View Full Version : What you did today/shop-made tool/gloat combo

tyrone shewlaces
02-27-2011, 04:05 PM
Threw this together over the past couple months. It's intended to do isolation milling of PCBs. I piddle in electronics some and this should be handy. It could also mill some small parts in softer materials and of course do engraving.


Machined almost all the parts from stuff pulled from the "scrap" pile. The bought stuff comes in at around $100 (driver board, power supply, various hardware). The linear bearings and steppers were also in my spare parts pile, scavenged from stuff which was pulled out of service.

The table is just flat because for what I intend to use it for I'll either be using CA glue/acetone or double-sided tape.

02-27-2011, 04:16 PM
Very impressive work.

I can't tell which motor runs which axis.

Is the motor on the left pillar for the z-axis with a keyed shaft, or is it for side-to-side using a leadscrew ? And I take it the fore-aft motor is hidden from the camera.

tyrone shewlaces
02-27-2011, 04:36 PM
Yea it's a gantry style.
Top of left post is the X-axis motor. Y-axis is way low and behind the table, but you can see the lead screw sticking out from under the front of the table (just 5/16-18 threaded rod throughout). Z-axis motor is mounted on the back of the block which slides L-R on the gantry rods - belt and pulley to transfer motion to the Z-slide on front. I hid it back there to keep things compact.

Working envelope is ~ 8"x8" X/Y and 3" Z



02-27-2011, 05:32 PM
That's a neat set up, any plans to scale it up to do larger projects?

02-28-2011, 05:39 AM
If you stretched the design a bit T/S, you could process 6' x 3' sheets. Might have to use 3/8" leadscrews though.

Regards Ian.

John Stevenson
02-28-2011, 07:16 AM
That's a neat little thing.
I bought a Techno Isel router a while ago with no motors or electronics, been robbed to keep other going.
Real fun machine, I'd like to spend more time on this but other things keep getting in the way.

02-28-2011, 09:18 AM
Cool,I like it! One thing for sure you shouldn't have any trouble with those columns flexing under load:)

02-28-2011, 12:46 PM
Any pics of the parts yet? :)

02-28-2011, 03:24 PM
Looks to be perfect size for average PCB machine, certainly anything short of major motherboard construction.

What size steppers, and which driver did you choose?

Are the lead screws driven 1:1 off the steppers or are they geared down somewhat?

02-28-2011, 05:29 PM
Nice job! I've long had my eye on making one of those.
What are you using for the stepper drivers and software?

Thanks for posting!

tyrone shewlaces
02-28-2011, 05:58 PM
I'll try to give answers.

Did this last night. Have to tweak the generating of the code - traces ended up being too narrow so must be cutting wider than it's supposed to. Not a big surprise. It will take a little T&E to work out the method. Isolation was done in three passes (6 between adjacent traces) so traces can definitely widened up with a simple parameter adjustment in the PCB-GCODE step (see below).


Machine can obviously drill the holes too, but I didn't need to test that as much as the trace milling, so maybe I'll show that a little later.

Stepper driver - about $33 + shipping from eBay:
(They've upped shipping $10 since I bought mine. Uugh)

Power supply (24V 6.5A) was about $15 + shipping from MPJA:
(Now out of stock. Uugh)

Eagle for PCB design. It's free for small boards, pay for unlimited (?) size files. Seems to be the industry standard for most folks I run into.

PCB-GCODE for generating G-code from the Eagle file for both isolation milling and hole drilling. It seems to work pretty well. And it's free !
This runs "inside" Eagle and it's easy to deal with.

Gsuite for optimizing the code generated from PCB-GCODE. Basically eliminates a ton of rapid moves from what PCB-GCODE generates for whatever reason and does a very good job of it. For a slow stepper motor machine, it's a godsend. It has a couple other handy utilities as well. Pretty neat. Also free.
Gsuite v1.3 (http://callkck.com/storage/GSuite/Gsuite_v1.3.rar)

Mach 3 (http://www.machsupport.com/) for running the machine. About $150 but all I'm doing is running the G-code to the machine and for that EMC2 (http://linuxcnc.org/) would work just about as well (some say better) for free. I think Mach 3 is a little overboard for this, but I bought a copy a while back so I'm using it.

That's it. If you want to make parts or do engraving, you may need to use some kind of CAM software for generating the G-code depending on how complex you get into. So far I haven't looked into that, so you're on your own.

Steppers are NEMA 23 and 1.5A, so about as small as this frame gets I think. For the force required for an engraving bit and those little bitty drills, these are more than adequate.

Lead screws are 1:1. Just 5/16-18 threaded rod. I was finicky about picking a pretty straight one and it wasn't too bad. Seems to be plenty accurate enough for the purpose, and dirt cheap. 200 Steps per revolution on the motor (which is typical and easy to find) and 18 tpi gives a nominal positional accuracy of .00028 per step, so more than adequate for me.
I machined the nuts from delrin (yer basic drill & tap) and that makes for a free-turning but close fit. Of course wear & tear will probably loosen things up over time, but they are easy to make and at the moment it indicates zero backlash.

And finally, no the columns are definitely not the weak link. Nice and roomy for routing wires through too. :D

Oh yea. Downloaded the board file in Eagle from here in case you are curious what it is:

02-28-2011, 06:36 PM
I'll try to give answers.

Did this last night. Have to tweak the generating of the code - traces ended up being too narrow so must be cutting wider than it's supposed to.

My money would be on the Dremel tool quill as the source of the problem.They aren't at all ridgid,I've always wanted to make a better quill and use the Dremel to drive it through a flexible coupling for that reason.

tyrone shewlaces
02-28-2011, 06:46 PM
No doubt the dremel is running out and cutting wider than the tool is supposed to. But that can still be modified in the software chain to still make a working board. The quality of the milling is workable, but the code called for too wide a channel to be milled and that can be reduced for sure.

A better spindle is on the drawing board and it was from the beginning, but a dremel was an easy way to get it working quickly. It's a quick bolt-on plate which can easily be switched out to install a good spindle (or laser, or extruder hehe, etc.)

Actually, here's a pretty darn good deal for a decent spindle if a guy didn't feel like making one from scratch:

02-28-2011, 06:46 PM
My money would be on the Dremel tool quill as the source of the problem.They aren't at all ridgid Yup, Dremels suck for precision work.;)

I ran into the same problem with my cobbled-up CNC for r/c making model airplane parts. I quickly switched to a little Porter Cable trim router. MUCH better. A real collet, good bearings and will howl away all day with nary a whimper. When I say howl, there's the rub. Dey do make sum racket!

edit: Oops, Tyrone's got a handle on it already!

02-28-2011, 07:12 PM
You can take the Demel tools apart,and add packing around the ball bearings to tighten up their spindle wobble. The bearing housings are just cast into the plastic,and do not fit the bearings very well.

John Stevenson
02-28-2011, 08:57 PM
A lot of these cheaper spindles do have run out.
I saw this setup at last years show which makes a lot of sense.


Setup on right.
Just a jig to hold a DTI so the max run out can be seen and the cutting edge of Vee tool can be set to the point of least run out putting the point of max run out into the relief section.

Not my work and to be honest not sure who's it is.

tyrone shewlaces
02-28-2011, 10:03 PM
That reminds me...
I was wondering today what I'll use to indicate a location on the table considering I have (at the moment) only 1/8" shank possible and only about 2.5" maximum Z clearance. Specifically, I think dowel pins will be used for a couple different things and sweeping them to locate and set the work offset with some precision.
I have a couple thoughts, but I thought maybe somebody may have a trick they've used for a setup like this.

Remember, with steppers and no encoders anywhere, the machine won't really be able to be "homed". I'll have to indicate some reference probably every time it's powered up and likely at other times on occasion too. Z is easy enough, but not much room for a dial indicator to pick up X & Y.

I need an itty-bitty DTI, hehe.

02-28-2011, 10:13 PM
Can you just drill a hole in your table (1/8" or whatever) chuck up a 1/8" (or whatever) dowel in your spindle then jog around until the dowel wil slide in and then hit the X & Y zero command in your control program? That's what I did on my router. Crude I guess, but it worked.:)

tyrone shewlaces
03-01-2011, 12:04 AM
Can you just...

Grandpa taught me never to start a sentence like that.;)

But yea of course that would get you into the ballpark. So would just a pointed tool and a pin point on the table. And I do that sometimes on a manual mill depending. But with CNC you get no feedback so can't tell by feel if you're slipping in easily or just cramming it into your nice, precise reference hole. I guess you could use a two-piece, collar-on-a-pin thing and slip a 1/8" hole up it and into a 1/8" shank cutter and get some feel. Might do something like that for the quick & dirty.

I'd kinda like to use some kind of dial indicator arrangement though. I think I have something brewing and I'll kludge it together tomorrow if I have time.

J Tiers
03-01-2011, 12:36 AM
We had a commercial version of that, German, but not built as well.... it was "down" a lot.

We ended up just driling holes, and doing the etch chemically, but the routing may work for you.

Nice work

03-01-2011, 09:42 AM
Grandpa taught me never to start a sentence like that.;) My Grandpa wuz a country boy.:p

My router X/Y table ran on drawer sides so I was able to jog and make fine adjustments until the table quit moving visibly as the pin was plunged into the hole.:eek:

Not the most rigid setup for sure but it cut balsa ribs & bulkheads with surprising accuracy. I'd love to re-do it someday with sections of oil pipeline like you used in yours.;)

03-01-2011, 10:04 AM
Hey guys,

Really cool little cnc router Tyrone. Might be a good way for an old duffer like me to dip his toe into the cnc world without breaking the bank.

Has anybody tried using a Roto-Zip Tool instead of a Dremel in this application? I have both that I use in carpentry mode, The Roto-Zip seems much heavier. It is capable of similar speeds as the Dremel. Just wondering.



john buck
03-01-2011, 10:48 AM
Your post gave me some great ideas for my next build , you did a neat
job on yours. Did you have any trouble with those TB6550 drivers.
There is so much negative publicity about them on theCNCZone.

tyrone shewlaces
03-01-2011, 06:16 PM
Did you have any trouble with those TB6550 drivers

The verdict isn't in on that yet. I had issues with Z missing steps pretty bad at first. I tuned (in Mach3) the X&Y motors and the best I could get out of them is 13 ipm. I guess that's not bad for steppers at a little over 200rpm. Z was missing steps really bad at that speed - and losing position of course. I fiddled with it and fudged with it, changed motors, changed pin assignments, switched Z with Y&X and various other hair-pulling. When driven out of the driver by the X or Y-axis connections, the motor ran fine at 13 ipm so the problem was in the driving and not the motor. So determined that either 1) the Z-axis data stream coming from my laptop is low quality (likely - and I feel lucky for it to be working with a laptop at all) or 2) data stream is clean but the pulses coming out of the driver are unreliable on z-axis. I suspect #1. I will eventually test it with a tower and see if things improve. For now, I was able to tune Z for a max speed of 5 ipm and it repeats fine at that setting with this laptop. Whew! Not ideal but it's doable. No issues other than that - it seems to work just fine otherwise. Has a good three or four hours of solid motion control on it in hour-long (plus) chunks and it all seems to work OK. For the money I paid, I'm happy enough with the performance.

Here's what I spit out today for indicating a pin from the spindle.


Those bitty Federal indicators are just cute. With the short plunger coming out of the side, this arrangement will allow me to put it into either a 1/8 or 1/4 collet (for later) and sweep a pin which simply needs to stick up from the table at least 1/4". Total height is 1.5" so that ought to work. Just a .001" indicator which should be plenty good for what I need on this machine.

With this I can now install a reference pin permanently in an out-of-the-way location on the table, and I think I'll put some various holes to slip pins in & out for fixture setups. That way I can have repeatable setups so I can throw a fixture plate (like 1/8" aluminum or masonite or something) from the eventual collection back onto the table and have quick, repeatable setups.

03-02-2011, 11:09 AM
But with CNC you get no feedback so can't tell by feel if you're slipping in easily or just cramming it into your nice, precise reference hole. Wouldn't a center finder -- the kind with a spring in the middle -- work for this? I'm told your fingers can detect a .001" error on one of those.

03-17-2011, 03:05 PM
Ok it took me so long to post the thread should be "what you did last weekend"
Here is 20 little pins I did for one of my clients...(my real employer:D )
It was a real pain to hold to cut the little grooves since the pins are only 11.5mm long and 9mm thick.
I had to make a little "collet" just a hollow bar with the same ID as the parts OD and then I cut a slit in one side with a hacksaw.
Can somebody please let me know if that is common practice and what is the pitfalls in doing that.
I'm pretty sure I missed something or maybe a simpler way of doing it ...Rack your brains guys. :D
Here is the entire job on a pack of 20 lucky's can't believe it took me 6 hours to do.

tyrone shewlaces
05-22-2012, 01:59 PM
Did you have any trouble with those TB6550 drivers.
There is so much negative publicity about them on theCNCZone.

Well after about a year of pause, I figured it was time to revive my CNC project and get the thing to finally being "done", i.e. actually able to make things and do a decent job of it.

First, to answer John's question, I did finally determine that my cheap TB6550 driver board I bought off eBay turned out to be the source of the low performance of the steppers, so I bit the bullet and ordered a Gecko G540 and it should be here tomorrow. I won't really have time to play with it much until this weekend, but I'm looking forward to seeing a big improvement.
Those TB6550 driver boards do have a lot of negative reviews and I've read through a long post where some folks have looked into them and corrected errors or upgraded things to make them work much better. But I figured I'd just skip over the uncertainty and purchase a driver which has proven over and over to perform well, at least for now. I'll try fixing that cheap old thing later on I'm sure.

I also considered purchasing a smoothstepper, but then I read that several people have had problems with them as well so figured if I want to add an interface like that I'll just look into it later and make sure I get something proven to work reliably on that as well. I hear that the ethernet smoothstepper is supposed to be much more reliable, but at the price (quite a jump from the USB for whatever reason) there might be a better solution anyway.

So by the end of this weekend I should have some results on the drive system to report about.

I ended up making a spindle and tried a motor on it which didn't work, then made a coupler to drive it from a dremel which exposed a bad rattling (maybe just dirt in the bearings) so that didn't work out so well either.

A pic of the unfortunate spindle experiment:

So I'm planning on trying out one of the high-speed air-cooled spindles from eBay. I queried about this here in a post a while back and determined that I should get the spindle separately and purchase a separate Hitachi VFD. So that's an upcoming upgrade too.

So the machine initially cost roughly $100 to build and now I'm biting off another $600 or so which makes no sense, right? Well there is a more complex master plan of course.

A while back I purchased a stepper driven CNC device for scrap/parts price. It is a little larger, much heavier and more precise. It appears to have been some kind of video inspection device of some kind maybe. I'll snap a photo of it and post it later. But the lowdown is that I should be able to use the new drive and spindle on the old machine to make some PCBs for decent home-brew stepper drivers which will ultimately be installed on itself so I can move the Gecko to the new, bigger machine. At that time I will move the VFD spindle to the new machine as well and work out a different spindle fix or solution for the smaller machine.

Redundant? A little. But the bigger machine will be rigid enough to do some milling and of course the larger work envelope won't hurt. Also, the bigger machine is too heavy to be portable while the smaller one is very easy to carry and transport. Sometimes I do demonstrations or the like so a portable CNC machine will be handy now and then. I could even loan it out to the local robotics or MAKE clubs or something like that now and then.

OK, that's it for now. More updates soon.
This stuff sure is fun.

tyrone shewlaces
05-23-2012, 09:48 PM
Ups delivered the Gecko today already. I'm currently loading XP into an old desktop so I can start from clean scratch. I even found a spare little 1024x768 LCD monitor for it - perfect.

I have a couple steppers in the parts bin I can mess with it a little bit. I actually loaned the little machine out a few months ago to my electronics guru so he could mess with it and try to learn Mach a little, but he didn't find any time anyway. So we're getting together this weekend so he can bring the machine back and we can start configuring things.

Trudging forward...

tyrone shewlaces
05-27-2012, 02:36 PM
Well heck and blast.
I made up the DB9 connectors with the current control resistors tucked inside and it all came out pretty nice. So set it all up according to the Gecko documentation and give it a whirl. Tuned up the motors to work as good as I could, but either my laptop parallel port is very weak and buggy or my motors are crap. Either could be true and possibly both. It works better than it did with the cheap Chinese driver, but it's still not good at all.

The laptop is being replaced by a nice little mini ITX system I've ordered and will arrive later this week. That needed to happen anyway and we'll see how that shakes out. It's a 2.13GHz processor so I should be able to pick a higher kernel speed in Mach3. Also tons more memory than what I'm currently struggling with at 2GB, which maxes out 32-bit OS Mach3 requires anyway. Yea I know these days 2GB RAM isn't "tons" but it's 8x what that laptop has. Pitiful, eh? Anyway, that weak link will be happily replaced.

So I wonder if experienced folks can recommend a good little NEMA23 motor to replace the ones that are on this machine if it comes to that, which I suspect is likely. I think these motors I've got are just not well-suited for a machine like this, being too small and also some kind of "special" with a model number that isn't found on the Vexta documents. Good brand, but not good for the purpose I suspect. They are about as small as a NEMA23 motor comes and who knows what their ratings are. I have minimal specs (resistance and voltage).

I've seen motors on eBay for decent prices, but since I've already had problems with these, which were inexpensive when purchased by the guy who donated them to the project to begin with, I'm hesitant to spend money on import no-name steppers which may not perform any better. They might work just fine, but I have zero experience beyond this machine so I sure could use some motor choice recommendations.

This machine is small and will likely do little more than engraving. At most it will drill 1/8" holes or mill plastics or PCBs with a 1/8" mill.

Here's a lot of 10 which are actually 15mm longer than what I have. Smallest I could find though:
(link) (http://www.ebay.com/itm/10-pcs-nema23-stepper-motor-9kg-cm-1-8-56mm-length-CNC-Milling-engraving-/320913621543)

Here's what seems like might work well, but will it?:
(link) (http://www.ebay.com/itm/3PCS-Nema-23-stepper-motor-290oz-in-CNC-router-or-mill-/220800592561)

Kelling CNC offers what appear to be similar motors, i.e no branding and sparse specifications. http://www.kelinginc.net/NEMA23Motor.html
Note the one at the bottom of their page (the Vexta ones). They may be better than what I've got, but are they?

The videos I've seen with Mach running steppers through a G540 show smooth running and relatively quiet operation. Mine have very little poop and are very resonant at slower speeds despite adjusting the trimpot on the G540. For a machine this small, it seems like it should be pretty basic to make it perform smoothly and reliably.

Thanks for any advice.

05-27-2012, 09:25 PM
I would relax..."Don't worry, be happy" until you get your new PC hooked up to it. I s'pec that'll help a lot.:)

tyrone shewlaces
05-28-2012, 02:23 AM
Yea you are correct.
I hooked it up to a desktop from the boneyard anyway and it wasn't working any better. Then I discovered that the two bad-running motors had a wire come loose on each of them. Hooked it back up snugly and it seems to work like a champ all of a sudden. Imagine that.

When the new system arrives I should be able to increase the kernel speed and get higher speeds from the motors if I want. Plus the not having to wait a couple minutes for this old thing to add 2+2 - it's taffy slow. It sure is much better with the Geckos than with the Chinese driver though. What a relief.

Thanks for the reply.

tyrone shewlaces
05-28-2012, 12:49 PM
Wow the Gecko is working great. With the Chinese driver I could get max feedrates of 13 IPM on the table and 4 IPM on Z. Now I am repeatably getting 40 IPM on all axes. This maxes out what I can get with the Mach3 kernel speed, so I may be able to speed that up by jacking the kernel faster once I get the new PC system.

Here's a short video:

05-28-2012, 01:09 PM
Awesome! Sounds like some happy lil' electrons flowing now that you got those Chinese circuits out of their way.:D

tyrone shewlaces
05-31-2012, 10:54 PM
Yes. Some of the better things in life still come from the small American business. ;)

Made a bit more progress.
If you watch the video, you will see that above the spindle there is a bracket holding nothing. I made that to hold a dremel and at first it was mounted at the bottom of the Z-axis plate thing. After I made the new spindle and found that the motor I intended to use on it was waaay too wimpy to work on it, I re-thought and decided to modify the dremel bracket and move it to the top so maybe it could drive the spindle. So I hooked the dremel back up and connected it to the spindle with a coupler and tried it out last night. There is some vibration, which is worse at some speeds than others so I just have to fiddle and get between the harmonic nodes. But it does work OK. I was afraid that the bearings would just burn up at those kind of speeds. I made absolutely no provision for cooling. But it ran for 20 minutes or so last night at about 20-25K rpm and it hardly got warm. A pleasant surprise.

I went a little further and milled flat a piece of plastic to true the table up to the axes and that worked like a champ. I can tape copper clad to the now flat plastic and etch PCBs. I'll be giving that a try this weekend.

Also got the new system built and installed. It's a sweet-running little thing and I've been able to ramp the rapids up to 50 inches per minute. Since I'm only driving my motors at 25V, any faster than that and it loses torque and skips. I'm happy with that. 50ipm is so much faster than I had before that I have no plans to increase the power supply voltage just to get a bit faster rapids out of it. And of course the new system is just generally tons smoother and faster than that relic I had it running on before.

Once I get it etching some PCBs I'll make another small video and link to it.

Getting pretty close now.

Alistair Hosie
06-01-2012, 02:36 PM
I wish I could get myself into cnc but I understand the prinicipal but don't have the energy to start again learning when I am still learning normal machining.I will dedicate myself to that.Anyway I enjoy it too. Alistair

tyrone shewlaces
06-16-2012, 09:34 PM
I finally milled my first usable PCB with my little machine.
It's not perfect, but it would be functional. You'd just have to be a little more careful with the soldering I think.

The method I used to flip the board to mill side 2 was fairly simple. I just drilled holes of a proper diameter to fit a couple small pins I had at 0,0 and 3,0. On this board, the way it was laid out on Eagle had the origin (0,0) slightly off the board outline, so the registration holes will be gone once the board is cut off the material. You could use any two holes, but using the origin for one of them is handy and quick way to get things set up for the flip.

I'm very pleased with the motion of the machine, but the spindle still leaves something to be desired. So I'll be doing something different eventually.

I'm not sure how this occurred, but you can see that the registration kind of got spread out from one side of the board to the other along the X-axis. The motors didn't skip steps, it's just off in the code for some reason. I'll probably try some other method of generating the code and see if I can fix that. The PCB-GCODE thing is a bit awkward to use anyway, so maybe the next thing I try will be better anyway.

The pictures didn't turn out very good. It looks quite a bit better in person even if it isn't perfect.

Side 1:

Side 2:

Here's a short video of the machine making the board this morning. There is no sound on purpose - it's just an annoying whining sound from the noisy spindle, and the sound and video got progressively out of sync as the video progressed for some reason, so I just left it out:



tyrone shewlaces
10-14-2012, 07:50 PM
Reviving this old thread one last time. The project is finally a success.
I finally got my little machine working pretty well. Yaaaaay!!!

I bought a fairly inexpensive spindle off eBay. As far as I know, they are kind of new on the scene. I've seen them before, but not common and not on eBay, though it could be that I just wasn't using the correct search string. At any rate, the spindle spins about 1K to 30K rpm as per the specs and the runout is very small (less than .0005"). It is very quiet as well - MUCH quieter than a router motor and even quieter than a Dremel by probably 3 or 4 times. You just hear a whoosh and little hum. It's pretty torquey too even at low RPM. It takes an ER collet like the one I built, but it's the next size larger (ER11 rather than ER8) and will accept up to 5/16" diameter shanks if I ever have a need for it. I won't on this machine, but that's the capacity anyway.

I wired a relay in to switch it on and off from Mach3 and plan to eventually have Mach control the RPM as well. It's pretty nice just to be able to let Mach turn it on and off - seems more professional or something. For now a simple 5K potentiometer controls the RPM. Another nice thing is that it comes up to speed in probably a quarter of a second, so no delay/wait necessary in the programming.

I did a little testing then ran the same board I did before. The results are dramatically better. I haven't figured out how to take a good picture of a PC board yet, but following is a picture of the spindle and the results of the routing. Hard to see (can't see it?) but the result is very, very clean and crisp. It's just tons better than before and I'm happy the long-awaited good performance is finally here. Looking forward to being able to actually do some good work on it.


Yesterday's new routing on top. Old routing (from before) on bottom.
Same exact code, cutter and depth as before. The old routing cut so much wider because of the runout. That was with my home-made spindle too, meaning a Dremel performs even worse.

That new little spindle is a nice setup for a reasonable price and I highly recommend it if you have a similar project. Search "300 watt spindle" under Business and Industrial on eBay and you'll find them there (with various options, i.e. with mounting bracket, with PWM speed control, with power supply, etc.).

Or here's a source in the US who sells them for a little higher price for the same thing: link (http://www.automationtechnologiesinc.com/products-page/cnc-spindle/300w-1hp-cnc-air-spindle-w-er11-chuck-kl-300a). This source also carries a good selection of other pretty nice stuff for decent prices. Interesting source. Their home page (http://www.automationtechnologiesinc.com/)

10-14-2012, 08:03 PM
Looking pretty good. Here are examples of PCB isolation routing on my mill:



tyrone shewlaces
10-14-2012, 08:22 PM
Very nice work. I'm happy that my results are approaching the quality of others doing successful isolation milling such as yours. Under magnification, mine actually looks fairly close to what you're getting there. The material substrate is different (more cloth content I think) but the surfaces and edges are pretty clean now.

Probably ought to start trying to figure out how to do some decent macro photography so I can prove it (or not). Not sure if it's possible with my modest Power Shot.

10-14-2012, 09:28 PM
Hold the camera up to the eyepiece as close as possible. Use some telephoto and you can adjust the vignetting. A simple holder helps a lot. It's called "afocal coupling" and it works fine. The above images were taken that way with my old Nikon 4300 on my stereo microscope.

Tony Ennis
10-15-2012, 08:03 AM
Not sure if it's possible with my modest Power Shot.

It can. There's a mode for it. We have one that's probably 7 years old now (an old Elf) and it does a lovely job.

10-15-2012, 09:54 AM
Not to hijack this thread, but Evan: May I ask what type/size cutter you are using and at what feed speed? (And how many you broke before you figured out the speed? :) ).

I've been using a 1/6" point end mill and trying to set my width of cut by how far I plunge the point. It's hit or miss, but it works.