looking for way to skip rapid plane in surfcam

[bigtown]

I am doing a simple face mll op to a high number of parts.
I start at the left top corner, feed 'X', rapid 'Y', feed 'X' and than would like to rapid back to start point without raising 'Z' and than just start cycle over
.015 deeper.

The G-code is taking me back to rapid plane before rapid back down for the next cut.

Is there a setting in Surfcam that will let me skip going to rapid plane??


: T10 M6
G0 G90 X0 Y0 Z2. H7
Z1. M8
S1000 F20. M3
G0 X-1.35 Y-0.05
G0 Z0.2053
G1 X4.6 F20.
G0 Y-1.35
G1 X-1.35
G0 Z1. I want to skip this step.
Y-0.05
Z0.1907
G1 X4.6
G0 Y-1.35
G1 X-1.35
G0 Z1. here it is again
Y-0.05
Z0.176
G1 X4.6
G0 Y-1.35
G1 X-1.35
G0 Z1. and again.

[Shepster]

Try setting your retract plane to incremental with a "0" value.

[josiahFRCC]

I ran this through my cimco and I looks like you can just delete the Z rapid, and it will do the same thing on the one end of your part as the other end. In essence your tool path is going to be a simple rectangle and the short ends will be in a rapid movement. Try this at 2.00 above the part, you never know when a crash is going to happen, when you edit a program (even on simple programs). Better safe then sorry.

[Lyndondr]

I would not skip the rapid just make it small like .010 otherwise you are dragging the cutter over the part and that not so great for the cutter.

[bigtown]

I can not find retract plane.I have rapid plane in the Cut Control tab. when I set that to ZERO it brings the cutter to zero on the first pass but I am starting my face mill 1 inch above ZERO and working down to my finish dimension which it .883

Originally Posted by Shepster Try setting your retract plane to incremental with a "0" value.

[bigtown]

I tried this and you are correct, it gives me the tool path I want.
Thank you.

Is there a setting in Surfcam that will do this for me?

Originally Posted by josiahFRCC I ran this through my cimco and I looks like you can just delete the Z rapid, and it will do the same thing on the one end of your part as the other end. In essence your tool path is going to be a simple rectangle and the short ends will be in a rapid movement. Try this at 2.00 above the part, you never know when a crash is going to happen, when you edit a program (even on simple programs). Better safe then sorry.

[bigtown]

I have the option CLEAR PART ON EVERY CUT checked so at the end of each pass I am off the part.

Thank you for the suggestion.

Originally Posted by Lyndondr I would not skip the rapid just make it small like .010 otherwise you are dragging the cutter over the part and that not so great for the cutter.

[josiahFRCC]

Sorry I do not have surf cam I do have access to master cam though. If you need anything.

[NICK REESE]

bigtown,

It can be done if you have "on" selected in the cutting method box under the cut control tab and put a high number in the maximum feed between box under the 2 axis options tab. I haven't gotten it to work when cutting method is set to climb or conventional.

good luck,

nick.

P.S. I about forgot, under the 2 axis options tab I had the feed between rate set to rapid instead of plung or feed.