2D Milling 2 Setup Program

[aldepoalo]

In this video I walk through programming 2 setups for a 2D part.



Similar Threads:

• New Machine Build- Mori Seiki ZL-253 program setup
• Need help with old DOS gcode program setup
• Free MastercamX setup sheets for milling free 3 axis milling active designer setup sh
• cnc lathe program/setup
• Newbie- How to setup and program sub-spindle on TL-25?

[photomankc]

Al,

So what would the normal course of action be to allow for the operator to re-position the stock between Setup1 and Setup2. In my other CAM package I created an auxiliary operation that forced a tool change to Tool 0, Sent a message to re-orient the stock and paused. If I had to re-zero then I'd just stop the program, re-zero and resume from that point.

[photomankc]

Never mind, I think I have this handled in the post:

16. Machine Setup Change
" "
"(*********** START SETUP CHANGE **********)"
n,"M5"
n,"T0 M6"
n,"G49"
n,"(MSG, Reorient Workpiece for Next Operation)"
n,"M0"
"(***********  END SETUP CHANGE  **********)"
" "

[stucapco]

Off topic. photomankc CNC: Making incorrect parts and breaking stuff, faster and with greater precision.

I'm still laughing, right on, don't let them discourage you man! You stand in!

Bobcad, fine, I've used it since version 8, mill and wire. V27? Over kill. By the time I fine tune, setup the post, I could write the code by hand.



Old school still running!

[aldepoalo]

That's what I would do, is using the advance posting tab giving you an option at tool change to throw an M00 or M01. I would change the feature name in the tree as well to note the part flip so the operator will see the flip in the code...

[photomankc]

OK,

That almost worked. First chips from BobCAM and everything went well up to the part flip. I ran a simple stock-prep facing routine first and after the flip and changing Z zero the @#%$ hit the fan when I did a "Run From Here" in LinuxCNC. The GCode asked for Z0.2" the control went to Z-1.825. It was impressive to see the Tormach SuperFly cut a cylindrical path into the side of my part at around 90IPM! More impressively it survived as it was a glancing blow.

It must have something to do with the G49. Despite me doing T15 G43 M6 in MDI mode, the canceled tool offset remained in place once running a program and shifted the zero to the spindle nose. BobCAM does not specify a tool load in the next setup and so the offset remained canceled from my postprocessor changes. Owch. I came up with this which seems safer:

(*********** START SETUP CHANGE **********)
N59 M5
N60 M9
N61 G53 G0 Z0
N62 G0 X-0.250 Y0.0
N63 (MSG, Reorient Workpiece for Next Operation)
N64 M0
(***********  END SETUP CHANGE  **********)
(>>>>>>>>>>>   RUN FROM HERE    <<<<<<<<<<)
N65 S1800 M3
N66 M8

My other CAM package the part flip was a custom operation and so the tool change/unload was known to the software, my custom post of course is transparent to BobCAM so I need to get back to where things were, spindle turning and coolant back on.

[jrmach]

mishaps already on BoB.
It happens
but
Preditor Editor 2 offers G-Code back plotting.This is available thru BoB as an add on.
Cannot even begin to tell you how many times it has saved mt butt.Well worth the money.
As cool as the simulator is , Preditor Editor will catch stuff the simulator doesn't.
But in the end,it is not fail proof either,just another tool in the box.

[photomankc]

We just had to learn to get along is all

I tried the HSM toolpaths and WOW what a difference. That 1.5" 3/8 endmill went from a squealing nightmare to purring along with a rooster-tail of chips flying out. I was damned impressive to see. 0.350 DOC, 0.060 WOC, 4200 RPM and 42IPM. Cut the job from 50 minutes to 30 minutes!

[stucapco]

"CNC: Making incorrect parts and breaking stuff, faster and with greater precision." I'm still laughing!

True, end of story.