Official Luthiers Forum!

I'd like to hear the opinions of some of you guys who've used both Mach 3 and an industrial controller. The new machine I'm looking at uses WinCNC.

Anyway, my old controller was a Shopbot. Kind of crude and course, but pretty much never gave me problems until this spring. I replaced it with a Mach/Gecko controller and was immediately impressed by the smoothness and speed, but have not found it to be very stable. It's also, in my limited experience, needlessly complex. Too many fiddly adjustments that inter react.

What's it like on the industrial side?

Hi Sheldon,

One of the other guys will have to pitch in on the industrial, but I can speak at length about Mach. I have used it since version 1. I am however, about to change. Take a look at this thread on the CNCZone.

http://www.cnczone.com/forums/showthread.php?t=64794

I have one of these in house, but have not yet hooked it up due to my need for some really long linear encoders, or scales. The CNCBrain is gonna get you near industrial controllers for a whole lot less money......thousands in fact. I spoke with Bruce Chaffins, the developer on Wed. of this week and he informed me he is about to make a major upgrade, and this thing is still in beta. He did say that all who had already purchased will be receiving a new board to go with their current Brain so no upcharge prices.

Bruce and I are internet and ph friends, whom have yet to meet in person, but hope to make that happen the last of Feb in Knoxville, Tn. at the Mach Convention there. So far, most of the people using the Brain or oem guys or retrofitters and haven't seen the need to show us p-ons how to properly do a machine!

That said, I plan to either build a new machine, or retrofit my current machine before the first of the year and will use my progress for a diy tut if no one has done it by then.

Now with all that said, Mach is an excellent controller that has tons of goodies. The Brain has the ability to do dual loop feedback at the encoders and on the linear scales, and in addition, it does automatic position correction when using the dual loop system.

Feel free to pm me for my personal email if you like.

Mike

Hey Sheldon,

I'm not exactly sure what kind of info you are looking for in an industrial controller. I work with a Haas VF-3 vmc and a Chmer wire EDM, pretty much everyday. Both controls are to some extent proprietary to the manufacturer (a lot of this is similar from machine to machine with little differences here and there). Both controls are excellent at what they do. They are relatively easy to learn and to use. They are both very reliable. I have had the Haas machine for 10 yrs and the biggest problem I have had with the control is figuring out how to get it to "drip feed" via a RS-232 connection. And that was really my problem and lack of experience.

All that being said...these machines were designed to be used in a metal shop environment and all the yuck that goes with that. I am not familiar with the types of controls that may come on an industrial router.

I doubt this was much help, but I will answer any specific question you may have beyond this. To the best of my knowledge anyway

Jeremy

_________________
________________
Jeremy Vonk

Haas uses the same control for the gantry routers that they use for their VMCs, and I've heard nothing but good things about them. However, all industrial controllers have the same limitations that keep most of us using PC based ones;

1. The trickle-feed issue mentioned above. These controls have 2 meg of RAM or less. They can only hold the equivalent of about 10 minutes of full on 3D work. The Fanuc 10M control is the most popular by far and holds about 800 lines. My standard archtop carving program is 45,000 lines. So you buy a PC that formats the program into little programs and sends them as the machine asks for them. It works fine, but it's $4,000 option on most new machines, which is ridiculous considering they could have just put more RAM in the control.

2. Many manufacturers sell the G-codes themselves as options. You have to pay to have certain ones turned on, such as helical boring, arc interpolation in Z, fixture offset, etc.

3. They are quite expensive, use proprietary amps and servos, and require a crap-load of electricity that is overkill for any machine you'd be building or retrofitting for CNC.

Techno makes a very good control that uses Copley amps and their own software interface. It's pretty basic looking when compared to Mach, but it does all of the same things and it runs a lot better. For about $4,500 you can have VMC accuracy and 1,200 IPM rapids. Their service is among the worst of any company that has ever existed, so it must say something about the equipment that I not only have bought from them more than once, but recommend them to other people. I still haven't gotten my receipt for the machine I bought last April.

My CNC lathe is running Mach3. It's a bit rough and a little unstable, but it works and it's accurate.

_________________
John Watkins
CNC Guitar Parts

I run Mach III at home and I run Fadal equipment at work. The Fadal's are of course faster and more accurate, but for what I am doing at home Mach III and my little K2 cnc work just fine.

I've used legacy Fadal controls and their newer Fanuc controlled machines. As John mentioned, the area where these controls lack the most is in memory - you have to drip feed larger programs. Since Mach III is PC based, it really doesn't matter. The Fanuc controlled Fadal's do have the option of running off of a memory card, which works pretty well.

It all comes down to what level of production you are looking for.

_________________
http://www.PeakeGuitars.com

Hello
Thought I would throw my two cents in and perhaps learn a few things also. My router uses deskcnc. It has a dedicated controller board (which mach 3 doesn't - perhaps an aftermarket one is available) According to the guy I bought it from, the dedicated controller is what makes it more stable than mach 3. I have run lots of programs and parts with deskcnc, and have never had any problems once the program is started. That being said, my main gripe with deskcnc is won't do a helix and doesn't have constant contouring. The helix issue is a problem because I cannot ramp tabs in mastercam (unless they are on a straight part of the design, which there are not alot of in guitar and violin bodies) this always gives me cutter marks (snipe) at the tab, as the machine has to stop, pull up the z for the tab, than stop and return to z. I have thought about switching to mach 3, but I hate messing with something when it works. I also have a wincnc controller board and software I got used, but have not installed it, so I cannot comment on it yet. Our mill at work uses a centurion 4 controller, which is a basic industrial controller. The one feature industrial controllers have (that most lower end pc controllers don't) is a feedrate knob. It is always nice when running a new setup or a new program to be able to slow the feedrate to a crawl so you can be sure it is doing what it is supposed to.

I agree with most of what John said, though there aren't too many programs that won't fit in two megs at the sort of resolution you'd be using on guitar parts. Molds are another thing, but I think a lot of VMC controls are drip feeding from an internal HDD now. The main thing you're (over) paying for on an industrial controller is a better feedback loop and better feedback processing.Most (but not all) PC-based controllers aren't using any specific hardware to handle and process feedback, and so they can't handle the same resolutions at speed that an industrial control can. The exceptions are essentially PCs drip-feeding dedicated motion control hardware which, again, will have a small buffer.

The people making VMCs can charge an arm and a leg for anything they want because they won't sell you a VMC without a controller on it, and once you've sunk 75K into the machine the 3-4K of 'controller upgrades' isn't outweighed by the cost savings of retrofitting a control. There are some companies selling industrial-quality controls for a lot less than Fanuc et al but if you want the system 'ready to go' then the prices start jumping again and there's still the issue of needing to buy the VMC to put it on in the first place if you want to take advantage of the accuracy benefits.

_________________
Bob Garrish
Former Canonized Purveyor of Fine CNC Luthier Services

Well I have to say what I don't like about VMCs are like other people said the propritary nature and learning curve for each machine. I have Mach 3 and love it. It's very stable never had one problem with it and I run it about 12 hours a day 4 days a week. To me it's very easy to use and making screen changes makes it very verstile. The screen program is hard to use as there is little information in terms of a user manual for it, but once you learn how to use it you can remove stuff from screens and add custom buttons and macro. SO I never have to type in offsets for different jigs and what not.

Good point on the feedrate knob. That would make running partfiles for the first time a lot less stressfull. Isn't there a third party one for Mach?

Regarding the helix issue, can you not select the helix and interpolate it into small line segments?

While I'm on the topic, where's a good place to learn more about cnc machining?

I'm self taught, which in my case means I learn as much as I need to get a process to work and then get to work. The advantage is that it's time efficient in that you only learn what you absolutely need. It sucks in that you lack the depth of knowledge that can solve problems you don't even know you have.

you can disable helix in mastercam and it will do just that, give you short line segments and basically do small jumps around a ramped tab. It just gives me a bunch of small snipes instead of two big ones.

I took classes at a local community college here in Phoenix (gateway community college) I took a manual programing class (this is a great help for checking and changing generated code) a class in solidworks, and three mastercam programming classes. I had an exceptional teacher for the first two mastercam classes, and as a result do almost all my work in mastercam (even design work) I also took an advanced cnc mill setup class. This was helpfull in learning the best way to index parts, vises, etc and we learned to use fanuc and haas controllers. As with all education, the teacher makes all the difference.

There are good textbooks on basic machining stuff (cutters, setups, etc), reading one of those should fill in a lot of the theoretical background to help you solve problems. I found the manuals/online help for both MasterCAM and Rhino to be more than adequate at filling in the blanks.

My 'intro to machining' was essentially "here's how to touch off a tool, here's how to square a vise, and here's how to upload a program to the machine....have fun". You can learn a bit from making friends with some machinists about fixturing and setups and dealing with different materials.

You should work to be pretty fluent in G-code, at least enough that you can modify programs in text if not to the point that you know exactly what they're doing. It's all about just reading the manual and watching programs run.

Over time, you should reach the point where you can tell if the feeds/speeds/and cutting conditions are right or not based on sound, but that's a product of experience and paying attention and I don't know of any really great shortcut.

_________________
Bob Garrish
Former Canonized Purveyor of Fine CNC Luthier Services

Thanks for the tips. I don't know why I'm not an online tutorial guy. I watched a couple of the Mach 3 ones and found the solution to my most pressing problems that the printed manual didn't cover.

For the guys with Fadal or Haas machines, how much tweaking did it take to get smooth contours consistently. What was the learning curve like with their controllers?

If you're talking about smooth machine motion then none. VMCs (at least VMCs from reputable companies) are professional machines, if there was tweaking involved to make them work right then the companies would be in all kinds of trouble. When you buy a VMC new the tech comes in, hooks everything up, runs diagnostics to make sure nothing got damaged in shipping, and then leaves you on your merry way (unless you got some sort of training package: the Haas people include some sort of training IIRC).

I haven't messed with the Haas control too much, though it can't be too hard- it has a button for every function, it seems! So far as the Fadal control went you've got Start, Slide Hold, M1 on/off, Feed Rate Pot, Spindle Speed Pot, and Rapid Speed Override on the left and those are all you'll use while the machine's running (spindle on/off is off to the right so you don't accidentally hit it while it's running!). There's one jog wheel, so there are switches to set the jog axis and speed. That's all pretty simple stuff.

There are buttons for coolant on/off, tool in/out, manual data input, jog mode, single-step mode, etc. Stuff that should be on there. Past that there are only a few commands you need to learn for setting tool length offsets, fixture offsets (if you use them), DNCing, uploading programs, deleting and editing programs, etc. You can fit everything you need to know to be a Fadal operator on a sheet of looseleaf. As the programmer, you'll need to learn your G and M codes but that has nothing to do with the control per se.

Oh, and the Haas control annoys me because even though I like a lot of the features a bit more than the Fadal controller it doesn't have independent feed and speed pots which makes it a real pain for proofing programs!

_________________
Bob Garrish
Former Canonized Purveyor of Fine CNC Luthier Services

Hey Sheldon,

The Haas machine is pretty much the way Bob described the Fadal. I learned pretty much everything I needed to know to run it in a 2 or 3 hour training session that was included with the purchase of the machine. It took way longer to learn the CAD/CAM software (Mastercam) than it did to learn the machine control.

Bob, I'm not sure what you mean about the individual speed and feed pots? I can control both individually. There are buttons for both speed and feed that will add or subtract 10% or with the push of another button either setting becomes infinitely variable with the scroll wheel. I guess it's all in what you have to work with and what you learn with. Any industrial machine like this will give excellent quality with little learning curve...as far as the control in concerned.

Jeremy

_________________
________________
Jeremy Vonk

The Fadal control has a pot for each mouted on the controller, so you can change both simultaneously in real time. It's the only thing I really specifically like about the Fadal controller actually. I'd pay extra to have them on there on my next machine (which'll probably be a Haas).

They're not so important for standard type parts, but for delicate or complex parts there can be a lot of fiddling around to get everything coming out at full speed. It would -really- make my day if they were digital pots and I could get a perfectly accurate readout of the exact feed and speed I settle on for a move, so it's either 'one pot at a time' with the Haas or 'it's at around 62%' with the Fadal. Maybe MAG will buy Haas, too, and then they'll make the controller I want

_________________
Bob Garrish
Former Canonized Purveyor of Fine CNC Luthier Services

Gotcha. That would be a cool feature...

_________________
________________
Jeremy Vonk