Desk CNC 3020 (or similar) accuracy and practicality for SMD PCB prototyping? - Page 1
Forum section: electronics / general

author: python50
author_rank: Newbie
timestamp: January 16, 2014, 12:13:17 am
content: Hello, I am considering getting a cheap desktop CNC mill for PCB prototyping. Specifically a cheap ChineseCNC 3020which seems to come with everything needed to mill. I have etched many boards and I have gotten them professionally made before, but I have never milled a PCBs. I always have enjoyed being able to mill out designs but I don't know what the limitations would be for milled PCBs.What does it take/is if feasible to mill fine SMD footprints like a 0.5mm pitch TQFP100 on a CNC mill?I notice the machine I am looking at has a max spindle speed of 8000RPM, would higher speeds be of much utility for PCBs?Is a different avenue for prototyping recommend instead? To me it seems that it a mill could pay for itself in a few large prototypes given its accuracy is not an issue.Do these Chinese machines work reliably over the long run or will I constantly have to tweak the mechanicals to make it preform satisfactorily?Thanks,Jason White

author: Frost
author_rank: Regular Contributor
timestamp: January 16, 2014, 01:30:18 am
content: Quote from: python50 on January 16, 2014, 12:13:17 amTo mill SMD footprints with an extreamly small pitch, you need very high RPMsto use a very small, we call it "Stichel", it's a mill cutter primary for engravingwith only one sharp 15 degree V-shaped tooth.For this small cutters you normaly use a inverter driven high speed spindlewith up to 25000RPM and more.Quote from: python50 on January 16, 2014, 12:13:17 amDefinitely yes!The smaller the drill diameter the higher the needed RPM,same for the trace spacing with the Stichel.Quote from: python50 on January 16, 2014, 12:13:17 amI never ever saw a chinese (except taiwanese) tool or machine, within the machine buildingsegment, that worked satisfactorily ex works without the need of massive tweaking and reworkFor PCBs with "normal parts" this mill could work for hobby purposes,but for SMD parts with small footprints like TQFP100, I am not sure.

author: python50
author_rank: Newbie
timestamp: January 17, 2014, 03:34:02 pm
content: QuoteIs the spindle RPM the primary limitation with machines or would more precise stepper motors and etc. likely be needed as well?QuoteWould it be possible to simply run the machine at a greatly reduced federate to compensate for low spindle speed? Or might that have some undesired consequences?QuoteIn your opinion would a SO (50mil pitch) package be feasible, or is that getting into the painful territory for milling?

author: orangecat
author_rank: Newbie
timestamp: June 01, 2014, 03:36:49 am
content: There's no problem milling the smallest SMD footprints. Here's a video milling a TQFN-48 (0.5mm between pin centres). Using a generic chinese CNC3040:

author: jeremy
author_rank: Super Contributor
timestamp: June 01, 2014, 04:21:25 am
content: Well done, that looks amazing!

author: ecat
author_rank: Frequent Contributor
timestamp: June 01, 2014, 05:37:50 am
content: Impressive.But. It is hard to know if anomalies are by design or due or errors. Looking at the introductory still image the stepping on the central horizontal channel may be backlash in the Z axis and the variation in the shape of the IC pads backlash in the X and/or Y axis.In common with the vast majority of CnC videos showing the final result is mostly pointless, what we need to see are a selection of squares and circles cut and then measured to better than 0.1mm.Two other points before the OP spends their cash: The machine in the video uses the 24,000 RPM water cooled spindle and these machines are available in both trapezoidal screw and ball screw configurations.High rpm is good for PCBs, the other consideration wrt spindles is run-out, the eccentricity of the tool when rotating.Ball screws are more expensive than trapezoidal but they should be more accurate along their full length, present lower backlash and maintain the lower backlash for longer. You can tweak trapezoidal setups to provide good results, then tweak them again after a couple of hours, rinse and repeat.

author: Fred27
author_rank: Unknown
timestamp: June 01, 2014, 08:08:11 am
content: I used to mill PCBs on my converted Proxxon MF70, but have switched to photo etching. Whilst I got reasonable results, I found that the the depth of cut meant that applying dry film solder mask was harder.If the router is anything like the Chinese laser cutters (and i've read that it is) then it probably won't be smooth sailing out of the box.Whilst these are both negatives, I would still say "go for it". It will be ideal for drilling and routing out etched boards. I'm sure you'll enjoy trying out PCB milling even if you don't completely switch to it. If you don't mind tinkering with the machine to get it running well, then they're great value. Consider it as a kit of parts rather than a polished commercial product. I perhaps wouldn't recommend one to the average guy on the street, but if you're on this forum then it could suit you.CNC machining is another fun new hobby. You're just as likely to use it to make quadcopter frames, front panels or project enclosures as you are to make PCBs.

author: orangecat
author_rank: Newbie
timestamp: June 01, 2014, 08:23:13 am
content: Machine uses ball screws on all 3 axis (I wouldn't bother using a machine with t-screws on any axis if TSSOP, 0.625mm or 0.5mm pin pitch, is required). The 800 watt water-cooled spindle is also a good choice, air cooled spindles tend to much noisier and they may have more runout. Any significant runout will break the endmills or ruin the board or both.There might be some backlash in Z, or it might just be the board slightly changing vertical position as the stresses in the board are altered as copper is removed, or as the tape holding the PCB down or simply due to temperature variation from start to finish. It's very small, something like 0.02mm -- not even important for cutting boards.The board looks almost exactly like the simulation:

author: jaxbird
author_rank: Frequent Contributor
timestamp: June 01, 2014, 05:34:07 pm
content: Quote from: orangecat on June 01, 2014, 08:23:13 amNice workBut you don't need ball screw to do 0.5mm pitch. I have a small cnc with acme screw and anti backlash spring nuts, no problems doing 8-10 mill traces. (got some pics under the PCB manufacturing main subject)I think most important is having a spindle with minimum runout and some sharp bits.I don't go as deep as your pictures show, just enough to remove the copper.

author: python50
author_rank: Newbie
timestamp: August 27, 2014, 10:40:26 am
content: Thanks everyone for your input. Especially after seeing that video on vimo, I think I'm going to get a CNC 3020 and try it out.

author: mazurov
author_rank: Frequent Contributor
timestamp: August 28, 2014, 06:21:22 am
content: The picture shows SO and 0603 milled on this machine ->http://microcarve.com/(MDF frame, Delrin nuts, 2 start turned ACME screws) with Bosch Colt spindle and 60 deg bit fromhttp://www.precisebits.com/. The gear is pretty basic but the machine needs to be squared and have very little backlash (freshly cut Delrin nut works very well for about a year ). Out of the box, any mill would require squaring, so choose the design which allows for that. If you have never squared a mill you may want to pick a model which is popular. Ball screws will help with backlash but not squaring.I can mill 0.65 mm on 1oz and 0.5 mm on 0.5 oz; however, results are less consistent and boards are harder to stuff.

author: maliqua
author_rank: Contributor
timestamp: September 23, 2014, 05:34:24 pm
content: I did something similar to what you have in mind I've been using a desktop cnc from mydiycnc.com with the laser cutter for traces and rotary tool for holesi found it very difficult (technically i haven't succeeded) using the rotary tool for an entire pcb.** i should note that i still get better results with the toner transfer method then etching in FeCl

author: eurofox
author_rank: Unknown
timestamp: September 23, 2014, 06:16:37 pm
content: I just wonder what kind of software you use, I know the generic Mac3 but the output from PCB software is not compatible with Mac3, is there other dedicated sofware available or tools to convert it?

author: mazurov
author_rank: Frequent Contributor
timestamp: September 23, 2014, 07:45:21 pm
content: I use pcb-gcode ulp for Eagle. It outputs GCode usable on many different platforms, including Mach3.

author: mikeselectricstuff
author_rank: Super Contributor
timestamp: September 23, 2014, 09:31:08 pm
content: Machines like this can be OK for very small boards, but maintaining an accurate cut depth over a larger, possibly slightly warped board is likely to be impractical. You really need something that can sense and adapt to surface height

author: Precipice
author_rank: Frequent Contributor
timestamp: September 23, 2014, 09:38:46 pm
content: Quote from: mikeselectricstuff on September 23, 2014, 09:31:08 pmDoes such a thing exist? I know it's a pain trying to keep plasma cutters hovering at the right height.Can you scan, remember and cut, hoping nothing's shifted in the meantime?(I'm trying to think of a scheme for measuring depth. Maybe spotting capacitance change as you repeatedly lift and lower the tool into the copper? Something optical, watching the width of cut? This seems hard, but I've probably missed something obvious...)

author: mikeselectricstuff
author_rank: Super Contributor
timestamp: September 23, 2014, 09:48:13 pm
content: measure-then-cut would probably work. Capacitance may work quite well, as you're sensing a flat metal plate at close proximity.

author: G0HZU
author_rank: Super Contributor
timestamp: September 23, 2014, 09:52:23 pm
content: My T-Tech 7000 machine auto adjusts for surface height by using a simple sensing foot. This allows it to achieve good results up to a max PCB area of 13 inches by 19 inches.It usually works well although it can cause problems if the foot falls into a wide area that has already been milled. But usually this is avoidable.The foot technology has evolved a bit since my machine was made though...http://t-techtools.com/store/index.php?main_page=product_info&cPath=14_19&products_id=288

author: G0HZU
author_rank: Super Contributor
timestamp: September 23, 2014, 10:10:39 pm
content: In case anyone wonders how the sense foot works, the spindle assy has a foot or 'heel' that the whole assy rides on and a fine rotary vernier control sets the tracking height of the tool tip vs the foot. So even if the board is warped the foot will press it flat and the tool will faithfully track against the foot and keep a constant cutting depth.If the cut depth isn't quite right, it's easy to just give the vernier a fraction of a turn to increase or decrease the cutting depth by a fraction of a thou of an inch as it mills the board.

author: G0HZU
author_rank: Super Contributor
timestamp: September 23, 2014, 10:14:51 pm
content: QuoteThere's always the 'dambusters' method I suppose () but the sensing foot method has been around for decades and it is reasonably effective...

author: mazurov
author_rank: Frequent Contributor
timestamp: September 23, 2014, 11:22:24 pm
content: Quote from: Precipice on September 23, 2014, 09:38:46 pmThere is an add-on to pcbgcode called autoleveler; it's a script which probes the surface of a PCB, stepping and probing every 5mm in each direction, and then uses the data to adjust Z during milling. Standard tool height probe input is used, you need it to clip one wire to the (stopped) spindle with cutter installed, another wire to the foil, run the script, remove wires when it's done probing, mill. I never used it myself but saw ppl raving about it on the forums.

author: G0HZU
author_rank: Super Contributor
timestamp: September 24, 2014, 01:08:05 am
content: Can they not adopt the foot method? I've not really looked at the mechanics of mine for many years but the foot pressure is set by an adjustable solenoid. It is done like this to preserve tool life. The ideal scenario is for the foot to only just lift off the PCB when it has finished a cut. So it has minimal vertical travel before hitting the PCB again on the next cut. It took me a while to set up the best foot pressure on my machine. The foot isn't used during drilling or routing.It can't be that complicated to replicate. I think some newer systems use a horseshoe shaped foot. Mine is the older generation and is round like the ball of your foot.

author: mazurov
author_rank: Frequent Contributor
timestamp: September 24, 2014, 01:22:48 am
content: Quote from: G0HZU on September 24, 2014, 01:08:05 amWhy? The height probe is much easier to make and you typically want one anyway to set zero Z.

author: Richard Crowley
author_rank: Super Contributor
timestamp: September 24, 2014, 01:57:25 am
content: Would it be practical to use a vacuum hold-down for the PC board material? That method is used successfully for much larger pieces, so it seems like it would work with most any size PC board.

author: mazurov
author_rank: Frequent Contributor
timestamp: September 24, 2014, 02:25:05 am
content: Quote from: Richard Crowley on September 24, 2014, 01:57:25 amDepending on what is considered practical. If you have it already, then yes. If you don't, you can either buy one (expensive) or make one (depends on how good you are with mechanical design, I'm not). On the other hand, carpet tape is not that expensive and works just fine for one-offs.I have a project in the future when I'll need to mill a bunch of the same boards ( 5mm 65mA SMT LEDs run cold being mounted on a PCB with almost all copper left in place on the both sides. I'm making a grow light out of them. See attached ). Since I need about 50 of them I'll attempt to make a vacuum table, good just for this board.

author: jeremy
author_rank: Super Contributor
timestamp: September 24, 2014, 07:29:22 am
content: Quote from: mikeselectricstuff on September 23, 2014, 09:31:08 pmSome high-accuracy, PCB-only machines I have seen use a combination of vacuum hold down, and a "stiff skirt" around the spindle (made of delrin/HDPE?) on a strong spring to push the board flat around the cutting area as the spindle plunges. I'm sure there is a proper name for it, but I don't know what it is

author: G0HZU
author_rank: Super Contributor
timestamp: September 24, 2014, 01:31:04 pm
content: Quote from: mazurov on September 24, 2014, 01:22:48 amWhat if you want to mill a really thin and bendy PCB material? eg 0.020" or 0.010" or even 0.004" thick like paper (including the 2 copper layers?)This is where the foot method really performs well. Sometimes you have to set the pressure carefully. eg for cheesy/bendy stuff like PTFE because the foot can compress the material if the pressure is too high.

author: mikeselectricstuff
author_rank: Super Contributor
timestamp: September 24, 2014, 01:55:42 pm
content: Quote from: G0HZU on September 24, 2014, 01:31:04 pmstick it down to a more rigid backing board. or use vacuum hold-down

author: G0HZU
author_rank: Super Contributor
timestamp: September 24, 2014, 02:34:39 pm
content: I'm not sure I'd want to use glue for a double sided board but I guess it's an option. It does rely on the table + backing material being very flat though.I've not used a machine with the vacuum hold down feature so I don't know how effective it is. Presumably it requires some air permeable backing material below the PCB material to allow it all to work?I can see the advantage of the vacuum with respect to preventing bowing up of the board material. It can be a real pain keeping the material flat because the ride height of the tool when lifted has to be higher than the PCB bowing in order to prevent fouling. This is one limitation of my old T-Tech machine.But I have milled double sided flexi PCBs where the PCB laminate is only about 0.0025" thick with it.

author: mazurov
author_rank: Frequent Contributor
timestamp: September 24, 2014, 05:25:25 pm
content: Quote from: G0HZU on September 24, 2014, 02:34:39 pmThere are adhesives that can be released by gentle heating ( ~160F, that's below boiling for water asl ). To make a mounting surface flat you mill it flat prior to mounting the first board to it. That's the beauty of general purpose CNC mills, they can be used for all kind of things, like making jigs for PCB milling (including vacuum tables). They won't work as well as specialized PCB-only mills but they are often good enough - I can mill 10 mil clearance consistently and when I want smaller clearance I also want a soldermask and PTH so I just order the board.

author: jeremy
author_rank: Super Contributor
timestamp: September 24, 2014, 05:35:11 pm
content: The vacuum systems are quite simple really, just a grid of holes in a flat piece of material hooked up to a vacuum on the underside. You just tape over the holes you aren't using, or I guess you could use a silicone sheet or something?

author: Richard Crowley
author_rank: Super Contributor
timestamp: September 24, 2014, 05:51:40 pm
content: Quote from: jeremy on September 24, 2014, 05:35:11 pmIndeed, constructing a vacuum hold-down table is very nearly trivial. The CNC machine itself can be used to create the surface.Here is a video of a PDJ PilotPro creating its own vacuum table.http://youtu.be/172rLt0oxogI am finishing a 26x26 inch version of this machine and I will likely make myself a vacuum table for it.And you can use something as cheap/simple/prosaic as a domestic vacuum cleaner (BrEnglish: "Hoover") to provide the vacuum.And you can cover the unused surface with scraps of plastic or even plain paper.

author: mazurov
author_rank: Frequent Contributor
timestamp: September 24, 2014, 06:23:16 pm
content: Quote from: jeremy on September 24, 2014, 05:35:11 pmThe difficulty is the setup. You mount a vacuum table (or any other jig for this matter) on the machine and start wondering if its surface is orthogonal to the spindle. The fastest way to make sure is to mill the top surface flat; however, since vacuum table is expensive and your machine may not necessarily be good enough to mill aluminum you spend time with indicator in the spindle measuring and shimming.Another way is to clamp a 1" thick piece of HDPE and make the vacuum table out of it. Everything can be machined except the horizontal hole which you would drill, tap and screw in the vacuum port. I've never done this myself but I heard that drilling/milling into the vacuum holes ( or grooves ) is not a good idea - weaker vacuum, abrasive swarf going into the pump, etc., so you spend time designing your table for the board you're making.Both methods will pay off if you're milling a batch since changing stock is very fast. However, when I mill a one-off I can do it many times faster with carpet tape. But again, I'm no machinist. I'm not a good enough circuit designer either so I have to build my circuits to make sure they work otherwise I wouldn't bother.

author: G0HZU
author_rank: Super Contributor
timestamp: September 24, 2014, 07:01:51 pm
content: Does the vacuum table add any significant noise to the overall system noise?My old T-Tech system is very noisy already as it uses an old school Nilfisk GM80 feeding to a basic nozzle at the tool area. I run with the GM80 pushed through a window to try to minimise recirculated dust particles and also to keep the noise down a bit. But the newer LPKF machines seem much quieter so I wonder if the vacuum table noise is noticeable on the newer systems.I'm probably 10 years out of date on milling technology. My T-Tech machines are both from the 1990s and the LPKF machine we have at work must be at least 10 years old.

author: Things
author_rank: Regular Contributor
timestamp: September 24, 2014, 11:13:13 pm
content: I've just used doublesided tape in the past - probably not practical if you're making a bunch of them, but for occasional hobby work it works fine.You'll want to fit a panel of wood or plastic over the actual metal bed to act as a work surface - basically set up a program and get the mill to face off the work surface, then you know it's completely flat. It'll also save you if you stuff up the programming and try drive the tool bit into the metal bed!

author: ozwolf
author_rank: Regular Contributor
timestamp: September 24, 2014, 11:48:47 pm
content: Quote from: Richard Crowley on September 24, 2014, 05:51:40 pmJust a consideration with the domestic type vacuum... Allow some bypass air as this is also the cooling air for the fan motor. If you cover all of the holes, the motor will soon overheat and shutdown/burnout.

author: ivaylo
author_rank: Frequent Contributor
timestamp: September 25, 2014, 08:32:01 am
content: And what's with the parallel interface of all of these brand new machines? The last computer I had with such a thing was like 20 years ago. Yes, I know, get an adapter, DYI USB, etc, etc, but there must be a reason for selling brand new PC controlled hardware with an outdated interface. Thanks for enlightening me...

author: mikeselectricstuff
author_rank: Super Contributor
timestamp: September 25, 2014, 08:40:13 am
content: Quote from: ivaylo on September 25, 2014, 08:32:01 amBecause the Chinese are no good at designing anything - they just run old designs for as long as they can get away with it.Even if they did design a USB based one it would probably suck ass.Unfortunately there is no accepted standard in the CNC world for a USB interface, and Mach3, with its crude bit-bashing, works well enough most of the time, so the Chinese are happy to ship cracked versions with their kit.Doing motion control over USB is a somewhat nontrivial, but perfectly solvable problem, and for reasons I don't quite understand, nobody yet seems to have done a really decent job of an open source motion controller.Seems to me that Mach3 is the Eagle (PCB) of the CNC world - they got in early with a free version that was OK for a lot of people, and became a de-facto standard because it was free and there wasn't anything better at the time.

author: ivaylo
author_rank: Frequent Contributor
timestamp: September 25, 2014, 08:45:56 am
content: Thanks, Mike...

author: Richard Crowley
author_rank: Super Contributor
timestamp: September 25, 2014, 10:55:31 am
content: Quote from: mikeselectricstuff on September 25, 2014, 08:40:13 amAren't there Arduino (or clone)-based controllers that take G-Code on a SD card and drive the motors as a stand-alone unit? (i.e. Rep-Rap) Presumably open-source.They are now promotoing USB-to-parallel external adapters to keep the old design running on modern computers.QuoteRumor is that Newfangled Solutions is developing a completely new generation ("Mach4"?) and will raise the price an order of magnitude and drop Mach3 (US$175) Will an alternative/replacement emerge that will take up the market it for hobby-level users? Mach3 seems remarkably fiddly and amateurish. I can't see how they have managed to sell it for THIS long.

author: Things
author_rank: Regular Contributor
timestamp: September 25, 2014, 11:04:51 am
content: I've heard most USB->parallel interfaces don't provide all the signals required to drive CNC machines, just things like printers. Just something to watch out for.They could probably make a USB interface OK - but don't even think about the software!

author: bookaboo
author_rank: Frequent Contributor
timestamp: September 25, 2014, 11:11:15 am
content: +1 to what Mike said, previously I've used LPKF and T-Tech milling machines and sometimes they work beautifully so you are can go from concept to PCB in a single day. However they often needed a lot of attention to get the right results, particularly on larger boards. Even the slightest warp in your FR4 can destroy your results and leave you with multiple efforts. Broken mill bits are another pain, you sit listening to the machine drone (plus vacuum and air compressor) for hours while you do other things only to realise the mill bit broke 10% of the way in. Bear in mind these were EU and USA built specifically for PCB work.Perhaps things have improved in the 5-6 years since I gave up on milling PCBs but personally I think you are much better off just paying for one of the fast turnaround fabrication services. When you consider the cost of your own time, the machine costs, material and of course bits it probably works out cheaper to get them done externally. You also get the added benefit of soldermask and silkscreen. Unless you are in the situation where you constantly need to be turning around designs on 2-3 day lead times I don't really see the benefit of this method any more.

author: dr.diesel
author_rank: Super Contributor
timestamp: September 25, 2014, 11:15:28 am
content: Speaking of, whatever happened to that nylon cube, Kickstarter mill thing that made a few headlines a year or so ago? I know it was small, had some hype, surprised nobody here ended up with one to show us?

author: sacherjj
author_rank: Frequent Contributor
timestamp: September 25, 2014, 12:18:18 pm
content: I'm using a Probotix Fireball X90 setup for all kinds of general CNC prototyping with machining plastics and also PCB prototyping. Luckily most of the quick prototypes are small enough in area that I mount as flat as I can and set height in the center.I've really been happy with the quality of bits and service fromThink and Tinker precise bits.If I had the input capability for a touch probe for PCB CNC, I would do it immediately. However, it means replacing the stock controller board that came with the Probotix kit. It isn't causing enough pain right now to cause me to drop a couple hundred on changing the setup.For setting Z height, I use a 0.250 brass rod. Lower the cutting tip with a very slow Z jog. Then I raise it until the bar just passes under the cutter. Then I set Z at 0.250. This gives very accurate and fast setup.Now as far as vacuum hold down, I see two problems:1 - Some PCB material is bowed enough that vacuum might not pull it flush.2 - Drilling, Routing of larger holes, and edge cut out will all erode the surface such that hold down force is no longer present.I am using CopperCAM to convert Gerbers and drills to G-code. For the most part, I've been happy with it for non-slotted designs. I've started using multiple holes to emulate slots where they are needed. This is a little annoying, as I can't use the exact same file for real fab. I make multiple pads over the existing slots and just ignore the slotted NCDrill file for CNC milling.CopperCAM allows you to add drill locations for layer alignment. If these are positioned so that board flit remains aligned, then you are set. I use a T-slot table and have some threaded rod that goes into them. I then turned down the 5/16" rod from the T-nut to a smaller diameter on the lathe and threaded (to 8-32 I think). If I position my holes to line up with my T-slots, then I can pull the board down to a flat reference with small washer and hex nuts into this threaded rod. By turning the rod through to T-nut to the base first, the position is fixed. While CopperCAM allow up to 4 layers, I've had no problem indexing dual layer boards.My next upgrade is to not use just scraps from the same board underneath, but machine a few slightly varying heights of plastic to tune the board flatness. I'm looking for some flat head 5/16" nylon bolts to make counter sunk mounted sacrificial board that I then machine flat. This with a common reference pattern on it to screw the PCB to might be the best solution. But I've been to busy to tweak the setup lately.Here is a picture of my setup (pardon the dust, I was milling a gift plaque for my wife out of Oak):I included the good old DS1052 for size reference.The guys at Think and Tinker are very knowledgeable on runout of common routers. We have their precision collets for 0.125 and 0.250 bits. This is required to machine with very small bits. I did some prototypes of clips in spring steel using a 0.010" bit from them. I had to manually drip fluid at the bit, but it worked great. I used a router speed controller to get the speed down. This has been replaced with aSuper PIDclosed feedback speed control that lets me run a router down to 5k RPM without issues. This lets me machine plastic with a 0.25" bit with no melting issues.

author: sacherjj
author_rank: Frequent Contributor
timestamp: September 25, 2014, 12:43:05 pm
content: Quote from: bookaboo on September 25, 2014, 11:11:15 amI think this is true with almost any non-trivial design. I've got to prototype some fairly simple power PCBs with 2 and 3 ounce copper. We started looking at the prototyping costs for some boards that were just glorified wiring and it makes sense. The whole board might take 20 minutes to cut, so I can baby sit.What I've found really useful is cutting out boards that have no traces on them. We are brainstorming a few ways to solve some interface and case design issues and 3D isn't as good as holding them. So I've been routing out the edge and mounting holes for jacks. Then I solder jacks directly to the copper clad. It is a real quick way to give our boss a real world feel for a board in the case prototype and physically plugging and unplugging cables.Another great use for this thing is cutting the opening for one off or short run projects in hobby boxes. I've even taken to engraving what would otherwise be a stuck on P-Touch label or something. It gives results that look really sharp. 4 holes around the clean opening for the LCD. Then machine a plexiglass cover to go over it and bolt in place. It really looks like a production piece.

author: mikeselectricstuff
author_rank: Super Contributor
timestamp: September 25, 2014, 01:15:50 pm
content: Quote from: Richard Crowley on September 25, 2014, 10:55:31 amThey really missed the boat on this - in the parallel port era they owned the market, if they'd done a reasonably priced USB to parallel interface to run all the existing parallel port devices (which could also have been a dongle for their SW) they could have totally cleaned up. There is other stuff out there now so their monopoly is gone.I bought a smoothieboard a while ago but not tried it yet.What I think is still missing is a standalone G-code to motion controller with sufficient inbuilt UI to do the stuff like zeroing and feed rate control - that's the only thing I ever do with Mach3's UI.Maybe something that interfaced directly with these cheap handheld MPGshttp://www.ebay.co.uk/itm/CNC-3-Axis-4-axis-USB-HandWheel-MPG-pendant-for-Mach3-engraving-Router-Mill-/111464851845?pt=UK_BOI_Industrial_Automation_Control_ET&hash=item19f3d2a985

author: G0HZU
author_rank: Super Contributor
timestamp: September 25, 2014, 01:56:56 pm
content: QuoteAll valid points and i think for general purpose FR4 boards (especially digital circuits with lots of PCB traces) it is false economy to use one of these machines today.But I use mine for RF research/design using various exotic PCB materials and the boards are often very simple. The key to success is to be milling small and simple boards on non standard dielectric on a regular basis and also to use it for other purposes like front panel design and making laminated tools etc. Also, there's no substitute for experience and this helps enormously because there are so many things that can go wrong during the whole process that can destroy a board. I've learned a lot in the time I've been using these machines and it's very rare that I get a dud board and I don't have many tool failures.I'm amazed that modern machines use parallel interfaces. T-Tech moved over to RS-232 about 20 yrs ago. I know an ex colleague who has one of the early T-Tech machines with a parallel interface and it is controlled via an ISA card that has to be fitted in a contemporary PC running MS-DOS. eg a slow 286 or 386 or the system will be erratic in operation otherwise.Mine are both controlled via RS-232 and I have a dedicated (old) Win98SE laptop that runs the Isopro software really reliably.

author: mc
author_rank: Regular Contributor
timestamp: September 27, 2014, 11:29:41 pm
content: The main reason people still use parallel ports for CNC machines is they're cheap, and for your typical home CNC they are more than adequate. However parallel ports are becoming rarer.Any half decent commercial machine will use a dedicated motion controller, and if PC driven, usually either via USB or Ethernet. Serial has pretty much died out, as it simply doesn't have the bandwidth to handle complex countouring, especially at modern machine speeds.I actually find the history of Mach pretty interesting, and think that Art Fenerty, the man behind Master/Mach, is a genius. He achieved something that many said couldn't be achieved on a windows operating system, which was a highly accurate pulse generator. And as far as anybody knows, it's something that has never been repeated. I know Art has said that the driver is essentially a virus that latches onto the windows kernal and hijacks processor time, which is why it will never likely work on 64bit systems, as 64bit kernals are encrypted to improve security and the encryption gets changed with most updates.Art developed Mach to the point of adding plug-in support, so it would work with external motion controllers, however Mach3 was originally designed to only use the PP, so Mach3 has been plaqued with many bugs due to interdependability issues since, which have only become more apparent as external motion controller/plug-in developers keep pushing the limits.At some point Art sold the company to Brian Barker, who spent a few years ironing out bugs, before finally biting the bullet and starting a complete re-write, which has only over the past few months been released for testing.Mach 4 is essentially just a framework, with various plugins to provide the GUI, trajectory planner, and IO. It also removes alot of the limitations that Mach3 imposed, such as limited IO numbers, and the 10Hz update rate for plug-ins/macros. Feedback so far has been good, however there is increased competition, but personally I think Mach will still be very popular, as it's far more adaptable than the other options without requiring a great deal of programming knowledge.The parallel port plugin for Mach 4, Art wrote under the working name of Darwin, as he feels it wil be the last evolution of the printer port for motion control purposes, as external motion controllers are getting cheapers and more common place (I've personally got 3 machines that all use external motion controllers).Art also wrote a test version of Mach with a high order trajectory planner to provide an S-curve motion profile, under the name Quantum. I read a post about what's involved in a high order planner, and my head hurt reading the description, let alone the amount of coding and thought that would need to go into writing one!One of Art's great attributes is he is willing to share his knowledge about such things, and explain it in a way in which most people will understand.Art's latest project is Gearotic Motion. I had a quick play with it when it was still pretty new, and it just blew me away with what it was capable of designing. For anybody interested in gears, especially more bizarre yet functional ones, check out the Users Pics, and Your Videos boards over on the forum -http://gearotic.com/ESW/FavIcons/For those who mentioned using a USB to parallel adapter, it won't work. Motion control relies on highly accurate pulsing, which standard USB to parallel adapters are just not capable off. The nearest thing you can get is CNCDrive's UC100, which looks just like a USB to parallel adapter, however is actually an external motion controller, shrunk to fit in a very small enclosure with only a single USB and single DB25 connector. It's essentially designed as an easy way to provide USB connectivity to a parallel port machine, without the need for rewiring/retrofitting.I've now retrofitted three CNC machines, with a fourth being planned, and have looked at most hobbyist level motion controllers and software. All have limitations, however Mach remains my personal choice as it provides a standard interface which is relatively easy to customise. I have one machine running Denford's VRMilling5, purely because it had been upgraded to the USB controller which provides pretty good performance, however it's just not got the features or easy adaptability of Mach, which is where most other options suffer aswell.I know I fall into the more experienced CNC builder category, so I know what I want from the hardware and software.Whereas somebody new, mostly decides on price, and often ends up with less features, which is fine until you realise those features can come in very handy, or the junk you've bought is hopeless (TB6xx drives being the best example!).And finally, the issue of non-level boards, check outhttp://www.autoleveller.co.uk/I've not personally used it, however feedback seems good. Although it requires probing, you just need a single available input connected to a couple suitable bits of wire with crocodile clips. One clip on the board, one on your spindle/cutter, and you've got a suitable probe.

author: G0HZU
author_rank: Super Contributor
timestamp: September 28, 2014, 01:14:17 pm
content: QuoteTo clarify my current setup, both of my old T-Tech 7000S machies are arranged as PC >> RS-232 >> T-Tech Control Box >> big custom T-Tech parallel cable >> Milling tableThe milling table houses the various motors and the spindle motor and Z solenoid and all the power and control to it comes from the parallel interface from the external T-Tech control box.I don't think it is a slow machine but then I don't know what modern machines are capable of. The modern? machine in the autoleveller link looked really really slow and clunky compared to my oldschool T-Tech machine.I also had a look at a few youtube demos of the Mach 3 SW and I wouldn't want to be using that for PCB milling. It's a very versatile interface with lots of low level user control/config but it looks to be very limiting when it comes to PCB milling. I'm comparing it to my ancient copy of Isopro.Isopro isn't 'great' SW by any means but it does seem to be well tailored to PCB milling with my 7000S. I use LPKF SW to produce the isolation/rubout files and import these into isopro to do the milling. This is because the isolation/rubout algorithms built into Isopro are very crude compared to LPKF.

author: mc
author_rank: Regular Contributor
timestamp: September 28, 2014, 06:46:42 pm
content: G0HZU, I should maybe of been a bit clearer and mentioned modern machines.For 2D work, which is pretty much what PCB cutting is, then serial is more than capable, as the majority of commands will be relativelt large linear or arc moves created from a DXF or similar 2axis file in only 2 axis, with the 3rd axis only occasionally being moved to set depth.The limitation of serial comes when you start creating G-code (or whatever machine code your machine uses) from 3D stl or similar files, which result in lots of relativelt small moves often in all 3 axis.Also, when I say parallel, I mean something that actually uses the parallel IO standard. By the sounds of it, your machine is using parallel connectors simply for connecting power/signals. The RS232 is what is doing the actual communication, with the control box containing some form of motion controller that converts the serial signals to/from power/sensors.Most of the Mach3 videos you'll see, are machines that have been converted using steppers on a pretty tight budget, and for various reasons, aren't really capable of high speeds. Certainly your typical 3040/6040 machines will shake themselfs apart if pushed too hard/fast, whereas I'm guessing your machine is well designed and tuned for it's intended purpose. Most hobbiests will be quite happy with sub 1m/min speeds, whereas that's verging on a crawl for commercial machines. The last commercial vertical milling machine I looked at, was capable of 6.5m/min cut rate with over 16m/min rapids. (yes I'd love one, however i can't justify one just yet!)Quite simply, Mach3, and all other motion controllers/software, are only as good as the G-code it's fed and the machine it's controlling. Here's a vid showing move testing of a Chiron mill that has been retroffited with Mach3 and an external motion controller -It's also worth checking the tool change vids, as the unique feature of this mill is the super fast toolchange with the spindle still turning.

author: sigxcpu
author_rank: Regular Contributor
timestamp: September 28, 2014, 07:25:16 pm
content: For hobby use Eagle->pcb-gcode->Universal G-Code sender->GRBL->chinese controller (3040 in my case) is a very good path. I've done tests at 0.5mm pitch and they came pretty good.

author: mikeselectricstuff
author_rank: Super Contributor
timestamp: September 28, 2014, 07:38:18 pm
content: Looking for Chron Mill on YT brings up some serious CNC porn! I particularly like how trapdoors open, stuff comes out, does something then dispappears back behind the door.

author: G0HZU
author_rank: Super Contributor
timestamp: September 28, 2014, 07:54:51 pm
content: QuoteOk thanks for the extra info...Mine only has crude Z capability via a solenoid and some manual controls.QuoteThe worst thing on mine is the manual tool changing. I think the T-Tech engineers all went on vacation when finishing the design on mine and someone from WW2 designed the tool changing system on my machine. It is a basic manual toolchuck with a little hex lockscrew. Totally horrible and it is the worst thing about the whole machine. I look with envy at any machine with decent auto tool changing.T-Tech kept advising me to run it at >50"/min for some tools. I just checked the manual and the max milling speed is between 60"/min and 80"/min. However, I rarely run it at >24"/min. So I guess it is just above 'slow' by modern standards. It sounds wonderful and smooth and tight when running at 50"/min but my ignorance of its capabilities means I apply sympathy to the mechanics and run it much slower.sigxcpu's image at 0.5mm looks pretty good. What amazes me about my machine is that I can mill part of a board, switch it off and carry on again the next day after re initialising it and it will still mill in perfect alignment on the second day. When i look at the relatively crude mechanicals of it all I still can't fathom how it is able to do this so precisely...

author: mc
author_rank: Regular Contributor
timestamp: September 28, 2014, 08:42:15 pm
content: Mike, CNC is very much a case of, how big is your cheque book?If you want cutting edge, you need to check out the Japanese 5 axis machines.Here's a couple of Daishin Seiki's videos.This one shows how intricate they can do, but the machining speed is pretty slow due to it being titanium-This helmet video shows faster machining as they're starting with an aluminium billet, although the speed has to slow down for the smaller tools -I've actually got a 3040 machine, and I was pleasantly surprised by how accurate the basic machine is. The biggest two issues I found with it, are the thrust bearings used to support and control the ballscrew endfloat are utter rubbish, and the motor to ball screw couplers are a pretty rubbish design (they're prone to failure, aswell as being a bit springy under load).I replaced the thrust bearings, which are just standard radial ball bearings with good quality ones, and it made a major improvement to the machine. I've done nothing about replacing the couplers, as I'm only using mine as a CMM/probing machine, so load is minimal, plus I fitted glass scales to make it closed loop so any play in the couplers/ballscrew doesn't affect the probe trigger point.

author: mikeselectricstuff
author_rank: Super Contributor
timestamp: September 28, 2014, 09:07:03 pm
content: Quote from: mc on September 28, 2014, 08:42:15 pmImprovement in what way? An issue I have is vibration/tool judder when cutting acrylic. Are these mods likely to improve this?

author: mc
author_rank: Regular Contributor
timestamp: September 28, 2014, 09:52:22 pm
content: Quote from: mikeselectricstuff on September 28, 2014, 09:07:03 pmI noticed the thrust bearing issue the most due to very noticeable roughness when jogging. I initially thought it was perhaps a bit swarf in the ballnut, however when I stripped things down, the ballscrews were smooth to turn. It was when I reassembled things and tried adjusting the ballscrew endfloat, the roughness reappeared.When I stripped the shields of the bearings, they only had 6 balls and lots of play.Roughness may contribute to vibration/tool judder, however it could just be an issue with general machine rigidity. I've never personally cut plastic on a mill or router, but I do know it can be a major pain to get a good cut. You need to ensure you're taking a reasonable cut and not rubbing the work, and also you need to make sure you have no heat build up. There are cutters optimised for plastics, which generally have far sharper edges, and are available in specialist materials to improve cutter life.

author: Fred27
author_rank: Unknown
timestamp: September 29, 2014, 09:17:44 am
content: I have no problem cutting acrylic as long as it's cast and not extruded. Extruded melts too easily (and it stinks when lasered too). My mill is a much smaller Proxxon MF70, although I'm thinking about a 3040 for a larger cutting area.

author: johansen
author_rank: Super Contributor
timestamp: September 30, 2014, 06:42:09 am
content: Quote from: mc on September 28, 2014, 09:52:22 pmI thought 608 bearings had 7 balls, are yours even smaller?If you want to throw money at it, VXB has 708A bearings and they are the same size as the 608 bearings which are in most small milling machines.at 13$ each though its a bit insane, for that price i would rather build a new bearing block and use 10mm or 15mm bore DG bearings (which max out at about 15 degree contact angle)it is pretty easy to brinell 608 bearings when preloading them but often times its contaminates in the bearings, not a failed race that is causing the problems.yeah its a lot of work but you can pry off the seal, wash the bearing out and regrease it and put the seal back on it.but at 79 cents each its not worth the effort.--you do have preloaded bearings, right?

author: mc
author_rank: Regular Contributor
timestamp: October 02, 2014, 09:44:08 am
content: Quote from: johansen on September 30, 2014, 06:42:09 amOf course. This is one of china's finest engineered machinesThe bearings were complete rubbish. 6 balls with noticeble play/roughness turning them by hand. I thought I maybe still had them, and was going to take some pictures, but I must of thrown them out.I'm not sure how many balls are in a good quality bearing, but it's certainly more than 6.I did look at various options, but fitting some good quality standard 608's was the quickest option. If I had been aiming to eliminate play, then I would of modified things and used some proper thrust bearings. Either needle roller or AC with a custom housing, as the ballscrews aren't long enough to fit a proper bearing block.

author: johansen
author_rank: Super Contributor
timestamp: October 04, 2014, 04:45:44 am
content: The 608 bearings i bought for 79 cents each have 7x 5/32" ball bearings in them (yep, its 3.969 mm)the 708A bearings have 10 or 11 balls in them, and combined with the 30 degree contact angle means you can double the load, that said vxb lists the same load capacity as the 608 bearing which doesn't make any sense.you should be able to stretch the leadscrew by preloading it from both ends rather than the usual double bearings on the stepper end.alternatively you can use the bearings in the stepper to support the ballscrew

author: mc
author_rank: Regular Contributor
timestamp: October 04, 2014, 10:16:42 am
content: 708A's are not commonly availble in the UK.Preloading the full length of the ball screw is bad practice, especially on a machine where the material it's mounted to has a different expansion rate. One end should be fixed, using a suitable thrustbearing setup, and if long enough/turning fast enough the other end should be supported by a floating bearing.My 3040 has two 608s setup to provide the fixed end at the opposite end from the stepper, with a solitary bearing (IIRC it's bigger than a 608) to provide the floating support at the stepper motor end. The stepper is then connected via a flexible coupling.From what I've seen of my 3040, the engineering principles are actually pretty good, it's just the actual components used leave a lot to be desired.

author: johansen
author_rank: Super Contributor
timestamp: October 04, 2014, 10:01:46 pm
content: the bearings aren't strong enough, so you're right in that regard.but if the preloading is by a stiff wave washer, you'll be alright, and the frame can flex more than the expansion coefficient.

author: oakkar7
author_rank: Contributor
timestamp: October 05, 2014, 05:04:02 am
content: Quote from: orangecat on June 01, 2014, 08:23:13 amOrangecat,If so, the machine is an original 3040 without any modification. How about controller? Is this original one?

author: orangecat
author_rank: Newbie
timestamp: January 16, 2015, 05:15:20 am
content: The machine in the video:uses an unmodified machine (i've just cable tied the air blast and vacuum hoses on). I modified the control electronics to enable me to have coolant pump and air blast control via g-code since the controller i bought didn't have connections on the back for these. The parallel port of the control electronics was connected to a beaglebone black running LinuxCNC (headless).

author: RogerClark
author_rank: Contributor
timestamp: July 13, 2015, 10:07:55 am
content: I bought a CNC 3020 to do some other milling, mainly wood and plastic, but thought I'd try to give it a try for milling PCB, however the accuracy seems too low even to drill accurate holes for 40 pin DIL sockets for modules or microcontrollers e.g for an Arduino Nano socket.It appears that older machines suffered from missing steps, because of the lack of decoupling on some lines to the stepper drivers, and also under driving the optos which resulted in rather curved squarewave pulses.However all the mods for the two issues that people have found seem to relate to some older control board, and my machine has a JP-382A control board which is quite different from the previous model.I see some people have posted some tests on small boards with small IC's and fairly fat tracks, and I expect mine would be fine with that sort of thing, but the accuracy over larger distances seems too low if I use drill holes of 1mm.It could also be that I need to attach a scope to my driver board and look at the same signal lines which the old board had issues with, but the issue may also be mechanical e.g. slack or hysteresis in the lead screw systems etc.So... I was wondering what other users have experienced with their machines.If the precision is too low even to drill holes, then that's fine, I can still use the machine for other stuff, but it would be good to know whether with some minor changes, whether I could make the thing usable for PCB drilling at least.

author: mc
author_rank: Regular Contributor
timestamp: July 13, 2015, 05:35:24 pm
content: I'd spend sometime going over the basic mechanics, before worrying too much about the electronics.The basic frames, are generally OK, but are let down by poor thrust bearing setups. I've got a ballscrew version, and the ballscrews are actually pretty reasonable (I wouldn't say they'd last long under moderate loads, but they're certainly a major improvement over the leadscrew option), but the thrust bearings that were fitted to mine were total rubbish. I just opted for a named brand version of the fitted single row bearings, but swapping to a similar sized angular contact bearing would increase durability/accuracy more.However, my machine was built solely for digitising/probing parts, so the original controller was removed, with a new controller and linear scales fitted to provide high accuracy.

author: RogerClark
author_rank: Contributor
timestamp: July 14, 2015, 05:53:08 am
content: ThanksI'll focus on the mechanics