Optional stop

[Anonymous]

Hi All,

I am working on a tube setup which is 60'' long and my table can only travel 28'', so I have to program my stock is three setups. I am adding optional stops to the program to move the stock before next setup but my program is not showing spindle start again(M03) so I have to manually add spindle speed before start of my next setup

G1 X1.4397 Y0.2509
G2 X1.4402 Y0.2496 I0. J-0.0008
G1 X-0.2496 Y-1.4402
X-0.3168 Y-1.3731 Z-0.3655 F30.
G0 Z0.6
M1
(MOVE STOCK 22'' TOWARD ORIGIN)

(2D Pocket1 2)
M3   Adding manually
G0 X8.5447 Y0.2515
Z0.6
Z0.2
G1 Z0.0394 F20.
Z-0.375
Y0.2496
Y-0.032 F40.

I like to keep one fixed origin and move my stock, even tried multiple work offsets but didn't help may be there is an option that I am not selecting.

Thanks

[Steinwerks]

This is something that can be set up in the post. I have ours set up to use the Manual NC Clean function with a Comment to instruct the operator in what to do. Which post are you using?

[lenny_1962]

When I did this once about a year ago I added two manual nc ops, one for the M1 and one with a tool change so that when I hit the start button it would start right up in the program. Only way to get it to work with out me putting into the code.

[Anonymous]

I am Posting to to generic HAAS milling,

something else I added a  force tool change(one of the option in Manual NC) and it has put optional stop and spindle speed back to every setup. Using same tool in my parameter operator just have to hit cycle start after new setup

X1.8841 Y0.1855
X1.9866 Y0.2496
X1.9362 Y0.3301 Z-0.3655 F30.
G0 Z0.6
(Flip to back side)
M5
G53 G0 Z0.

(2D Pocket1 2)
M1         Force tool change
N15 T1 M6
S4000 M3   Addition because of tool change
G54
G0 X4.7526 Y0.2506
G43 Z0.6 H1
G0 Z0.2

Thanks

[Greg_Haisley]

This is exactly why we need to be able to drive the tool via. a 3D sketch with some options like spindle orient (M19), spindle stop (M5), optional stop (M1), program stop (M0) maybe even 4th or 5th axis positioning, ect..... This way you would be able to drive a tool along a 3D toolpath and implementing the options checked or some other way of designating the desired CNC action. Then you would have another 3D sketch to retract the tool on a path the user desires. No manual edits. I hate manual edits because you are doing a work around because the software won't give you what you want. Another reason for the system to do this is the ability to be able to simulate the program. In this case the simulation would stop at the M0 or M1 program stops and wait for the CNC programmer to hit the enter key to resume the simulation.

A robust CAM program would provide the ability to do something as simple as a program stop without manual NC function intervention or manual edits.

This is my little CAM rant for Friday 1-6-2017.

Have a great day everybody.