Official Luthiers Forum!

Here is a picture of what I created today, I spent some time this weekend modeling up a bridge. I just used my Micrometer and a good eye, this this morning I worked on the toolpath, bugged Watkins about some stuff and after 4 attempts this is what I came out with using MDF:





It looks rougher in the picture than it does when you are holding it, I set my stepover to %4 for this one, I also did a quick rough to make the final pass go through less material, total time was about 30 minutes but I think I can get that down by upping the feedrate and making the roughing pass use a larger stepover to save steps. When I was done I checked the bridge with my calipers and it's spot on to what the drawing is...

Very very cool...

-Paul-

_________________
-Paul-

Patriot Guitars

Nice job Paul, you're gettin' there with that CNC, Way to go!

Way to go! Looking good.

So how large of a learning curve is there? How many hours of reading and learning code, playing with the software etc. before someone could produce something like that?

I'm curious of course because eventually I would like to have a small cnc rig. I have a cad background from many years ago, but I'm afraid it's way basic compared to what's out there today, and I never did any 3d stuff at all...

_________________
"I want to know what kind of pickups Vince Gill uses in his Tele, because if I had those, as good of a player as I am, I'm sure I could make it sound like that.
Only badly."

Looking good.

I've got a homemade CNC router I made several years ago.
I may have to dust it off and see if it still works.

Mike

[QUOTE=Don Williams] Way to go! Looking good.

So how large of a learning curve is there? How many hours of reading and learning code, playing with the software etc. before someone could produce something like that?

I'm curious of course because eventually I would like to have a small cnc rig. I have a cad background from many years ago, but I'm afraid it's way basic compared to what's out there today, and I never did any 3d stuff at all...

[/QUOTE]

Well strictly speaking you don't need to do 3D to do CNC, you can do 2D drawings and use those for cutting out parts and things but at some point you will want to move to 3D to do more natural shapes like bridges and necks and things.

I'm actually working on an article that talks about how to get started in CNC and what alls involved. The learning curve goes like this:

First you have to learn the software, this would be the CAD program and the CAM. I use Rhino as do a lot of people, it's easy, priced well and has GREAT support. Plus they offer reasonable training classes in spots all over the country. For the CAM side it's not as intense as the CAD part but it's more tweaky, you just need to spend some time seeing what works and what doesn't. Most people use Visual Mill (they have have Rhino Cam which is visual mill light but is part of the Rhino Interface, this is what I use).

In my opinion those two are the hardest thing to learn, I still struggle with some things in 3D but my teacher from the Rhino class has always offered support when I'm stuck so it makes it easier, also MecSoft who makes visual mill have top notch support, I have yet to have a slow or inarticulate response to my questions.

From there is the hardware end of it, the machine and the control software, it's not as hard to learn. One thing that I'm really starting to believe in is that systems that use the Parallel Port like the Mach Control sofware are not the best way to control a CNC machine (they are cost effective though), the better way is to invest in software that talks to a hardware controller that actually tells the CNC machine what to do. Without going into specifics, you can use a setup like Mach without problems (I'm doing it now), but it's really not the best way to control the machine and in some situations can lead to problems of control or missed steps.

I think the last hurdle is learning how to machine, I have finally started to get a full handle on how to approach this. I'm starting to make vaccum jigs with indexing pins made of acrylic, I like the material because it's flat, machines easily and is airtight.

This is such a broad subject and covers so many areas I've been struggling to get all the information represented correctly, it's been a monumental task so far.

The one biggest help have been people here like John Watkins, without their advice (and Johns patience) I would not be as far along as I am...

Cheers

-Paul-

_________________
-Paul-

Patriot Guitars

Thanks, Paul. I'm happy to help and it looks like you're making great progress.

You're dead on about the parallel port option. The PC should not control the machine, it should be the interface between you and the control.

The Gecko 320's that come standard on a lot of the more affordable machines are still step and direction even though they are servo drives. That makes them a "quasi-closed loop". Since the feedback comes back to the Gecko, not to the PC, the system never knows about the mistakes that the control makes, and as such cannot correct them.

When I build another machine, I will buy a complete control system from one of the less expensive production machine builders like Techno or Haas or Fadal. They all sell it separately.John Watkins38986.3054861111

_________________
John Watkins
CNC Guitar Parts

John--It's been a few years since I last priced a dedicated control but arent' they fairly pricey?
Nelson

Might mention that digitizing 3D shapes is "sometimes" an alternate approach in lieu of 3D CAD. And sometimes a combination of the two works well as a reverse engineering tool. Digitize your bridge with a spindle probe and then import the point cloud into 3D CAD for tweaking.   Only wish that I was as good as John at 3D CAD.
Nelson

Nelson, they start around $5k, which I think is dirt cheap considering that they really do define the line between commercial machines and hobbyist machines.

A great example of this is the new Tormach mill. I was about 5 seconds away from hitting the 'add to cart' button on this thing when I realized it was stepper driven. The machine is very robust for the $6,800 price tag, though. So add a closed loop control and you've got a serious machine for about $12k.

Thanks for nice comments, too (again).     

_________________
John Watkins
CNC Guitar Parts

Nelson I'm getting one from Cam Soft for about $3300 that uses my same servos, it's much more robust than what I have today and if I want to upgrade to better motors they offer those too. The more research I've done and the more I learn the more convinced I've become that it really is the best way to go, I know it's more money but the advantages outweigh the cost, had I known all this when I orderd my machine I would have probably gotten something different or at least something without motors and just ordered all the motion stuff from Cam Soft.

Digitizing is an interesting option, point clouds can present their own set of problems. I have to be careful because again I don't want anyone to walk away thinking that if I just get a digitizing arm I can duplicate any shape. Technically that's true, but to make it proper you will still need to spend some time checking tolerances, making sure everything is smooth from all angles.

I have a MicroScribe and instead of using it on that Bridge I decided to do it free hand, partly because in the end I was able to make the frame for the bridge very simple by doing cross sections and then adding surfaces to those. Rhino works really really well if you can keep your models simple, use simple curves and watch the tangency of your objects.

I've also started to center everything on the X & Y, because it's easier to find the center of a piece than rely on an edge and at some point some of my jigs may have to come off, so I'm adding a little point to each of them that my center finder will reference too. Also for things like inlays a center axis makes it sooo much easier to locate where it's going to be cut.

I'll post some pictures of my jigs next week, I have 100' of vac tape coming in this week and then I'll be carving up all my jigs once I determine the right depth for the rubber chanel It's pretty cool what I've done, I found tap so I can actually screw in the vacuum quick connect, these things look great, just a little tweaking and I'll be all set

Cheers

-Paul-

_________________
-Paul-

Patriot Guitars

Guys--I think that we may not be talking about the same thing when we say "dedicated control". I think of a Fanuc, Heidenhain etc. which can interface with a PC for downloading programs but can run without a PC connected. Looks like the Tormach (nice looking machine, by the way) requires a PC for it's control and Cam Soft is software to run on a PC to control the machine.
When I mentioned digitizing, I was thinking in terms of a spindle probe rather than a digitizing arm such as a FARO.
What kind of machine did you buy, Paul?
Nelson

Ahh yes those are different, the CAM Soft has a controller that handles all the communication with the motors, that's the most delicate part and the most intensive. I would bet you ANYTHING that the other like the fadal actually have a similar setup internally. The Cam Soft setup uses a serial port to push just the GCode to the controller, it in turn handles all the translation to the actual machine movements. Unlike Mach where all that takes place over the Parallel port.

I bought a K2 machine, there is an option for a probe but so far I've not been interested, I'm still playing with the digital arm and seeing what it can do :)

-Paul-

_________________
-Paul-

Patriot Guitars

Paul--What kind of digital arm do you have?
Nelson

I have a Microscribe-3D, I bought it used off of EBay, I've used it a couple of times but not with a ton of success. It's like anything else with CNC I need to spend some time working with it to get a good feel for what it can do.

-Paul-

_________________
-Paul-

Patriot Guitars

Paul--Im confused as to what you will be getting with the $3300 Camsoft upgrade that you mentioned above. Does the package include more powerful drivers for your servos?   Are you running Mach2 or Mach3 now for software? What is it about your current setup that is deficient? Just curious.
Nelson

That's a fair question, let me explain what led to me do all this...

The machine I have uses servo drives controlled by Gecko controllers, one for each drive as your no doubt aware. All of that is run through the parallel port where MachIII handles all the signals to the geckos to make the motors move. The machine I have is a dual core Pentium from Dell, it's no slouch and is faster than my desktop. But I can only run Mach in the middle setting (you can set the pulse rate, I don't remember the numbers offhand). If I run it at the slowest rate the machine is very slow, in the middle it's better. But if I run Mach at the highest pulse rate the CNC machine rocks but the computer goes almost non-responsive. To the point that I can barely control MachIII...

I did all their tweaks and changes to the OS and it passes all of their tests, but I still have to run it at the middle speed. I could live with that for the most part, however I started running into some bugs with MachIII. For instance when you issue a tool change command nothing happens, it seems that you have to change or add a script to get that to happen, not a huge deal but annoying. What's more annoying is that some commands like GotoSafeZ will do things like move the move the X&Y before raising the Z which is BAD!.

Here's a really cool one for you to figure out, if you go into the inputs on MachIII and make ANY change, it resets your home position settings and defaults your directions and such and never tells you it's doing it. So you go back out and some things are backwards and it homes in the wrong direction. It's incredibly frustrating when your setting up a machine because one screen makes changes in a screen thats in a totally different menu.

What motivated me to start looking at other solutions was that there seems to be no desire to fix these problems, it would be easy to just add the script for the tool change stuff and put out a patch release. Instead you have to go onto the forums to ask for help, and no one from ArtSoft wants to address my concerns. The program does work, but spend some time reading the forums and you will see that a lot of people have problems with missing steps and things of that nature.

The last problem is that I can't expand to do things like turning on dust collection and doing a probe without buying and wiring my own break out box. I spent over $6k for my machine alone and I'm not comfortable modding it like that. K2 will do it but at a higher cost and I would have to add a second parallel port to my machine to accomodate it. Same with a spindle if I got one, I'd have to add a second port.

Because I want to use this machine to make parts and at some point in the very near future I will need it to be reliable I started looking for a better solution. After searching for a while I read some posts from other CNC entusiasts about CAM Soft and went and checked them out, their solution is much better. I had a long conversation with one of the owners and was surprised that he not only knew my machine but explained in detail how their hardware setup would make it more reliable (he actually wanted me to go to better drives to remove the Quasi-Feedback stuff John talked about).

So out of this I get the following:

- I can run my machine faster and it will run smoother (it jerks now when I up the feedrates) because my computer can only push out commands so fast, their hardware does not have that limitation and can feed the machine as fast as it can take it.

- Their software is more mature, has better support and from what I have seen is easier to operate.

- They offer free training if I want or need it.

- Support was reported to be very very good.

- The hardware is already setup to do probes, dust collection, router on and off and I can easily add to it.

- They offer a full set of step by step instructions on how to set their stuff up for my specific machine..

The machine works today, it's slow but it does work and I've learned to work around some of the MachIII stuff but very shortly here I'm going to start making repeatable parts and in my opinion I just don't find MachIII up to the task. Last week it lost ALL my settings and I had to reload them all (I kept a backup in case), that makes me nervous when it's swinging around a 2-1/4 router with a bit in it, so I'm going to switch over to Cam Soft here shorty.

-Paul-

_________________
-Paul-

Patriot Guitars

I find it -really- strange that anything driven through a parallel port should need that amount of processing power (enough to slow down a core duo). If a Fadal controller from before 1990 can run a machine fine at 250IPM then the MachIII people must have really soiled the bed on the software.

It really sucks that your CNC has cost you so much on top of the machine itself. The controller/PC combo is now going to add up to nearly the cost of the machine! By the looks of your progress you'll be rocking it once the tool's doing what you tell it to, though.

_________________
Bob Garrish
Former Canonized Purveyor of Fine CNC Luthier Services

Paul, it sounds like you talked to Gary at Camsoft? That guy really knows his stuff. Doesn't their system use a proprietary language; i.e. not G-code? I could be thinking of the Galil control.

I think we made need to have three categories of controls for the purposes of discussion;

1. the PC pushing steps to individual amps like Paul has,
2. the PC interfacing with a control like I have,
3. the Fanuc-style stand-alone controls like the Fadals have.

I believe that the best solution is number 2. The off-board processing power makes everything so much smoother. You know how when you're cutting something like that bridge above, Mach II will make some jittery movements in the tight areas or segment the cut over the top into 10 movements with pauses at each one? The proprietary control never does that. It just goes back and forth in smooth, sweeping motions regardless of the speed. The Fanuc control will do that too, but only for about 20 seconds because it has so little RAM (typically 256k or 512k) that it can't do more than 200 lines of code in any program. I'm guessing Paul's bridge was something like 5-10,000 lines? They have "trickle" programs that will feed the program from a PC to the control in little pieces, but those become a real pain for pausing the job and backing up a bit.

I think you're going to be much happier with the CamSoft solution, Paul, and I would encourage you to eBay those Geckos if you can and get some traditional amps.John Watkins38989.3134143519

_________________
John Watkins
CNC Guitar Parts

Paul--Thanks for your explanation, I understand now where you're coming from. I registered and visited the CAMSOFT site and understand that you and John are talking about a controller card added to the PC. Several years back that was the only way available to build a reasonably low cost CNC. I remember well drooling over these cards and not being able to afford it. Looks like CAMSOFT is a "one stop shopping" for retrofits and OEM builders.
My first experience with benchtop CNC was a little MAXNC with steppers. Didn't take long to figure out that the tiny steppers were extremely slow and unreliable because of being underpowered. (losing steps) I ran across Kerr Engineering who offered low cost servo drivers with control software and retrofitted the MAXNC. Great improvement.
The Techno router that I'm running now uses a control with Gecko servo drivers and Mach2. I had been thinking about upgrading to Mach3 but now I'm wondering after hearing about all your problems. KERR
Nelson

Edit--John, looks like we're both up early this AM. Do we need to add a 4th category, that being the plug in PC card controller?
Nelsonnpalen38989.3222569444

Your correct John I talked to Gary, I learned more in 20 minutes than all my studying. He knows EVERYTHING and told me all kinds of stuff about my machine, he told me that I made a really good choice but that the controller setup was terrible. So once he understood what I wanted he set me up, what a great guy he is.

It's an expensive soltution but the bottom line is that if I keep running parts like the bridge it's going to wear out the machine because it shakes the gantry. It's not the machines problem it the controller setup, I KNOW that machine can do smooth fast passes but the software can't keep up. No machine can go fast and stop go fast and stop all the time...

I have not decided on what to do with the drives yet, Gary wanted me to upgrade them but that's even more expensive so we compromised on this solution and I can upgrade later if I need too. That seemed the most reasonable solution to me at the time...

Nelson the one I'm looking is a seperate unit all to itself, you hard wire it to the gecko's in my case and then all communication is done through the serial port with the computer.

As for MachIII like MachII it will do the job, make no mistake about it but it has some of the weirdest behaviours I have ever seen and they just don't even want to talk about it. It could be a great package actually with some refinement, I've run into a lot of software like that. I had to decide what was important for me in using this machine, at some point I will be making tools and jigs using this and possibly some other things (the wife wants to get back the cost of the machine somehow ). So it was either struggle with Mach or upgrade and get smoother cuts and more reliable performance and that's the choice I'm making, but it hurts the pocketbook

One thing to keep in mind that Gary told he, if your machine pauses, crashes, stalls or anything while issues a movement command to the controller (like the Geckos), it CAN crash the machine. He related a story about a shop that had a machine run a spindle down into a clamp, through the part and shot scrapnel across the shop. The guy was planning to upgrade and was having computer issues, the computer locked up at the wrong time, destroyed his spindle and all kinds of stuff. With Gary's setup that would only happen if you programmed it to do that, since the controller actually talks to the machine, if the PC dies the controller just stops the machine and waits.. AND the other thing is the emergency is tied to the controller and NOT the PC, if you PC dies in that case and your using Machii. There would be nothing you could do to stop the machine short of powering down...

Just something to think about..

-Paul-Sprockett38989.5103356481

_________________
-Paul-

Patriot Guitars

Paul--Have you tried using the G64 command for continuous contouring? I don't get the shaking problem that you're describing. Also might want to look at your configuration settings for speed and acceleration in Mach3. You want the graph to show some gentle slope rather than vertical for acceleration and deceleration. (ramp up/ramp down)
I'm guessing that you've already looked at this?
I'm not selling Mach, just trying to be helpful.
Nelson

I'll look today and see, the motors should be tuned correctly.. it only happens when I push the feedrate up, otherwise it's nice and smooth...

-Paul-

_________________
-Paul-

Patriot Guitars

This seems like a great instructional book waiting to be written.

Mach3 videos
I watched the Mach3 video on "screens" and now I'm excited about upgrading as it has several neat features unavailable in Mach2.
Nelson