origins, offsets, WCS ,and things that make my head hurt

[Marc Davis]

Hello All

I’ve been lurking for a bit trying not to pester with too many nubby questions. For a bit of background I have a small manual machine shop. Lathe, mill, surface grinder, welding … about 6 months ago I got a deal on a Matsuura 560V CNC mill. It had blown transistors in the spindle VFD. Once I debugged that and replaced the dead IGBT’s it all seems to work. Now I’m trying to get a software tool chain organized. I’m a proficient ProE user so geometry creation is not a problem. What I’m new to is Mastercam. After going through several book and tutorials I’ve got a handle on the basics but they all seem to have a major hole. What is the proper way of relating the coordinate system of the tool path you create to the actual machine. The control on my machine has a physical origin. It also has 6 origin offsets (G54 to G59 I think). Mastercam has the WCS. Several places in the help it says not to move geometry in relation to the WSC in order to relate it to the machines coordinate system, but I can figure out what the correct way to do this is. Would someone be willing to walk through the steps they take in programming a simple part for 3 axis milling, and setting up stock in a mill so that the tool path relates to the stock to be cut correctly? Not the geometry and tool path creation, just getting the coordinate systems to jive. Obviously the details will be different machine to machine, but the broad strokes are what I’m looking for.

Thanks for any help.

[thebowman]

The WCS that you create in Mastercam has to match how you are going to hold the part in your CNC to machine it.

[Matt Berube]

This video has pretty much everything you need to know.

http://www.mastercam-cadcam.com/sample1.zip

If you're using Mastercam X4 take some time to learn how to use the new Dynamic WCS feature... There should be some instruction within Mastercam's help files... maybe even some video if I recall correctly...

[Marc Davis]

Thanks for the video. That answers a lot of questions. The post will use G54-G59 coordinate systems to control where the tool path is relative to that point.
Now, I take a hunk-o-metal and clamp it in the machine in some random place. I turn the machine on and find home so it knows where that is. I stick an edge finder in the spindle and touch off the part to find the point where I want the G54 to be. Then what. Edit the G code to reflect this point? My post seems to include code to set the G54-G59 points. If I set the registers for G54's locations in the control, then it seems like it will be overwritten when the g-code runs.

%
O1007
(PROGRAM NAME - TESTPROG)
(02/13/10)
G54G10Q2P1X0.0Y0.0Z0.0
G55G10Q2P2X0.0Y0.0Z0.0
G56G10Q2P1X0.0Y0.0Z0.0
G57G10Q2P2X0.0Y0.0Z0.0
G58G10Q2P1X0.0Y0.0Z0.0
G59G10Q2P2X0.0Y0.0Z0.0
M63P1

At any rate it seems like I'm very close to understanding this. Thanks again for the video.

Marc

[Matt Berube]

Not sure what all that code is all about. It should be as simple as setting the G54 position, setting the tool length offsets, and pressing the green button.

You should never never NEVER have to edit g-code manually !!! Your post processor can be adjusted to output exactly what you need.

The beginning of my programs look like this so you can see that whatever the machine's offsets determine G54 to be is used in the program.

I am guessing you may have to make some post processor adjustments to get the correct output for your machine. How confident are you that you have a suitable post processor for the machine ?

%
O0000 (TR1896-4D)
(FADAL FANUC MPMASTER 3 AXIS VMC )
(MACHINE GROUP-1)
(MASTERCAM - V13.)
(MCX FILE  - C:\MCX\TR1896\TR1896-4\TR1896-4D.MCX)
(POST      - FADALFANUC_MPMASTER_VMC)
(PROGRAM   - TR1896-4D.NC)
(DATE      - FEB-19-2010)
(TIME      - 12:00 PM)
(T18  -  .750 INS MILL       - H18  - D18  - D0.7500")
(T7   -    .250 CAR BEM      - H7   - D7   - D0.2500" - R0.1250")
(OVERALL MIN DEPTH =  Z-.5)
N100 G00 G17 G20 G40 G80 G90
N110 G91 G28 Z0.
N120 (WCS NAME - TOP)
N130 (TOOLPATH GROUP - TR1896-4D)
N140 (COMPENSATION TYPE - COMPUTER)
/ N150 G0 G90 G54.1 P1 X0 Y0
N160 T18 M06 ( .750 INS MILL)
N170 (MIN DEPTH = Z-.5)
N180 (TOOLPATH - ROUGHPOCK)
N190 (STOCK LEFT ON DRIVE SURFS = 0.)
N200 G00 G17 G90 G54 X-1.5985 Y-.9221 S6000 M03
N210 G43 H18 Z2.
N220 M07
N230 Z.075
N240 G94 G01 Z-.025 F40.
N250 X-.82 Y-.875 F80.
N260 Y.875
N270 G02 X-.375 Y1.32 I.445 J0.
N280 G01 X.375
N290 G02 X.82 Y.875 I0. J-.445
N300 G01 Y-.875
N310 G02 X.375 Y-1.32 I-.445 J0.
N320 G01 X-.375
N330 G02 X-.82 Y-.875 I0. J.445
N340 G01 X-.599 Y-.5709

[Marc Davis]

I got the post with the machine. The company had been using it for years and gave me a V9 post as well as a X post. I'll take some time and look over our G-code so I'm sure I understand it.
Now that I'm starting to understand the WCS and G54-G59 thing I'll post some new code and see what it look like.

Thanks
Marc

[Matt Berube]

One thing I'd like to point out is that it sounds like you do not have a valid license.

It is not lawful to purchase a second hand license of Mastercam unless you contact CNC Software or an official dealer and pay for your own license.

Regardless of what they may have told you when you bought it if you read the "end user license agreement" you'll see that I speak the truth.

Proceed with caution. The fines could cost a lot more than a legal seat of software would.

[Marc Davis]

My day job is for a very large company. We have site/floating licenses for many software packages including ProE and Mastercam. With a bit of finagling I've gotten permission to use a seat of mastercam in off hours. It's hard for me to get help locally because Mastercam is not used in my division. I'm also not anxious to widely advertise my off hours use for fear that someone will put a stop to it. The only thing I got with the machine was the post. My company obviously does not have any equipment as old as the Matsuura.
My machine shop and the Matsuura are a hobby. Permission to use the license is contingent on my not using it to make any money. They frown on double dipping around here.

Marc

[Matt Berube]

That sounds like a reasonable explanation. Just let me know if there is anything else I can help with.