How to run Shapeoko Pro as a production tool

We are a custom molder and purchased this equipment to clean-up edges and adding cut-out features to molded parts.
I works well for 1 piece, but how do I get it to repeat without returning all the way back to home between parts?
I want to be able to hit start from where the motion ends and begin again from that point.

Edit the G-Code to remove the end-of-file code (M02 or M30) — replace it with instructions to move the machine to where you desire.

2 Likes

There are several ways/methods. I’ll give you a few of the easy/beginner ideas. ((but SOME basic GCode skills are required). I always recommend that if you are making money, feel free to pay a CNC Programmer to edit the file (should only take a programmer a few minutes to do this, but they may have a min. charge) , but you decide what you want to do)) It’s also how we learn…

First the basics, GCode is just a text file so you can do the editing on any text editor. (Not a fan of MSWord since it likes to put weird stuff, and wants you to save it as a special text file. So I recommend using the free text editor that came with your machine (Mac: Text/Edit, Win: Notepad)

  1. Cut and paste.

Figure out how many you need to make in a day/session and copy the program and paste it below the program that you have (that many times) WITH a few exceptions.

So first the what you need/should do:
As Will said, remove the M02/M30. Next you SHOULD BE using something to control your spindle/router (e.g. BitRunner?) for safety, so shut off the spindle with a M5 command (spindle off), next you should raise have the Z raise and move away from your part/fixture (for safety) and lastly add a M00 (pause) to allow the operator to load another part. When the operator is ready to cut the next part, press START

It would look something like this: (just an example)
%
(TOOL/MILL,0.1,0.05,0.000,0)
(FILENAME: )
()
G21
G90
G0X0.000Y0.000Z25.400
(TOOL/MILL,6.3500,0,1.0000,0.0)
M6 T201
M3 S10000
G0X-27.668Y-27.624
G0Z25.400
G1Z-2.540F317.5
G1X-27.503Y-27.781F1905.0
X-27.358Y-27.901
X-27.238Y-27.991
X-27.114Y-28.075
X-26.980Y-28.156
X-26.726Y-28.287
X-26.576Y-28.351
X-26.312Y-28.443
X-26.047Y-28.510
X-25.900Y-28.537
X-25.752Y-28.557
X-25.603Y-28.570
X-25.453Y-28.576

(((HERE IS WHERE YOU START TO ADD THE EDIT INFO)))

G0Z25 (LIFT Z 1 INCH)

M5 (STOP SPINDLE)

G0X100Y100 (MOVE X AND Y RIGHT AND BACK 4 INCHES)

M00 (PAUSE, RELOAD, PRESS THE START TO RESTART THE PROGRAM)

(PASTED PROGRAM BELOW)

M3 S10000 <---- START THE CUT/PASTE WITH THE TURNING THE SPINDLE PART. ((MEANING YOU DON’T NEED THE STUFF ABOVE SINCE IT IS MODAL (LOOK THAT UP IF YOU NEED))
G0X-27.668Y-27.624
G0Z25.400
G1Z-2.540F317.5
G1X-27.503Y-27.781F1905.0
X-27.358Y-27.901
X-27.238Y-27.991
X-27.114Y-28.075
X-26.980Y-28.156
X-26.726Y-28.287
X-26.576Y-28.351
X-26.312Y-28.443
X-26.047Y-28.510
X-25.900Y-28.537
X-25.752Y-28.557
X-25.603Y-28.570
X-25.453Y-28.576

(((AND REPEAT XX NUMBER OF TIMES))

G0Z25 (LIFE Z 1 INCH)

M5 (STOP SPINDLE)

G0X100Y100 (MOVE X AND Y RIGHT AND BACK 4 INCHES)

M00 (PAUSE)

(PASTED PROGRAM BELOW, ETC)

M30 ((( READD THE M30 AT THE END OF YOUR CUT AND PASTE TO END THE DAY/PROGRAM)
(END)

  1. Loops but you will also need something other than Carbide Motion to run them.

  2. etc… multiple fixtures which can use arrays and can be programmed in Fusion360 to run multiple parts on multiple fixtures.

10 Likes

This topic was automatically closed 30 days after the last reply. New replies are no longer allowed.