Masterwood/Holzher project 316-K Help

[moultim]

Hello,

I have just purchased a masterwood/holzher project 316K (1997 manufacture) machining center and I was wondering if someone could point me to a reference for the g-codes that the machine uses. I plan on doing fairly simple 2-1/2D geometry on the machine, and I think I will write my own or adapt an existing DXF to Gcode file. I currently use Sheetcam and an old license of Mastercam for my mill. If I could write a post-processor for this machine on one of these, that would be ideal.

I am sure I am in a little over my head with this machine, but I have rebuilt several metalworking CNCs in the last few years and wanted something bigger. Any information that anyone can provide including sample code, manual or post-processor for holzher/masterwood machine of this vintage, that would be great. I imagine they all use the same controller.

Thank you!

tim

[ger21]

Do you know if it's a CN10 control. I program for a 1998 Masterwood 327 with a CN10.

There's a roughly 10 line header in the g-code file that contains the part x, y, and z dimensions and some other stuff, including the machine park position for that particular part. Say your running a small part at the far end of the machine, you can have the machine park close to the part instead of going home after each part.

As for the G-code itself, it's not standard code, but it's close.
First, there are no rapid moves. The machine does them automatically.

To route, the first line is the start location of your route, and starts with G172, and subsequent lines are either G101, G102, or G103. These are the same as standard G1,G2 and G3 codes. Feed rates are probably in meters/minute. F2 = 2 meters per minute, S is spindle speed in thousands of RPM.

So, say you want to route a 100mm square with the lower left corner at 0,0 here's what you do. Lets use a 16,000rpm spindle speed and a feedrate of 2m/min. YOU also need to call the tool number of the router. We have two, tools #41 and 42. Our tool 41 has an ATC, so it's called as 41/1, 41/2..... 41/5 (for 5 position tool changer). You can also specify an entry (plunge) rate with the E word, as the first move will plunge into the part if the starting Z depth is not 0. Z zero is the top of the part, and Z+ is down into the part.

G172 X0 Y0 Z2 S16 T41 E1
G101 X100 Y0 Z2 F2
G101 X100 Y100 Z2 F2
G101 X0 Y100 Z2 F2
G101 X0 Y0 Z2 F2

This is routing 2mm deep.

You can also use cutter comp with G41/G42, but you must have a lead-in and lead out move.

Something like this. Also just remebered that Y+ is down, so I'd actually program this way. I also ramp in and out during the lead-in and lead out:


G172 X-10 Y-10 Z0 S16 T41 E1
G41
G101 X0 Y-10 Z2 F2
G101 X0 Y100 Z2 F2
G101 X100 Y100 Z2 F2
G101 X100 Y0 Z2 F2
G101 X-10 Y0 Z2 F2
G40
G101 X-10 Y-10 Z0 F2

To drill holes, use G100

G100 X10 Y10 Z10 T5

will drill a 10mm deep hole at 10,10 with tool #5. To drill multiple holes at the same time, you create a sort of "vitrual tool".

I think it's something like:

#T81 = 1,2,3,4
#X81 = 4,3,2,1
G100 X10 Y10 Z10 T81

This will drill 4 holes with tools 1-4, with tool #1 at 10,10 and all 10mm deep.

The X81 reverses the tools if the program is run in a mirrored runfield, if your machine has mirrored runfields.

I don't have access to a manual until Monday, but let me know if you need any more info. If this works at all.

[moultim]

Wow, that is fantastic information! Thank you. I would love to try it out this weekend, but I am still searching for the right shop space with the right 3 phase and space. I am working on getting all of the software in line for when I get the machine going and am primarily in the research phase.

Those examples are incredibly useful. I think I can write a post from almost just that! Let me make sure I have the same controller, but if I do, I would love to get a copy of the manual that relates to this stuff. I hope to have the machine going by christmas, but that may be a little ambitious.

My machine has a 4 position ATC, a grooving saw, a bunch of vertical spindles and three horizontal spindles. So each drill spindle is separate tool and the toolchanger is deliminated by a "/"? I guess then the controller deals with the offset between the router spindle and drill spindles on its own? Any idea how the horizontal spindle work?

I can't thank you enough for the help.

tim

[ger21]

On our machine, the saw is tool # 50, and is programmed the same as a route.

G172 X50 Y50 Z6 T50 E1
G101 X0 Y50 Z6 F3

Don't plunge the saw blade too fast into the work, it's hard on the gears, and they're about $500 just for the parts.

Off the top of my head, the left and right horizontal drill codes are either G82, G83 or G182, G183. One is the left edge, and one is the right. Front and back are similar, adjacent numbers, but I can't remember exactly which ones.

With horizontal drilling, here's what you need to remember. For left to right, the X is the depth of the bore. and for front to back, the Y is the depth of the bore. So if your drilling into the left edge, say 50mm from the front, and 9.5mm down (center of 3/4" board), you'd have something like

G82 X50 Y15 Z9.5 F3 T33

to drill a 15mm deep hole. Now, the right edge would be basically the same code (only G83 for the right edge). The actual X location of the right edge of the part is contained in the program. Remember I said the part size is contained in the file header.

As for the offsets between router and spindles, it's both extremely complicated, but pretty easy once you understand it. There are several sets of parameters that are accessible with passwords. From the tool screen, entering a password will get you the tool parameters. It's similar to a spreadsheet, with X, Y and Z coordinates (usually expressed as UVW) of each tool in hundreths of a mm, typically 5 or 6 digit numbers. This lets you fine tune the locations of the router, saw, and horizontal drills in relation to the vertical drills. Since the vertical drills are at 32mm OC, you don't want to change those. You also have the same information about the pop up stops. What I do is adjust the stop parameters to align with the vertical drills, then, once the stops are where I want them, then I align the other tools to the vertical holes.

When you turn on the machine, you should see a menu of 8 items. Here's what our are, although I don't know the exact terminology they use.

1. Program

This is a g-code editor where you can hand write code, or modify an existing program. There is also a 2D view of your part showing machining operations in greyscale, with white be shallow to black all the way through your part. Programs are organized by number, and are called up to run by there number.

When in this screen, there's a menu at the bottom. If you use the left and right arrow keys, you'll see another set of menu items. In the second menu, on the far right, is a list of all the G and M codes. This is actually a text file on the hard drive in the machine. I can post a copy here Monday if you'd like.

2. Not sure, as we don't use it.

3. This is a CAD/CAM interface which let's you graphically program the machine. I knew how to use it 10 years ago when we got the machine, but have never used it, and don't remember too much about it.

4. Automatic

This is where you run your programs. We use a barcode scanner to load programs from labels on our parts. You can type in the program number, or choose it from a list. Just a note, the list is verrrrrrry slow when you have over 100 or so programs. When you have 1000 or more, it's all but unuseable.

5. Tools

This is where you set yout basic tool parameters. For the drilling spindles, you enter the length, diameter, and feedrate. The vertical drills should all be 70mm, the horizontals 57mm. On our machine, the max horizontal length you can use is about 60mm without the machine giving errors. The feedrate is the default that is used if you don't specify a feedrate in the code. It's not a max feedrate, as the g-code feedrate can exceed the value in the tool table.

6. ??? Not sure what it's labeled

This screen has machine DRO's, as well as Inputs/Outputs. It also has a rest button to home the machine when first started. The machine will not run until it's homed. After pressing reset, you should see a message to "Press Start", which is the cycle start button.

On this screen, you should also be able to raise and lower drilling spindles to change them. Look for a "function" button, then, after pushing it, enter the tool # and push the "on" button to lower the tool, "off" to raise it back up.

7. Again, not sure.

Basically the same as the previous screen, but a display only, with no controls on it.

8. Files.

File management screen, for loading programs into the machine, and changing directories.

[RParton]

Hi,

I am the Parts & Service Manager for Masterwood CNC in North America.

If you are still looking for info or manuals please let me know.

RParton@MW-PS-USA.Com

[KitchenElements]

hi guys,

my boss has recently come into the above cnc machine

he would like me to sell it, the machine is in very good condition, just wondering what is a reasonable asking price and if there are any websites to sell these types of machines


cheers