Anyone have one of those PCNC machines?.......

[Mace]

Anyone have one of these machines?
Thanks
Mace

 

[David Wesner]

Hi Mace, What is the "P" ? I have a bridgeport type mill with a 3 axis control on it. So far its had the ability to run any G-code type program that I've had the smarts to input.

Where are you going with this question ? I would give you more answers if I knew what direction the questions were headed

Need something made ? I'd love to help you out !

 

[Mace]

Hey David.... the P stands for "personal". I keep seeing this add in "Blade" for the Tormach PCNC 1100 3 axis mill. Thought it might be something I would like to add to my shop in the future. Problem is I have no idea what even a "G-code type program" is. I am willing to learn and I was looking to just bend an ear of someone who has one or has spent any time on one.
Thanks
Mace

 

[dannyvp1]

What you guys need to look for is one that can accept cad/cam drawings. No programming required then. You have someone like me draw them or teach you to, then just send it to the machine and it does the work.

 

[Nathan the Machinist]

What you guys need to look for is one that can accept cad/cam drawings. No programming required then. You have someone like me draw them or teach you to, then just send it to the machine and it does the work.

No offence Danny, but I have to disagree. I believe you're better served with a machine that runs on industry standard G-code. You don't want to dumb down the process so much that it limits the work you can perform, and getting that G-code is easy. You want your mill speaking the language that comes out of CAM programs. Here is how a beginner's work flow might look like:

1: Draw a profile in CAD or an art program. I actually draw on paper, scan it in and use Nonuniform Rational B-Splines (NURBS) to trace my design. This makes a more natural organic shape without constraining your design to the arcs and lines that make computer generated designs look so artificial. There are free drawing programs available

2: Export that profile in an industry standard format such as DXF (or IGS or STP if a 3D file) and bring it into a Computer Aided Machining program (CAM). There are free simple CAM programs available.

3: Generate a tool path. In your CAM system you'll have a place where you can specify depth of cut, feed rate, lead ins and lead outs and things like defining your cutter diameter for cutter offset compensation. There are free CAM programs out there that will do this. I use a not free program, but I'm machining more than knives.

4: Clamp your work piece to your table and find your zero on that part with an edge finder or similar. You can zero the machine at that point with a G92 command, or you can specify an offset from your machine zero with a G54 or similar. You zero your cutter length in a similar way. I'm afraid you're gonna have to learn this stuff. It ain't rocket science. There are a bunch of different ways to zero out a part and cutter.

5: Hit the green button and drink beer. I'm drinking Miller.

Now, this is very basic profile machining. If you have a 3D part design and a 3D CAM program, you can machine more complex parts. See the picts below.

http://nathan.broadtime.com/milled_scales.jpg

These scales are "as machined" meaning there was no sanding or anything, they came of the mill like that. Thats canvas micarta there. The design and fixturing and programming and setup required some skill. The machining required some beer.

You will want a mill that reads industry standard G-code to do complex 3 axis work like that. There are a few basic G-code instructions that most machines understand (though I've had a couple mills that didn't), they are G00, G01, G02, G03. There are also a few basic machining commands such as M03, M06, T codes, S codes and F codes. I won't go into details here, but they're all very simple basic stuff that is pretty well standardized. You'll need to learn the stuff, but it ain't rocket science.

I've used a number of motion controls over the years including Thermwood, Haas, Fanuc, Dynamatronics, Osai, and a PC CNC retrofit from Art Soft called Mach2 (they're up to Mach4 now). The PC CNC has a few quirks, but it is a very solid controller that works very well. That's what I used to cut these scales. I have another mill with a modern Fanuc controller (high dollar motion controller) sitting literally right next to my retrofit mill, but I usually use the retrofit. I'd say that Haas and the Mach2 (now Mach4) are probably the easiest and most ergonomic to use. I'd say the Fanuc is the most robust. I'd say the person who developed the Dynamatronics should be drug out and shot.

I recommend servo based motion control over stepper based. Steppers will get the job done, but servo is smoother and less likely to screw up, just costs a little bit more.

In conclusion, PC based motion controllers work pretty well and are perfect for knife makers because of the low cost and ease of use. I highly recommend Art Soft Mach PC based motion control (very inexpensive, powerful and robust). I got my retrofit hardware from lowcostcncretrofits.com and the thing was just about "turn key".

Anybody getting into this with questions can email me and we can talk on the phone.

 

[Bruce Bump]

Nathan you are my new best friend. Thats informative right there. I've seen the ad for that cnc mill in Blade mag and wondered if its any good. Have you seen it?

 

[Nathan the Machinist]

Nathan you are my new best friend. Thats informative right there. I've seen the ad for that cnc mill in Blade mag and wondered if its any good. Have you seen it?

You talking about the "Syil"?

This may or may not be a good deal for a new small machine, I don't know. "solid concrete polymer" sounds a little strange to me, but perhaps that's a killer innovation, I don't know. It is a stepper system, which I don't like. It only weighs a little over 400 lbs. The smallest CNC mill I've ever used weighs about 3,000 pounds and it is certainly not a stiff heavy machine.

I'll bet the Syil would do fine on scales, I'll bet it wouldn't do so well on steel. But then again, while most folks care a lot about speed, accuracy and surface finish, knifemakers don't need that as much, you end up sanding the snot out of stuff regardless.

Keep in mind you can get a workable used CNC knee mill for $10,000-$15,000 with hardened and ground ball screws (not rolled) powerful servo drives (not 700 watt steppers) and tons of mass.

 

[David Wesner]

Keep in mind you can get a workable used CNC knee mill for $10,000-$15,000 with hardened and ground ball screws (not rolled) powerful servo drives (not 700 watt steppers) and tons of mass.

Which is where I come in. Thats what I have. There are quite a few companies making retrofit controls for the old standard "knee mill". Both 2 axis & 3 axis controls are available. Today, its no longer 100% necessary to be fluant in G-code. Most of the controls I've worked with have whats known as conversational software loaded into the control (usually for more simple 2D work). The CAD/CAM programs that Nathan mentioned will also create the G-code for you (both 2D & extremely complex 3D geometry). The conversational software thats out there now (I'll bet $100 the "?Syil?" machine you're talking about has conversational loaded) have what are know as "canned cycles" (usually often used mini programs where you fill in the data, again... like Nathan mentioned "depth of cut;feeds;speeds;tool being used etc) canned cycle examples might be a slots, pockets, boss', drilling cycles etc. You can couple these canned cycles with standard G-code commands to create a program. One advantage for the small shop knifemaker in going with the smaller bridgeport retrofits is the cost of the machine & control is actually affordable,the tool holders too (the larger CNC machines use CAT tool holders and they can be $$$$$$$$$$$ ), and if need be you can go back to the machine and use in the manual mode. Like while you're learning ,or just have something simple to do where you don't want to spend the time programming and setting up as CNC.

Mace, if you would like to talk about PCNC and how they might help you out in your shop give me a call and we can chat 906-355-2492. They are most definately applicable to what it is we love to do :thumbup:, even if the machine isn't a Syil

Nathan, your work is AWESOME !!!

 

[bhyde]

If you want to check out some of these machines...There is a forum for it,...Search around a bit. Not sure if I am allowed to post a link but it is really informative and is basically a gathering of machinists similar to BF.... CNCzone.com.

There are a few forums I believe dedicated to these smaller machines. I think most of the users are using the largely free CAM programs or very cheap ones. I couldn't tell you if they are conversational or not as I have never ran one. As with Nathan I have programmed, set up and ran several types of mills, lathes. Both with CAM and manually input g-code. Believe me....the CAM programs make life MUCH easier.


HTH


Bill

 

[Vinny203]

mace i was running a bridgeport with a 2 axis bandit hooked up to it today. It was fun. i agree with nathan i have very little machine shop experiance as far as running machines, but even with the big nc mills you never use a cam supplied
code with out checking it and most the time changing it. atleast this is how im being tought. again i wouldnt really count my opinion 6 7 months in the shop with maybe total of just a couple hours of milling experiance isnt enough.
but i like to chitchat

 

[Bruce Bump]

This is the one in Blade mag. Its called a Tormach. sells new for $6800. It's a 3 axis and looks plenty heavy for what we do at least. What do you think?

 

[dannyvp1]

Very informative. But we are on the same side of the fence. I dont run a machine shop just a CAD department. But some machine have to be programmed by hand, and these can take along time to program. My point was just just get one that you can import a stl or dxf file into, by whatever means.

 

[Nathan the Machinist]

This is the one in Blade mag. Its called a Tormach. sells new for $6800. It's a 3 axis and looks plenty heavy for what we do at least. What do you think?

I think you're right. That looks good for what you'll be doing. Flood coolant, three axis simultaneous motion, VFD spindle, ground ball screws, 9.5X18 inch travel, 1100 LBS. Seven grand sounds like a good price if the motion is good. I'm still a little leery of stepper systems, but it sounds like these folks probably do it well.

65 IPM rapids is very slow, but for your application that is probably moot. Actual machining is often done between 10 and 40 IPM.

It does need something to contain chips and coolant, that stuff goes everywhere. It is listed as an option.

Neat machine.

 

[btboone]

I've got the Tormach. It's a great machine for the money. The tooling system has R8 collets with face contact as well, so run very concentric. It's a pretty heavy machine and uses a PC based Mach 3 control.

 

[Nathan the Machinist]

Very informative. But we are on the same side of the fence. I dont run a machine shop just a CAD department. But some machine have to be programmed by hand, and these can take along time to program. My point was just just get one that you can import a stl or dxf file into, by whatever means.

Yes, absolutely. You certainty need the machine to accept data in one form or another other than punching in code at the control. I don't think you have a lot to worry about with anything built in the last twenty years or so. RS232 data transfer for loading G-code is pretty much universal today, though it hasn't always been. Another common problem was very limited control memory which limits program length unless the mill is DNC capable and can be drip fed from a PC. If anyone has questions about this stuff, drop me a line. It is all really very basic once it is explained, nothing to be intimidated about.

 

[Nathan the Machinist]

I've got the Tormach. It's a great machine for the money. The tooling system has R8 collets with face contact as well, so run very concentric. It's a pretty heavy machine and uses a PC based Mach 3 control.

Mach 3 is good stuff.

 

[Chris Meyer]

Well, I think it's all settled then. Mace will buy the Tormach, and the rest of us will take turns borrowing it from him. Better yet, Mace can mount it in a trailer and haul it around to the rest of us.

All in favor say "Aye".

 

[Bruce Bump]

Well, I think it's all settled then. Mace will buy the Tormach, and the rest of us will take turns borrowing it from him. Better yet, Mace can mount it in a trailer and haul it around to the rest of us.

All in favor say "Aye".

AYE :thumbup:

 

[Daniel Koster]

I am very close to buying one of these......scary close.


I can CAD (2D, 3D, NURBS) all day....and use it for pretty much all of my knife designing.

I would love to be able to put it into a PCNC...

Like the others...I'm unsure as to what's involved...full on CNC machines scare me...



Nathan - would you mind guiding me through what I would need to do in order to make use of the Tormach pictured above? (given that I already own/use CAD)

 

[Nathan the Machinist]

I am very close to buying one of these......scary close.


I can CAD (2D, 3D, NURBS) all day....and use it for pretty much all of my knife designing.

I would love to be able to put it into a PCNC...

Like the others...I'm unsure as to what's involved...full on CNC machines scare me...



Nathan - would you mind guiding me through what I would need to do in order to make use of the Tormach pictured above? (given that I already own/use CAD)

Daniel, that isn't a simple question.

Jesus... Where to start...

To me, to fully take advantage of CNC you need a foundation of three things:

1: 3D CAD, to create the geometry you're going to machine. Ideally your CAD skills are strong enough that you're getting the design you want, and not just what you can eek out of the computer.

2: Machining skills. You have to be able to fixture a part and machine it. You don't need to be some zen machining master, but you need to know the basics. There are books out there with speed and feed tables and charts, so this bit isn't too bad.

3: CAM. This is probably the skill you'll need to develop. This is where you take the first two skills and make G-code. This is probably the easiest to learn because for basic needs the programs are straight forward. You're not making injection molds or programming for high volume production. If you can drive CAD, you can learn this.

So, to answer your question:

1: Set up the mill. Set it on the ground, level it, and run 220 power to it. Fill the sump with coolant, the oiler with way lube, break in the spindle.

2: Obtain a CAM system and learn it. This is probably the simplest part of the three part foundation above, but it is the area where you're starting at zero, so figure on about 80 hours before you're very proficient. Hopefully you don't crash your spindle or cut up your table and vice while you learn. Small cutters break before you damage much, so I'd stick to little cutters while you're learning.

3: Set up a post processor. This is usually bundled with the CAM. This takes the machine motions developed in CAM and converts it to G-code specific to your machine. Mach 3 speaks Fanuc Gcode, and there is almost always a default Fanuc post in CAM. Mine needed no tweaks at all to generate good code. This is where an understanding of CNC G-code is important. You need to know the basics of CNC programming so you know what all the code means. It is pretty basic stuff and there are books. You'll need to know the stuff, but not be a master of it.

4: Set up communications with the mill. Being a PC based controller this is simple. You could use a CAT5 cable setup for direct communication between two computer's network cards. Jump drives, floppy disks, a network hub etc. Industrial machines often use RS232. Setting these up requires a little program on a PC and a special cable. The cable is $20, some of the programs are free. You set the communication parameters to match those in the machine, which is normally documented with the machine. You won't need to worry about this because you're using a PC control. Not a big deal regardless.

5: Get a beer fridge. Because you're not turning the cranks anymore, but you want to sit mesmerized by the machine motion, you'll probably want something to drink. And a comfy chair. Perhaps some tunes...


Since you've never seen CAM before I'll describe it:

You create your 3D design in CAD. Hopefully it is good CAD like Pro/E or SolidWorks. Rhino works. FormZ does not.

You export your geometry into your CAM program (as a STEP, Parasolid, or IGES) and define how it is orientated. You define the 0,0,0 point (the coordinate system) on the design.

You define the machining sequences. Perhaps you'll start with a rough bulk material removal with a volume milling sequence. Define a volume (perhaps as simple as making a box around your workpiece) specify a cutter (perhaps a 1/2" square end), rough stock allowance, your speeds and feeds and depth of cut and step over and other machining parameters. The program creates a cutter location simulation and shows you the tool motions it came up with. Then perhaps you'll put a finish cut on some contoured surfaces. Specify a cutter (perhaps a 3/8" ball end) and you'll do a surface mill by specifying the surfaces you want to finish and the machining parameters such as speeds and feeds, accuracy (allowable deviation between programmed motion and surface geometry, I often use .0001"). Perhaps you'll put a finish cut on some profiles with a square end finishing cutter. Perhaps you'll drill some holes by selecting the holes, defining the start and end surfaces and a drill bit and the machining parameters such as peck depth. You may thread a hole with a thread mill. You may bore a hole. One could write a book about all this and I'm getting a little long winded here so I'll stop here.

There are a lot of CAM systems out there. I've only used a few. Many can be bundled in a CAD program, such as a plug in for Rhino. You'll have to find one that does what you need.

Once you have a program and have sent it to your mill and you've got your work piece fixtured and the machine zeroed on the work piece and your cutters zeroed out, you press the green button...

Sorry if I've missed something. This isn't a brief subject I'm afraid.


Nathan