machine's base and part of the column. I estimate an increase of 15-20% in the rigidity as a result. I have already mentioned making the column to base connection stouter and there are many other's postings on places like CNCZone to help with ideas there.

6) Prep the workpiece. The writer mentions the surface of the angle iron was "wavy". Being a resonant phenomenon, chatter can feed off those waves. In fact, a flat surface that has gotten wavy because of a chattery pass is even more chatter prone afterward. Try to break up the waves if you can. I'd be tempted to hit it with my big disc sander if all else failed.

Last thought: this particular poster asks about G-Wizard's climb milling recommendations. As the G-Wizard docs (and many other sources) will say, if your machine has backlash, you'll need to be very very careful climb milling, and unless you have a lot of experience, you should just avoid it altogether. On a real light machine like a Sieg X2, I just wouldn't try it unless I had ballscrews to reduce backlash to a minimum. On my IH, before I had ballscrews, I used to get away with it by taking very light cuts with relatively small tools. A ¼" endmill taking 15 or 20 thousands was the maximum I would attempt. In addition, I used to really tighten up the gibs and lock and unused axes. The handwheels were very hard to turn, and the machine is relatively heavy, so it was tough for the cutter to drag the table into the backlash.

2/1/10

Finished Making the Vise Jaws of "Doom"

More on these handy tooling items on my vise tooling page. Here's the pic:

24" long, 4130 steel, and spanning two 6" Kurt (well one is a Kurt and one is a Glacern) vises to make one Super-Vise. There's the beef!

(In this shot the jaws are clamped on a couple 1-2-3 blocks just so I could indicate them and make sure they were square)

BTW, the handy way to tram two of these vises is to tram one and then clamp my big Brown & Sharpe parallel in it. Clamp the other one on the parallel while lose and then clamp it down. Done!

(I can always indicate them both in for really critical jobs but this gets it pretty darned close!)

Making Some New Way Covers for My IH CNC Mill

I finished this job a few weekends ago, but I'm just now getting around to documenting it. Here is the finished result:

I used some simple aluminum clamps that work using a bunch of neodymium magnets:

Hoss Uses Slot Pins for Big Jobs

What to do when the job is bigger than your mill's capacity? Hoss uses slot pins as an alignment guide:

Once the pins are trammed in properly, and you can design them so the tramming is automatic based on their fit to your table slots, you can be assured that any work you clamp up against them is properly aligned with the table.

Programming a Higbee Thread

The Higbee is a modification to your existing thread that makes it thread much smoother and without possibility of cross threading. A proper Higbee looks like this:

Not how the rough final thread has been smoothed out...

The goal is to remove the final part of the thread which is usually a small fin on the turned 45 degree angle portion of the part blank up to where it is a full profile 60 degree thread form. To do this you use a grooving tool (or a parting tool) after you are done with the threading cycle.

To start, you must calibrate your threading and grooving tools to the face of the part, which will be your zero. The center or tip of the threading tip has to be calibrated so it is equal to the leading edge of the groove tool and the groove insert must be as wide or wider than the base of the thread form. For example, a 1/8" wide insert will work up to 8 TPI because 0.125 is the pitch of an 8 TPI.

OK, let's go through an example. You're doing 10 TPI threads for a 1" thread length. Your threading cycle will give you a full 1 inch of thread, and the length of the first thread is Z minus 0.100" (since it is a 10 TPI). That first thread is the length to deburr. Program your grooving tool using the same threading cycle to a depth of Z minus 0.100". Make a couple of deburring passes and play wit hthe starting X value. Your spindle rpm and the machines rapid traverse rate with determing the amount of angle of ramp on the deburred thread. The rapid rate will stay constant, so for a squarer ramp run slower rpms. For a tapered ramp, run more rpms.

If your controller has G32, tapered threads, then you're really in fat city. Just cut a 45 degree tapered cut for that first thread and you are done.

Also worth noting: the Higbee was invented for fire couplers. A real Higbee would eliminate the first thread entirely and "Higbee" the second thread.

If you have a CNC lathe, it almost makes sense to Higbee every thread. They'll certainly be a lot cleaner and nicer if you can afford the time and the toolchange.

Cool Plasma Table Work from Algeria

DZStar posted a video of his shopmade plasma table and some of the designs he has made with it on CNCZone:

This machine uses a simple spring-loaded Z-axis (no electronic torch height controller) to maintain the torch distance from the workpiece. The torch is an inexpensive ($700) Italian unit. All in all, it shows just how easy and simple it is to create a plasma table that can do some pretty amazing work. Here are some of his designs:

Doors with intricate mosaic patterns...

My personal favorite!

1/31/10

Parkerizing in a Small Shop

I'm a sucker for metal finishing and treatments because they add that final finish that leaves whatever you've made looking very professional. They can also add durability and rust proofing. Parkerizing is a popular metal treatment for firearms because of its incredible durability and resistance to corrosion. It's actually very straightforward and even relatively inexpensive to Parkerize in the small shop, so I captured some photos of the process on my metal finishing page. Here is a teaser:

I'd love to set up to do some Parkerizing in my shop. I've experimented with Cold Bluing, which is a lot simpler and even cheaper, and was very pleased with my results.

1/23/10

Rigid Tapping Example for G-Wizard from CNCZone

Every time I see some example out on the boards where someone has a question, and especially if there is a good answer, I like to run the parameters through G-Wizard just to see what it recommends and whether it is on track. Recently, there was an example on CNCZone where a machinist was having trouble with rigid tapping. He was trying to tap 1/2"-13 threads in a 27/64" pilot hole to a depth of 1.25". Speed was 530 rpm with a 20.5692 IPM feed rate, and the material was A36 steel. His problem was frequently breaking taps and wanting help with that. In particular, he could only make much progress if he stopped after each hole and applied tapping fluid to the tap.

First, I looked up the 1/2" - 13 thread in G-Wizard:

The tapping drill table tells us that the 27/64" pilot hole is a 78% thread. That's going to be hard on the tap right there, so we might go with a 7/16" pilot hole which is still a 62% thread. The tap will have to remove quite a bit less material. We also note the Pitch of 0.0769", which we'll need for the Speeds and Feeds (eventually I'll add 1 button to go from the Threads page to Feeds and Speeds and it will initialize that information for you!). Now here we are in Feeds and Speeds:

A couple of things are interesting to note. He was using 530 rpm with a 20.5692 IPM feed rate, but G-Wizard suggests a slower speed--290 rpm--and a much different feedrate--22.326 IPM. When I override spindle rpm to match his 530, I get a feedrate of 40.757! Here was a case where the feedrate was way off, which, with a rigid tapping setup in a collet, was inevitably going to have the machine stressing the tap against the threads as the spindle was moving downward fast enough.

Some other good tips from the thread on rigid tapping:

- He was using a 50 taper VMC. The spindles are pretty massive on those, so a tension/compression tap holder was recommended to absorb any vertical tension as the spindle accelerated and decelerated. In fact, several folks opined that a tension/compression holder was just an all around good idea even though rigid tapping shouldn't require it because it saved a lot of wear and tear and provided a margin for error. In this case, the programmed feedrate was too slow (22.326 IPM versus 40.757 IPM). Over a distance of 1.25", that's 16 turns times the error in feedrate times the pitch and we get an error of less than 40 thousandths. If he'd been using a tension compression holder, it would've completely absorbed that error which would've helped a lot, leaving only the too-fast spindle rpm.

- Geof suggests Repeat Rigid Tapping (sort of the tapping equivalent of peck drilling, I suppose) for a hole that deep. He would break it into 4 depths of 0.4, 0.7, 1.0, and 1.25.

- A36 is soft enough to allow Form Tapping, which makes stronger threads and involves no chips.

- The ER15 collet being used is probably too small for a 1/2"-13 tap. Try an ER32 or go to a tapping chuck.

- Program the tapping at the end of the cycle because the operator needs to be at the machine anyway and can apply tapping fluid.

Another thought I had was that rather than hand brushing the tapping fluid, find a defined place to put one of those no-spill-if-you-tip-it-over containers and program the machine to dip the tap each time. Might almost be worth it to epoxy some magnets to the container if that makes it easier, or make some kind of bracket to attach it to your machine's table at a location where the spindle can access it.

Stallion Trunnions for 4th Axis Work

I just got my harmonic drives in the mail from an eBay seller the other day, so a 4th axis has been on my mind. It'll be some little while before I get around to it, but meanwhile, I love looking at tooling and setups for 4th axis work. Recently I came across the Stallion Trunnions by Martin Manufacturing, which let you mount a Kurt double vise on your 4th axis. What a cool idea:

Normally you'd be futzing around with clamps, angle plates, and maybe sine plates, but this Trunnion lets you mount your Kurt vise. Now you've got full access to softjaws or you could even set them up with some vise pallets to make your setups go real fast. They also offer the slightly shorter Mustang Trunnion which will hold 2 8" 3-jaw chucks:

Or you can get the Trunnions with an interchangeable tooling plate system:

1/23/10

A Fair Bit of G-Wizard New Functionality and a Sneak Peak at the G-Wizard G-Code Editor

I've built up a pretty fair inventory of improvements to my G-Wizard Machinist's Calculator so released another update today. The software is free for the time being if you join the Beta Test. Details for how to do that are on the G-Wizard page.

Here is what's new in this version:

• Since the old "Logout" button was confusing some users, it has been changed to say "New Login". You only need to use it if you are changing your login credentials (e.g. switched to a new email).
• Added tapping feedrates for rigid tapping.
• Added "Torque" as a unit conversion type in the Calculator.
• You can undo an individual override by clicking the padlock on the Feeds and Speeds calculator. This way you don't have to reset all of them.
• The feeds and speeds calculator now recommends when it is best to use climb versus conventional milling per the thoughts from AB Tools who make the popular AlumaHog and ShearHog cutters. Note that if your mill has much backlash at all you shouldn't be climb milling in any event.
• Added thread cut depths to the Threads Quick Reference tab. These depths tell lathe users at a glance how deep to cut with either a sharp pointed v-tool or a UN/UNR form tool. Still need to add the equivalent to the metric and pipe threads.

My favorites are the climb vs conventional milling recommendation based on thoughts from AB Tools, and the new thread cut depths on the Threads page, which makes it easier for lathe users to know how deep to cut:

"Use Climb Milling" is a machining hint that is based on the Radial Engagement or Cut Width...

Thread cut depths are on the left where they're easy to see...

In addition to the G-Wizard Calculator changes, I've started a new page to offer a sneak peak at the G-Wizard G-Code Editor. Here is a sample screen shot of the editor:

You can see several of the editor's key features:

The editing pane is on the left. A full tool simulator with Rhino3D-style views (Top, Front, Right, and Perspective that all pan, zoom, or rotate with the mouse) is on the right. Below the tool sim is what I call a G-Code "Hint". This is a learning tool for newcomers and a timesaver for old timers. It tells you in plain English what that line of g-code will do. There is a full page of hints for every line in the program available via the "Hints" tab on the editor pane.

Much more to come!

Note: The editor is not yet available for Beta Test. When it's far enough along that it can add some value without being a nuisance, I will open it up to Beta Testing by anyone who was included in the Beta Test for the calculator. That means the easiest thing to do if you are interested is to just sign up for the calculator Beta Test on the main G-Wizard page.

1/19/10

Congratulations to Tormach on the New PCNC 770

Saw this first on the Yahoo Tormach board:

It's a new mill, which is something that comes along very seldom. The 770 is somewhat smaller than their 1100 flagship mill, and has some intriguing new features:

- 10,000 rpm 1 HP spindle: Should be awesome for aluminum work. Slow spindle speeds is the largest problem with small mills.

- 130 IPM rapids, to go with that faster spindle you'll need faster feeds.

- Breakdown construction to make it easy to move into basements and other hard to reach areas.

- 110V Single Phase: No need for 220.

- Same R8 taper and 5/8" table slots as on the other machine, so accessories are compatible. It'll be interesting to see if that extends to the power drawbar and whether there will be an automatic tool changer.

All in all, it looks like a very well thought out machine. The 770's are supposed to be available today in the $6-7,000 range. I'm betting we'll see a 10K spindle for the 1100 before too long as well, but time will tell. There was talk in the video about the 770 being part of an overall "2nd generation" of Tormach mills.

Congratulations, Tormach!

1/17/10

Collet Rack Eye Candy

Seen on HSM:

I'd love to have a drawer like that on my CNC cart for collets and things less often used than the tool holders themselves. Have to give it some thought...

1/16/10

Started a New 4th Axis Page

Just a few design notes so far since I finally snagged a Harmonic Drive from eBay.

A Vacuum Table from ZealCNC

Vacuum tables are a real fast and easy way to hold down flat plate work. Amazing how much force can be applied: nearly 15 pounds per square inch. A 4" x 8" plate will have almost 500 pounds bearing down on it.

Here's a really nicely made little table from ZealCNC, a new site I just discovered with a lot of great work on it.

You can see the grooving in this photo. In practice, you'd block off grooves that were exposed and not under your workpiece with some rubber gasketing of the right cross-section...

Here you can see the manifolding. He used a venturi vacuum generator but remarks that a vac pump would be better.

Sweet Lil 4th Axis

Also on ZealCNC was this cool little 4th axis:

The silver box is an integral harmonic drive, which gives zero-backlash gear reduction. Looks like he has made the spindle out of an ER collet chuck. Like all the projects on the site, the 4th axis looks absolutely gorgeous. It's anodized or polished in all the right places and has the clean well-thought out lines of a production-quality piece of tooling.

1/14/10

Austin Barnett's Killer Car Badges

I came across Austin's work on CNCZone, by accident. It was one of those "follow the link" treasure hunts, but boy was it worth it. Check out these amazing custom badges he makes for the Corvette community:

Aren't they gorgeous?

He provides some details on how he makes them on his Mach3 converted Bridgeport Boss mill:

I cut them from 6061 aluminum, sanded them up to 800 grit and buffed them out. I chromed them using copy chrome from caswell plating, which I really recommend. Then I filled in the engravings with paint. It a pretty laborious process and it takes a bit of time, but it keeps me from having to punch a time clock.

That Copy Chrome product sure sounds interesting. I'll have to check it out.

Postscript:

I got a nice note from Austin saying he was no longer using Copy Chrome. It's a fine product, apparently, but the badges pictured above are all just polished aluminum. Also, here is his sanding routine:

Sanding:

1. start with a palm sander with 220 grit and do as much as I can.

2. Same palm sander and switch to 400.

3. I use a Dremel contour sander with 220.

4. Continue with the contour sander with 400.

5. Paint the emblems

6. Palm sander the paint with 400 to get rid of the extra clear, that went outside the lines of lettering.

7. Wet sand with soapy water and 800

8. Start the buffing with an automotive style buffer with a wool pad and 3M perfect it rubbing compound.

9. After the paint has been properly smoothed I move back to the contour sander. This time I put a microfiber cloth on it, instead of sand paper, and use some mothers billet polish.

10. Laser cut some double sided tape, using the Rabbit HX40B, and apply it to the emblems.

11. Finally I go back over the emblems with the mothers billet polish by hand using the microfiber cloth.

In addition, Austin mentions that he switched from using automotive touch-up paint to using automotive base plus clear. He says that combination not only adheres better to the aluminum, but it can be polished. Lately he is experimenting with powder coat.

If you are interested in any of Austin's badges for your car, here is his contact information:

Austin Barnett

(218) 828-4544

(218) 839-5928 cell

austinbarnett@charter.net

Here is Austin's mill with some more notes:

A table enclosure to control the flood coolant. Also note the bungee tensioner on the router: low cutting force at these rpm's!

High speed auxilliary spindle for fine engraving...

The badges are machined on this fixture plate that clamps into the vise...

Here is a piece of 6061 Tee'd up. There is double sided carpet tape underneath to hold the plate on the fixture, as well as the two clamps on top...

The backing paper from the carpet tape makes a nice feeler gage to touch off!

1/11/10

Some Neat Little Setups for a Steam Engine Project

HMEM is a board dedicated to buildling model engines, and you see some really cool stuff there. These are some photos taken from a nice beam engine that had some setups involved I liked:

Cutting a stack is a great way to be sure they all come out the same. I like this little tooling plate for the vise, and the twist drills are handy precision pins to hold the stack in alignment. The clamp is purpose-made for this kind of fixutre. And, when did you ever not find a good use for a Kant-Twist?

No setup, but I thought the part was cool. He milled some flats on this spacer to simulate a lock nut...

He's got that part surrounded! This is a tough cut with the saw because it's a tall skinny piece that will want to vibrate like a tuning fork. I think I'd have sandwiched it between 1-2-3 blocks and stood the blocks on something so very little stock protruded...

Now this part is really in there tight. Rigid setups are second nature to good machinists, but beginners always try to get by with less than enough...

This is cool. Hand ground form tool in a flycutter to radius the top of the bearing block. Form tools can save a lot of time...

A little custom aluminum block holds the bearing block in the vise step for boring...

That bore is dead true. Nice job with such thin walls!

Now it's time to mill 2 square pieces to taper at either end. Two different sized center drills act as pins against the top of the vise jaw to create the angle...

Now they are tapered!

Back onto the vise top fixture plate (that's a handy little gizmo, eh?) for some decorative grooving...

Nice series!

1/10/10

Speeds and Feeds for HSS Reamers

Saw this question come up on HMEM. A lot of machinists are taught a rule of thumb:

     1/3 the SFM, 1/3 more feedrate than the same sized HSS Twist Drill

Opinions vary on exactly what that rule of thumb ought to be. Is it 1/3, or is it 1/2?

Here's what G-Wizard would suggest for a 3/16" HSS Reamer in 300 series stainless, which is the question in the post:

30 SFM, Feedrate of 3.67 IPM...

and here is the equivalent HSS Twist Drill:

45 SFM and 2.75 IPM...

That's 1/3 less SFM (spindle rpm) and 1/3 more feed. Pretty close to what manufacturer's like Redline show for their reamers, and pretty close to the old rule of thumb. Hey, sometimes the rules of thumbs are just the thing!

Give G-Wizard a try. It's free during the Beta Test!

Tooling Plate on a Tormach

One of the many many projects on my wish list is a nice tooling or fixture plate for the mill. When done right, they can save a lot of time. They use a grid of alternating dowel pin alignment holes and threaded workholding holes. You put all of your tooling like vises on subplates that mate and you can swap tooling and have it retain alignment to very tight tolerances. I keep an Idea Notebook of information about various things and I have a page on Tooling Plates too.

Nice fixture plate on a Tormach as seen on CNCZone:

1/9/10

Nice Tooling Drawer

Seen on CNCZone:

1/6/10

Mini-Mill Comparison + 5-Axis CNC Tool & Cutter Grinder

I've been pondering a project that would involve a smallish mill: a 5-axis Tool and Cutter Grinder. A lot of the amateur world has a fascination with T&C grinders. There are a number of designs out there for manual machines that can be built from scratch that are aimed at this group, and I've even dabbled with a manual design of my own that I have to date not tried to construct. I can't quite get excited about doing a manual machine though.

Why would I need such a thing? Two reasons. First, I would just enjoy working with another CNC project, and this one seems a little more bite-sized than my IHCNC was. Realistically, I will finish my project to convert my 9x30 lathe to CNC first, but this could be the thing I tackle after that. Second, I get a lot of value out of the Drill Doctor drill sharpener I bought. I can imagine getting a lot of value out of a general purpose T&C grinder too. Not just for twist drills, but for sharpening endmills, putting a radius on them, making special forms, and so forth.

To build such an animal, we need a CNC'd 3-axis mini-mill plus two extra axes that look like this:

2 Rotary Axes viewed with the X-axis running left to right...

I'm still evaluating which of the mini-mills would make sense for the project, so I put together this comparison table:

Specs for various small mills...

Eventually, I'll make a decision. I lean towards the BF20. It has a nicer look to it than the Sieg X3 and seems considerably stouter than a Sieg X2. Hoss over at Hossmachine has said he prefers the BF20 to the X3, and I think he has already ordered one. Even though he just got an RF-45, the BF20 is slated to be the next thing he CNC's, so I'll be watching that build closely to get more of an "inside" perspective on the BF20.

Meanwhile, I did order 2 nice zero backlash 50:1 harmonic drives from eBay to power the rotary axes.

1/4/10

Micro-Miniature Tormach Tooling System

A lot of folks are adding auxilliary high speed spindles to their mills for things engraving and running very small endmills or twist drills. G-Wizard's recommended rpm for a 1/16" HSS twist drill is over 12,000 rpm, for example. Smaller drills, like you would run to drill a PC Board, require even more speed. In fact, there is a whole market out there for companies that sell small very high speed "sensitive" drill presses for this sort of thing. But, they're not CNC.

It's pretty easy to attach such a spindle to your CNC mill's head, and people have done this with everything from Dremel's, to their higher quality Proxxon cousins, to routers, laminate routers, and all sorts of other appliances. Take a look at the page I linked to for some ideas. This is a pretty handy thing, but pretty soon, you're wishing for some of the comforts of home. Perhaps a toolchanger is out of the question, but at the very least, a way to make the cutters repeatable in Z so you don't have to do a touch off for the tool table every time would be nice.

Enter this great idea I saw on CNCZone:

0.020" Endmill with a Distance Ring...

First attempt at a holder with Tool Table numbers. Those cutters are so tiny!

Here is a little fixture to help us press the ring onto the cutter...

Of course when you have a CNC at hand, a nicer holder is only a matter of time...

Tiny train wheels next to a penny...

All this micro-machining work was done on a Tormach with an auxilliary Proxxon spindle. I have to say I am very impressed. The requirements for runout and precision have to go way up at these scales. The distance rings are available from PC Board drilling suppliers such as LPKF.

Very cool!

1/3/10

A Drillpress Table Lift

Jerry over on HSM had this nice table lift for his drill press to show:

Nice use of a surplus reduction-geared motor, and very compact. I think I'd have mounted the switch up on the drill press head, but that's just me. I have a whole page of drill press mods that I will be adding this one to!

1/2/10

The Ultimate Gang Lathe?

My friend Pete put me onto this cool video:

Check the live mill tooling on this gang lathe...

That gang lathe is about the same in capacity as the many Hardinge-based gang lathes out there. The thing I couldn't quit thinking about was that live mill tooling. You could do something similar pretty easily:

Get yourself a Sieg X2 at Harbor Freight with the 20% off coupon so it costs a little under $400. Rip the column off and build a mount for your gangslide. Save the table for your drill press or other project. CNC that Z axis. Now you have a removable milling axis. You can add a belt drive to the Sieg for like $150 and bump the spindle up to 5000 rpm. Or you could mount one of those Chinese 20K rpm spindles I keep seeing for more performance.

If you want the tool changer, that's doable too. Make one like Hossmachine has on his Sieg X2 with Tormach Tooling System as your changer bits.

The mill attachment could be made removable just like the other gang tooling, in case you wanted to recover the space. Think of it as a sort of "Lathe 4-axis attachment", though in this case it is more of a 3rd axis. It's cool the way they're reusing the X and Y motions available to the gang slide.

Why would you need such a thing? Oh golly, lots of things can be made that would benefit. Suppose you need to mill some wrench flats on a fitting, for example.

12/31/09

Gorgeous NEMA23 Stepper Motor Back Covers

Saw this on CNCZone first, very cool! Just the thing to make your project look more professional:

Available here on the Mach3 supprt forums for $10 each (bargain). These are NEMA23. This guy should make similar housings to slap an encoder on the back of a servo too!

Hoss Machine Has a Nice Rack

The piccy says it all:

It pivots out of the way...

12/30/09

G-Wizard G-Code Editor Lives! (Well Sort Of...)

When people ask what I did over the Christmas vacation, the answer will be that I wrote code for my upcoming G-Wizard G-code editor. GWizardE will be the second module in the G-Wizard series, with the Machinist's Calculator being the first. It's still very early days yet for the editor, but I did want to capture some screen shots for posterity. Here is its very first backplot:

This is a backplot of a g-code program I wrote to cut the lefthand support for my R8 Tooling Rack...

You have no idea how hard that first step was, LOL! GWizardE will incorporate a number of novel features. For example, to help new programmers learn g-code more easily, it incorporates the idea of g-code "hints". The hints are basically English translations of the cryptic g-codes. Here is a view of the Hints Tab for this same program:

Hint tab shows an English translation of the g-codes, line by line...

There's a lot more coming, but for now, I just had to capture the moment. We're still a ways away from making GWizardE available to Beta Testers, it's not even alpha quality yet. But, if you want to make sure you get an invitation to test GWizardE, sign up for the G-Wizard Machinist's Calculator Beta Test. There are hundreds using the calculator now and it is working pretty well. I'll be adding some more nifty stuff there too, and best of all, these two will be integrated and able to exchange information. I'm keeping mum about what all that means for the time being, but rest assured, it will be very cool!

Scraping Video

Scraping is the preferred method when surfaces need to be flat to a high degree of precision, such as when making machine tool ways. lt's a painstaking manual process that I've often wondered about. Here is an excellent video of a Kitamura machinist scraping a casting for one of their machine tools:

Lots of good learning here about the angle to hold the scraper and you can see how he aims for the bluing (which in this case is black). It also looks to me like his scraper is set up so he can apply force with his hip.

Shopmade Motor Couplers

Couplers to link your stepper or servo motor to the leadscrew or other drive mechanisms can be surprisingly expensive. It's not hard at all to make them in your shop. Here's some Oldham-style couplers made as part of a Weiss mill conversion described on CNCZone:

The plastic inside parts where bought as replacement parts very cheaply, which meant only the metal ends had to be machined. As you can see, they're very simple!

Another example, done with a slitting saw...

What's nice about making your own couplers is you can accomodate whatever special requirements you may have. I've had to bore store-bought couplers to fit a shaft, for example.

12/26/09

Vise Pallets

The secret sauce for a lot of very clever machine work is in the fixturing, so I always pay attention when people are posting pictures of their fixtures (he's a poet and just don't know it, yeah right!). Here is a nice simple little fixture from Travis on CNCZone:

It's kind of like 4 little vises, and you could stick this fixture into a vise (or 2) as a pallet. Pallets are great because you can be setting up parts on alternate pallets while the machine runs. This particular fixture is made of aluminum, which, as the CNCZone thread commenters say, won't last too long. Steel would be better, but more trouble if you don't need a lot of parts.

12/24/09

The 17 Cent Flood Coolant Enclosure

Next time you're getting ready to machine, forget the age old HSS or Carbide question. Instead ask, "Paper or plastic?"

I couldn't resist!

There's something quite entertaining about this very pragmatic solution!

Swing Threading Toolholder and other Threading Aids for Manual Lathes

Threading on a manual lathe seems to be a scary process the first time around. I didn't attempt it for my first year or two of turning, for example. Eventually, you reach a point of needing to thread something that's too big to make sense for a tap or die, and then you just have to deal with it. I'm not going to try to attempt to explain threading on the lathe here, there are lots of good resources that do that. Personally I like the Southbend Lathe Book, which is readily available.

Rather, I'm going to talk about a couple of aids for threading that I have come across recently. It seems that the issue that really bothers people is the retraction, often complicated by the desire to thread up to a shoulder. There is a certain amount of pressure on the operator to do several things very quickly: stop the feed, retract the cutter, reverse to start the next pass, advance the cutter, restart the feed at exactly the right point on the threading dial. If you make a mistake, you can bollocks up the thread or crash your threading tool into your shoulder. I hate when that happens!

So the first aid I came across is what I will call a "Swing Threading Toolholder." This is a cool idea from HSM and other boards. When it comes time to reverse, stop the lathe, and simply reverse. Leave the half nut locked (some shops feel this gives a more accurate thread anyway). The "swing" is because the tool is free to swing upwards when it contacts the threads moving in reverse, so it doesn't cut on the return pass and you needn't retract.

Here are some Swing Threading Toolholders:

John Stevenson modified a carbide threading tool with a pivot and shelf underneath...

Gary Hart made a swing threader that uses carbide inserts...

It pivots on a 1/4" dowel pin.

That's a fancy looking little design. I wonder if the handle locks the swing or what?

(A kindly reader has informed me this is a George Thomas design that was published in Model Engineer. The lever may be used to withdraw the cutter.)

Bogstandard's very elegant looking version. I saw his first, so I saved it for last...

By all accounts, these Swing Threaders work really well. John Stevenson says it is the fastest thread he had ever cut.

Another manual threading aid is a system of stops on your handwheel. The Monarch 10EE's came with such a system. There are various shopmade ways of providing something similar:

This is John Stevenson's copy of the 10EE system...

The exploded view of the 10EE system. Note the setscrew on the right.

To engage the system, just wind the set screw in. It will engage the first of the three dogs. That gives you one rotation until the first dog engages the second, giving another rotation to engage the third for a last rotation. So you can turn the handwheel 3 rotations against the stops. The depth of cut is set by the top (compound) slide. Set the depth, crank the lower slide all the way to the stop, cut a pass, retract the lower slide to opposite stop, and traverse back for another pass. I kind of like the Swing Tooling better, but who can argue with the genius of Monarch? John has retrofitted this to some other lathe in his shop, a TOS I think?

A similar idea that engages a pin in the dial. This would only allow one turn of retraction.

Here the thread stop is flipped up to disengage it...

12/22/09

Jared's Cube: Baffling and Beautiful

If you like Turner's Cubes, perhaps Jared's Cube will appeal:

I found these quite by accident via Google. Aren't they cool?

12/20/09

Spectacular Tormach Flood Enclosure

This was up on CNCZone, just gorgeous:

Some Vibratory Polishing Tests...

I threw some parts I had in the vibe and left them for 4 days with walnut shells impregnated with green rouge. Here is what I got back:

On the left is a part straight off the mill, covered with all sorts of tooling marks. Unfortunately, the flash makes it hard to see when looked at face on. It's hard to photograph these finishes!

Next up is the part marked "deburred". It ran overnight with some deburring media until it had a nice satin finish. There is definitely some grain still on it. In fact, I had some parts that had the vibratory deburr and some that didn't. The ones without were shiny with deep scratches left from the tooling marks. I didn't bother photographing them as the satin finish from the deburr looked better to my eye. Lastly, we have 3 parts on the right that got a 4 day polish in the vibe. There is still some grain visible, so I can't truthfully call it a "mirror", although I notice a lot of people want to call any shiny part a "mirror". But, they are quite shiny. You can see the bottom photo they are reflecting the grain of the granite countertop they're sitting on. All in all it is a nicer finish than the deburr. I suspect it would be nice to have had some grade of abrasive in between the deburr and the polish. I'm not sure what that would be, but there's still too much grain after deburr for the polish to get it to a mirror.

I find when polishing I often have the problem of moving to the next finer grade too soon, only to have it do a wonderful job highlighting scratches that should have been taken care of with the coarser grades. In any event, I am reasonably happy with this first time polishing result. It looks like something you'd buy commercially and think nothing of it. Best of all, I literally forgot about it while the vibe did its work.

I need to experiment a bit more on my exact processes, but I really like this approach. The polished parts also picked up a wonderful smooth feel.

12/13/09

Amazing Shopmade Plasma Table

This plasma table from CNCZone is probably the most impressive table I have yet come across:

It's a big beast. The gantry is mounted on the long axis so that when it is slid out of the way, access to the table with a full sheet of material is easy.

They had the various parts laser cut by a nearby supplier. Note the copious use of "tab and slot" construction. I see this a lot when parts are to be welded together. Also note that cutting out parts like this would be a perfect job for a plasma table (or laser or waterjet).

The gantry is made of aluminum, and was powder coated. The details of the X-axis motor are showing how they used gas springs to preload against the rack. The whole thing rides on Thompson 1.5" linear rods.

Table is 4' x 10'. The torch is an ESAB 1500.

Hang on, hold the phone, I've got an ESAB 1500. I'm adding this build to my Plasma Table Idea Notebook.

There's my brother playing with it shortly after I got it...

A Gantry Mill From Two Column Mills?

Looking at the following made a crazy unbidden thought spring to mind:

I look at the two columns and I see two conventional column mills (bed mills) mounted on a new base with moving table. It so happens I even own two identical Industrial Hobbies mills!

I wonder how such beasts perform? It'd be very tricky to get it all squared up, I suspect. But the work envelope on such a thing would be awesome and it would be much more rigid if done well than the original.

I think I'd use either some massive cast iron bar stock or possibly 70xx aluminum for such a project. That big base could be done as a weldment (fabricated plate welded together) filled with epoxy granite. A big thick plate connecting the column tops also seems like a good idea.

At some point, I would like to build a machine from "scratch". This might be the right one. Or the right one might be a CNC Tool & Cutter Grinder based on a Sieg X2. I've been wanting to play with one of those little mills too, and they're available very cheaply from Harbor Freight with the 20% off coupon.

Separating Chips from Coolant in a Shopmade Enclosure

If you're going to run flood coolant, an enclosure is a must to keep the mess under control and out of you shop. I keep an Idea Notebook of shopmade enclosures because at some point I'll be tackling this chore for my IH Mill. There are lots of good ideas there. The latest one I ran across is this approach to separating the chips and the coolant seen on CNCZone:

At first I thought it was a chip conveyor...

The idea is to slow down the flow along a shallow incline so the chips can drop out through gravity. Presumably a couple of ridges would help even more with the process. He also uses the normal arrangement of de-humidier foam filters and that sort of thing, but I think the real secret is this trough. Most of these enclosures just mount a kitchen-sink drain in the bottom and pipe it straight down to the coolant reservoir. Letting gravity and slowly moving coolant (because that trough has only a shallow incline and is very wide and deep compared to the amount of coolant seems a clever move.

Ultimately the coolant winds up in this reservoir under the enclosure...

12/12/09

Blast Cabinet Tweaks

Blast cabinets are really handy to have in the shop (if you've got room, they're not compact). The cheap ones actually work really well (I gave $60 for mine on eBay), but they have their drawbacks too. So, as any good machinist would do, we start thinking about how to "improve" the cabinet. Here was a good idea I came across on HSM:

Note the PVC with holes run along the top. This is Steve45's idea to blow some air across the window to keep the dust away so he can see what he's doing. The other thing that seems to help is adding a ShopVac-based dust collector. I understand even the cheap ones from Harbor Freight make a nice difference.

Lately I have also been eyeing some higher quality guns. The gun that comes with a cheap blast cabinet is serviceable, but not very slick. At some point it will wear out and I'll look at nicer guns. A company called TP Tools has some interesting blast cabinet accessories including higher quality guns and a lot else. Their niche is air equipment of all kinds, but they specialize in blast cabinets, painting, and compressors. I found out about them after purchasing an electric compressor drain on eBay for my big Eaton compressor.

12/11/09

The Devilmaster Redux: Gorgeous CNC Router

If you've never seen the Devilmaster's work, you must take a look. It is really outrageous. Here is his fixed gantry CNC router as pictured on CNCZone (which brought me back to Devilmaster's delightful work):

So many tasty touches on this beauty!

Here is his watercooled PC video card, which is one of the things he likes to use his router to make:

My brother loves woodworking, and we keep talking about building a CNC router for him. I'd love to do something like this but on a much larger scale. He'd need 4' x 4' or maybe larger as he likes to do furniture. I keep thinking about building a fairly massive gantry out of epoxy granite too, and did a design sketch and some notes about how to go about it.

Epoxy Granite Table with Inserts...

12/10/09

The Master Jaw System: Turn Your 3-Jaw Chuck Into a 5C Collet Chuck

Yantra3D, from CNCZone, sent me a note today letting me know that if you liked Geoff's Excellent Collet Chuck Alternative (see the article below), you can buy one off the shelf called The Master Jaw System. Apparently it is a "precision length" system. I assume (you know where that leads) that means that if you align the workpiece against a stop and then lock down the collet it doesn't move. One annoying thing about 5C's is that most collet closers pull the collet back into the taper, which of course means the length is all over the place.

Cool!

12/8/09

Make It Easier Changing Pulleys for Machine Speed With a Bicycle Chain

Well sort of. I thought this idea from Weirdscience on HSM was pretty clever:

Bicycle chain hinge on the bottom is pure genius...

Sure beats yanking on that capacitor!

12/3/09

G-Wizard Calls Those Speeds and Feeds Pretty Close!

Every time I see a thread on one of the machinist's forums discussion feeds and speeds I like to crank the scenario through G-Wizard to see what it comes up with. I've learned a lot and refined the program quite a bit in the process. Just today I ran across a thread about real small ballnosed endmills in aluminum on CNCZone. G-Wizard accurately predicted the feeds and speeds the poster was able to achieve through trial and error pretty darned closely.

There were two scenarios. First was full width slotting with the 1/8" endmill. G-Wizard predicted that could be done at 24 to 34 IPM using the 12K rpm spindle this fellow has. His result was 27 to 30 IPM, although he says 30 is unreliable. Pretty close!

The second scenario was after the initial slot is cut, what could be done with the 1/8" endmill at an 0.010 - 0.015" stepover (stepover corresponds to the cut width on G-Wizard). He says he can run at 100 IPM for that cut. What does G-Wizard come up with? At an 0.010" stepover, it would be 122 IPM, but at the 0.015" stepover, I get 99.77 IPM, which is almost exactly his 100 IPM:

Radial Chip Thinning FTW @ 99.77 IPM with G-Wizard!

Why can you run so fast versus the full slotting cut? The answer is radial chip thinning. Read more about it in my CNCCookbook article to understand why.

If you haven't tried G-Wizard, give it a whirl. The Beta Test is free at the moment and will be for quite a while.

Geof's Excellent Collet Chuck Alternative

He just made a set of softjaws for the 3-jaw:

5C Collet in soft jaws on a Haas TL lathe...

Looks to me like if you don't release the jaws too much you could even pull a little bar through that collet. He used a Bison Set-Tru chuck so he could get the collet to run concentric with the spindle. Clever and easy to do. I'll bet the TL was perfect to CNC the 5C profile onto the jaws!

12/1/09

Going to Try Some Vibratory Polishing

I've played with vibratory deburring on several occasions and been very happy with the results, so it's time to get on with trying some polishing for an even nicer finish. I was over at a friend's shop a while back and took a look at some parts he had vibed. Very nice mirror finish. Mind you, he has a much bigger vibe and he let it run 4 days, but the pieces looked very nice. HIs biggest issue was having them bang together and scratch each other if he turned up the action on the vibrator too much.

What spurred me to move forward was seeing a post in PM. It listed a source (Graves Company) for small quantities of green rouge-impregnated walnut shells. A 5lb bag will be perfect for my little vibe. Price wasn't too terrible at a bit of $20, so I'm going to give it a try when it gets here. If you order, you want their Tumble Dry Green media. The thread says this particularly media will get the polishing done in a much shorter than usual time. The walnut shells are meant to be run dry, and they already have all the right active ingredients impregnated. Just put them in your clean vibe unit, add parts, turn it on, and walk away until the shiny sets in! Typical times from the thread are supposed to be 24-48 hours. I'm emotionally prepared for my smallish vibe to take longer.

BTW, another interesting trick from the same thread is to throw the parts in the dishwasher with Palmolive gel soap for some super shiny after they get done in the vibe. Not sure the wife will stand for that one!

If I really get to liking this vibe stuff, I'll probably spring for a 2nd vibe and leave one set up with plastic media to deburr and the second set up with the walnut shells for polishing.

11/26/09

Happy Thanksgiving, Everyone!

Additions to Toolpost Grinder Idea Notebook

Added some new TP Grinder projects to my Toolpost Grinder Idea Notebook page.

What does a first-time Mill user need?

Every now and again, a newcomer wants to know what basic tooling they should acquire. The trouble is, as a newcomer, you're not in a good position to judge (been there, done that). So I thought it would be helpful to create a thread where experienced machinists talk about what the MINIMUM set of tooling to get started with a mill might be. By MINIMUM, we're trying to help folks out who are on a budget, but not go crazy with it. Let's also have a NICE TO HAVE category of the first things you'd buy after you get past MINIMUM. And, let's assume they own no tooling whatsoever, not even a calipers. My list is below. What's your list?

MINIMUM

Workholding:

- Kurt-style vise (or a grinder vise if the mill is really small)

- Parallels

- T-Slot Clamping Kit

Tool Holders

- R8 End Mill Holders

- R8 Keyless Chuck

Note: Some prefer R8 collets, and they're definitely cheaper. I've always used the solid holders and like them a lot better!

Measurement & Layout

- Digital Calipers

- Counterpunch

- Sharpies (Buy a box, they're cheap and hugely handy!)

- Calculator (Online like G-Wizard or handheld)

- Dial test indicator. Don't get a tenths indicator to start, though you could consider 0.0005" indicators.

- Some way to attach the DTI to your mill spindle for tramming. An Indicol or clone (available cheap!) would work great.

Cutters

- Spot drills / Center drills

- Twist drills (I prefer screw machine length as they're more rigid. I almost never use the jobbers, and most peeps will already have some of those anyway)

- Endmills: 1/8, 1/4, 1/2 in 2 flute and 4 flute. At least 2 of each size.

Other

- We haven't talked about how you will cut stock to size. Hopefully you have a bandsaw or chopsaw. Failing that, get a hacksaw.

- WD-40 to use as coolant. If you can, buy a spray bottle and the gallon can of it rather than the aerosol. It's cheaper in the long run.

- Cheap chip brushes

- A decent file

NICE TO HAVE (What to buy after you have a little time with the MINIMUM)

- Make or buy some softjaws for your Kurt vise.

- 1-2-3 blocks, and eventually 2-4-6 blocks

- Edgefinder: I like the electronic kind, which can be converted to probes in Mach3 if you go CNC.

- Small Kant-Twist clamps: Tons of uses beyond clamping. They make great vise stops, for example.

- Deburring cutters. I like the zero flute style.

- Scraper-style deburring tool

- A flycutter or a face mill

- Surface plate and height gage: This one is borderline NICE TO HAVE. But I sure do use mine a lot, especially for layout when manual milling.

Must We Have a Burr When Drilling?

Lately I have seen arguments break out over whether machining will always produce burrs. The answer, so far as I can tell, is "Yes, but not always noticeable burrs." For example, when doing my light cut/high feedrate machining with chip thinning, I see minimal burring. A fellow named TatooMike, who frequents various boards gave a great suggestion about how to eliminate burrs when drilling. He suggests creating a fixture so that the workpiece is stacked atop another piece. You've probably noticed when drilling stacked parts that only the bottom part in the stack gets the burr. If that bottom part is your fixture, you may have saved yourself some deburring.

The other thing I saw suggesed, but haven't tried, is the idea that excessive burring with a twist drill is a result of plunging too fast. Certainly having the proper feeds and speeds helps, but I wonder if slowing the plunge as you near the hole exit on CNC ops wouldn't also be helpful.

11/25/09

Metric, Imperial, Fractions, Decimals, Oh My!

There's a good thread over on the HSM board talking about the pros, cons, and preferability of the various systems. It got started by Doozer, who likes to reverse engineer parts and when he is measuring, tries to determining what the preferences were of the designer so he can round to the nearest value.

I can appreciate the problems with all of these conversions, so I set up a number of features in my G-Wizard Machinist's Calculator to make it easier:

The red underlines point out the unit conversion facilities of G-Wizard...

As you're typing in values in G-Wizard, there are various functions to make it easire to deal with units. For example, as you type in a decimal value, the fractions display will pop up with the appropriate fraction (in this case 3/16's) if you get within a tenth (0.0001) of the fraction. The fractions are good to 32's. If you click the fraction button, you get a popup list and you can select a fraction to be entered as a decimal value into the calculator.

In addition, there is continuous unit conversion going on. By default, the calculator is set to inches and millimeters. Whatever I am typing into the main calculator display is assumed to be in inches, and is continuously updated to the corresponding millimeters. There are lots of other unit conversions available. Want to switch? Click the "<-Use" button and the units swap places so that now you're typing mm and getting inches back.

Unit conversions even extend to angles. There are certainly degrees and radians, but the D:M:S button lets you enter degrees, minutes, and seconds and convert that to decimal degrees or radians for entry back into the calculator.

11/24/09

Another Shop for the Hall of Fame

I collect pictures of great home shops and put them in my Home Shop Hall of Fame. If nothing else, it's inspiration and sources of ideas to improve my own shop and its organization. The latest addition is RTravis100's shop which includes a Haas Super Mini Mill 2:

StorLoc wall unit is nice!

11/22/09

Expanding Studs for Fixturing

I like Mark Hockett's fixturing idea. He uses some expanding studs for fixturing a piece. That way, there's not even a bolt head standing proud to run into with the cutters:

Expanding studs on the fixture and ready to go...

A stud looks like this. Through bolt with tapered head...

The head drives into the expanding part as you tighten it...

Here is a part being tightened down with a hex key...

11/18/09

Glacern Machine Tool: Great Tools for Less, Crash Course in Milling Videos

I've recently been enjoying some new tooling purchased from Glacern Machine Tool. They are such a pleasure to do business with. The tooling has that super high quality feel that puts it a notch above a lot of other tooling that is similarly priced. And the prices are darned hard to beat, especially while they're running their Black Friday Specials.

So far I've purchased a couple of ER32 collet chucks, a 3" 45 degree face mill, and a 6" premium vise. I keep finding more things I need, but let me comment on the face mill, and then on something else I need. I haven't tried the rest of it yet, and the something else I'm about to order as soon as I get this written!

I had a little bit of time late last night (my work day often extends longer than I wished!) to try the new face mill. I ordered the 3" 45 degree lead angle face mill along with 2 sets of inserts. I've got the general duty inserts, as well as some extremely sharp inserts intended for milling aluminum. For reference, I also have a 3" face mill from Lovejoy (225 series) and a 2" from Iscar that takes APKT inserts (Helimill series). The other two face mills are 90 degree lead angle, so they cut a square shoulder. I've wanted a 45 degree face mill because I've heard from a number of sources that they leave a finer surface finish if you don't need the square shoulder. Most of my face milling is just surfacing stock square, so the 45 would be ideal.

I assembled the face mill onto its R8 arbor and then installed a set of the razor sharp aluminum cutting inserts. I set up for an 0.040" depth of cut on a block of aluminum, cranked the spindle speed all the way up, and made a very slow (4 IPM) pass just to be sure everything was working okay. This cutter was so quiet, my brother (who was watching) and I couldn't hear it working. If it hadn't been for the chips flying, we would've thought it wasn't actually engaged in the cut but was moving above the workpiece. And the finish was excellent. Easily the best finish I've yet seen come out of my shop.

Now we were curious to see how fast we could feed without compromising the finish. 4 IPM was obviously too slow for this cutter by a lot, and we only made such a slow pass to ensure all was well. I cranked in another 0.040" cut and tried a pass at 30 IPM. Another excellent and very smooth result. Great surface finish, almost indistinguisable from the really slow pass. The chips themselves were gorgeous little corkscrews about 3/8" long. Clearly a little more feedrate would be beneficial.

OK, at this point it was time to explore the limits. I fired up G-Wizard (I knew roughly the parameters from experience with prior cutters) and wanted to see what it recommended as a cut. I got back 900 rpm and about 55 IPM. That would be blistering. The 30 IPM run had really thrown a shower of chips and this was almost twice the speed. We tee'd it up and let it lose and...

DOH!

The spindle motor stalled! Well, you know, that's what the big red E-Stop button is all about. No real harm was done, but I sure did chip the heck out of an insert. First thing was to rotate the insert in its pocket to expose a new edge that wasn't chipped. Second thing was to figure out what had happened. I looked back over the G-Wizard parameters to make sure I'd read everything right and found the problem. This cut called for an estimated 1.4 HP. The IH mill only has a 2 HP motor on it, and we were running at a high spindle speed, so the gearbox was giving no torque multiplication. My guess is the 2HP is a little bit optimistic as it often is for import motors. I'll have to try this cut again when I swap my new Baldor 3 HP motor on with the VFD and belt drive.

Meanwhile, I set a horsepower limit of 1.0 HP in G-Wizard, and it automatically scaled back the feedrate to 38 IPM. This produced a gorgeous finish very quickly! The 1.0 HP limit gives me a little safety margin, as 1.4 was clearly too much for these conditions. Another approach would have been to take a 0.020" cut which is half as deep.

All in all, I am extremely satisfied with the facemill, even more so considering it only cost me $99.

A couple more thoughts on Glacern. First, I've really been enjoying their video series, "Crash Course in Milling." If nothing else, you have to love the title, but there is a lot more there to like as well. Production quality is great, and there's a lot of good information. I was watching the latest release, "Tool Holding," when I came across something else I had to have (I hate when this happens). Their keyless chucks are set up for spanner wrenches. None of my keyless chucks have been set for spanner wrenches. Consequently, if they get too tight, you have to take a pipe wrench to them, an act which is very unsatisfactory, to say the least. What a great idea!

So, looks like I will need to put together another Glacern order before the Black Friday sale ends!

11/17/09

New Chip Thinning Cookbook

I've added a new learning page on chip thinning and other forms of cutter feed and speed compensation. Check it out to understand more of the tricks that are built into my G-Wizard Machinist's Calculator.

The geometry of chip thinning...

Auto-Mill: Use Mach 3 as a Power Feed

There are times when CNC is just wonderful, and there are times when you're thinking, "Man I could do this faster manually." Mach3 provides a set of G-Code Wizards that are kind of in between. For quick and dirty work, I often resort to setting the Mach3 jog to my feedrate and just holding down the arrow key. I know Hoss of Hossmachine fame added toggle switches in parallel with the jog keys so he can flip a switch and just let it feed.

But what if you had a Mach3 screen that was all set up to make it easy to treat Mach3 like a power feed? Enter, Auto-Mill, by Jerry "Ozzie" Pryor:

Looks very cool!

I currently use the Aqua screen set by Ger21, but I may have to look into grafting Auto-Mill into that screen set. It sure would be handy. I suggested to Jerry that he add push button peck drilling as well. It'd be real nice to be able to just pop a hole right under the spindle with a minimum of effort. Currently I use the MDI to enter a drill cycle, but it could be done so much more nicely on a Mach 3 screen.

Jerry offers a complete screen set with Auto-Mill, comprehensive electronic probe functions, and a lot more on eBay. Just track down seller "Ozzie34231".

Tapping With Ye Olde Butterfly Impact Wrench

Josh from the HSM board sent me a PM this morning. He has made a real nice video on YouTube of my idea of tapping with the Butterfly Wrench:

Tapping made easy...

You need a set of Irwin's tap wrench adapters for a socket wrench, I got mine from Enco:

It's amazing how well these little wrenches work, and they're dirt cheap. I have one built into my powered drawbar, one loose, and one attached as a "hand powered drawbar" to my 2nd mill:

Just reach up on top of the spindle with this and tool changes are a snap!

People worry these impact wrenches will break their taps. I haven't broken one yet, but I'm not sure I'd use a really tiny tap in the impact wrench.

To reduce the likelihood of breaking a tap, consider the following:

- Always use tapping fluid. I like tap magic and keep a can near the vise where most of my tapping occurs. I apply it liberally to the tap. Josh is spraying on some WD-40, which ought to work too.

- There is a built-in regulator on the wrench. Turn it down for smaller taps so you don't have full torque. These little wrenches don't have a ton of torque anyway. You can see in Josh's video his wrench really slowing down when it starts to cut.

- Use sharp taps. Josh is using a hardware store tap. They work, but there are better taps to be had. Do yourself a favor and get some form taps and some spiral taps for the hardware sizes you use most often in your shop. Wait until they go on sale and buy a few in each size. Be sure to get quality US made taps. Try them by hand first and you'll be amazed at how much less pressure is needed to tap a hole. The spiral taps extract the chips right up out of the hole very nicely. They designed so you don't have to keep reversing to break the chips, just keep on going. Form taps require a little more effort. They don't make a chip at all, they cold form the metal to produce a thread. I read on one manufacturer's site that they are 4x stronger (and therefore less likely to break) than cutting taps. I prefer form taps in aluminum, but there is a limit to how hard a material they will cut. Mild steel at best.

- Make sure your've got the right-sized hole! My G-Wizard Machinist's Calculator will figure that out for you based on what % thread you want to cut. If you're at all worried, choose a lower % of threads. The threads won't be as strong, but the bigger hole will make it easier to tap.

- It really matters to thread along the axis of the hole. That means the tap has to go in straight. There are lots of ways to ensure this, but a moment of inattention is all it takes to blow it. Once you have cut threads at an angle, it's too late. The smaller the tap, the more sensitive they will be. For real small taps, I use a piloted tap wrench in a drill press, a milling machine, or my lathe tailstock.

Eventually, I am going to build a tapping arm, which makes it easy to tap holes that are perfectly vertical:

Commercial tapping arms use air drills. They're available, but you want one with a low rpm and easily reversible with your thumb. So far I haven't seen one like that for less than about $500. So I use my Butterfly Impact Wrench which cost less than $25. Try it, you'll like it!

11/15/09

CNCCookbook Gets a New Bandsaw

It has been a busy weekend for the CNCCookbook.

I have had the ubiquitous small Harbor Freight horizontal bandsaw for a long time. I found I use it more often in vertical mode than horizontal once I made a little table for it. The little saw has been handy, but it's just too small for many projects. A lot of stock and machining time can be saved by using a bandsaw to cut things closer to size. A rule of thumb is to get within about 0.100" of your milled cut. So I've been on the lookout for a bigger saw for some time. I wanted something local and good sized.

The new (to me) saw is a Delta Rockwell 18", which is quite a bit bigger!

It looks gorgeous and new with only has 500 hours of running time on its Hobbs meter:

This saw looks identical to the saw we had in my high school shop class, although it is much newer. Nice to be able to put a piece of American Iron still in good shape into my shop. This machine is capable of cutting either wood or steel, so it has a nice broad range of speeds that include a 2 speed Lo-Hi gearbox and a variable pitch pulley to change speeds within the range.

Now I will still need to come up with some 3 phase power before I can fire it up!

Chip Thinning: Cutting Steel at 35 IPM With HSS on Bechtop Mill

There is quite a bit of skepticism about this when I talk to some machinists. For example, over on the HSM Board a discussion recently broke out where I was accused of pushing feeds and speeds that were only attainable by professional machinist's with fancy tooling and $100K milling machines.

Here is a video of my RF-45 bench mill cutting mild steel at 30 IPM:

This cut works because of a phenomenon called "Chip Thinning". Any time you take a depth of cut of less than 1/2 the diameter of your cutter, the cutter actually cuts a thinner chip than the normal equations would predict. If you can reliably predict this effect, you can speed up your feedrate until you're producing the recommended chip thickness (chipload or inches per tooth). The difference in feedrate is often surprising.

In the HSM discussion, 6 IPM was viewed as aggressive, yet the poster was trying to make a cut 50 thousandths thick with a 3/4" endmill. 50 thou is a lot less than 1/2 the diameter of the endmill, so the chip thinning effect was significant.

Adjusting for chip thinning really just puts you back where you thought you were with the old math. It was invented by the high speed machining crowd, but it works great for regular low speed machining too. The only issue is that its more work to calculate your chip-thinning-adjusted feedrate. Being able to do this automatically is one of the reasons I created my G-Wizard calculator.

During the Beta Test period, everyone is welcome to try out G-Wizard. The page gives details on how to get access.

BTW, the part in the video is a knuckle joint for my recent coolant mister project:

Finished a New Coolant Mister Last Weekend

But I'm just now getting the article written and photos posted. The full details are on the project page for the mister. It looks like this:

Originally I was going to build the mist nozzle/mixer too, but I got an eBay deal on a Noga unit...

11/14/09

Mitutoyo 190: Swiss Army Knife of Calipers?

Saw this on PM after a kind soul brought it to my attention via PM:

That's cool!

Wouldn't work for me, being a child of the digital rather than the vernier age, but it sure is cool!

I'm wondering if there isn't a project here somewhere to adapt a standard digital caliper to do all these tricks.

11/13/09

Glenn Wegman's Indicator Holder

I really liked Glenn Wegman's indicator holder because it has a knurled wheel to make easy to turn the spindle while using it:

11/8/09

How Accurate is Your Co-Axial Indicator?

There is a raging controversy over on the HSM board about the utility and accuracy of the Blake Co-Axial indicators. First, let me open by saying I've got a cheap knock-off of one and I really like it a lot. It's the easiest way I know to center a round feature (hole or boss) under the spindle. I've seen people use them to align their lathe tailstocks back to center too, though I've never tried that. Here is a picture of a real Blake, mine is an inexpensive Chinese clone:

Blake Co-Axial Indicator. Note that the indicator has graduations of 0.0005"...

What I like about my Co-Ax is that it is a really fast way to set up on a feature and be accurate to say 0.001". I don't claim more accuracy, although Blake apparently claims 0.0002" for theirs! Nothing could be simpler to use. Install the indicator, start the spindle rotating (not too fast!), and turn the handwheels (or bump your CNC jog) until the needle on the indicator holds still. Done!

Much of the controversy has to do with the cosine error of the long probe that sweeps the feature. There are more accurate ways to center over a hole if you want to take the trouble. A tenths indicator and a rig like a "Zero Set" or similar would be a lot more accurate than the Co-Ax, but it takes longer to futz with. BTW, my Zero Set was made by the Fidgeting Widgitmaster of CNCZone. He periodically does a run of these and sells them on eBay. They're absolutely gorgeous and I highly recommend dropping him a line if you want one:

With all that said, I reach for the Co-Ax far more often than the Zero Set, just because its faster and easier if you don't need the maximum accuracy. But how accurate is it?

It occurred to me that answering that question would be a perfect task for my new G-Wizard Machinist's Calculator. If you want to try G-Wizard, go to the G-Wizard page and there are directions for how to get signed up for the Beta Test.

First, consider the mechanism of the Co-Axial Indicator. It basically uses a probe that swings a little lever. That lever raises or lowers a ring, and the ring is connected to an indicator. The lever on mine is about 1/2" long. So an important question to understand is how far must that lever move in order to move the indicator a particular distance, such as 0.001"?

Here is the geometry:

And here is G-Wizard calculating that the angle of the swing is 0.1146 degrees to move the indicator 0.001":

Given that knowledge, its easy to use the same calculator to figure out for a given probe length, how much it deflects to generate the same angle (0.1146 degrees)?

Here is our result:

So the accuracy is based on how well you can read the indicator. As mentioned above, the Blake's is calibrated to 0.0005" increments. You can certainly see that much motion of the needle, in fact it looks huge. Can you see the wiggle of 1/5 of a division? I certainly can, which would get me to the 0.0001" column. The longer the probe, the less accurate you will be, but I seldom use a probe longer than maybe 3", so the accuracy of the indicator is not too bad.

11/7/09

CubeStudio's Ridiculously Cool 4th Axis/Lathe

I don't get over to the ArtSoft forums as often as I should. I was checking in this morning and noticed I had missed out on some very cool posts. Probably the best was this one. The videos speak for themselves:

First generation, built on a Spindexer...

Latest generation, including rigid tapping!

Grinding ballscrew ends...

He is driving the spindle with a pretty beefy servo, and he has a index pulse from an opto switch as well. He's written some macros to allow Mach3 to switch back and forth from lathe spindle to A axis indexing mode in support of all this. I love the lathe gang tooling mounted on the side of the mill head. For certain kinds of jobs I would think this little rig would be amazingly productive.

How Many Plates, Er CNC Machines, Can You Keep Running at the Same Time?

I've seen numbers up to maybe 4 or 5 machines. Load one up, hit Cycle Start, go to the next one, rinse repeat. If you can keep 4 or 5 machines going at the same time, that's hot stuff. Most shops think about their business as though the machines are "hourly income". A machine makes say $75/hour. Keep 4 of them going with one operator and that's $300/hour.

But with so much going on, it's easy to lose some minutes here and there. You walk away and get focused on something, the machine finishes, and you don't notice. What to do?

I liked the note in this PM thread about a guy named "Ox" who started clipping egg timers on to his clothing. One for each machine. Start the timer when you hit cycle start. When it beeps, it's time to go back to check on the machine.

11/5/09

Single-Edged Razor Blade Line Pivot

A diagram for a CNCZone discussion:

11/3/09

Nice Rigidity Bump Up for Small Sieg Mills

Dougal over on CNCZone has the right idea. He bolted a nice piece of channel to the back of his Sieg X2's column. It even looks factory:

Now why the heck doesn't the factory do that?

11/2/09

The Case for Parabolic Drills and Some New G-Wizard Functionality

It is always hard to drill deep holes, where deep is defined by a hole that is many diameters of the drill bit deep. I recently came across a question on CNCZone that started me doing some research on the topic of parabolic drills. Parabolic-style drills were developed in the early 1980s. They use a heavier web to create higher rigidity and increased flute area for chip removal on deep-hole drilling operations.

Precision Twist Drill has a nice discussion on their site of how to vary feeds and speeds to accomodate deep holes when using regular and parabolic twist drills. I was so taken by the CNCZoner's question and that nice discussion that I wound up adding a bunch of functionality to my G-Wizard Machinist's Calculator.

The new functionality is both to implement the feeds and speeds adjustments recommended by Precision Twist for deep holes, but also to give recommendations based on the hole depth. For example, it suggests when you need to use a peck drilling cycle (where you drill down a little ways and then retract to clear chips) as well as when you should be considering a parabolic bit instead of a regular twist drill.

The question the CNCZoner raised was what feeds and speeds to use when drilling a 0.201" hole 3.5" deep. That's over 17x the diameter in depth, so a parabolic drill is definitely called for!

Here is what G-Wizard shows when you enter those parameters:

Note the box for Parabolic is checked, which tells G-Wizard we want to use a parabolic drill. Also, it is recommending a peck drilling cycle (DUH!) for this 17.412x Diameter hole depth. If we enter a less severe hole depth, 0.2", it recommends 3800 rpm and a feed of 16.85, whereas you can see from the diagram it has compensated for hole depth and slowed down both the feeds and speeds. The feed is slowed as a result of the spindle rpm. Parabolics don't need further slowing. A regular twist drill would also get feedrate reduction on top of that.

11/1/09

More Clamping Tricks

Ray Behner's clamping trick spawned some more good ideas:

I'm going to have to CNC a big table clamp like that one on the right!

Of course the table clamps can be turned on their sides to accomplish the job in the bandsaw vise!

Earlier Entries in the Blog...