Pause after retract on g81 drilling

When I use g81 for drilling a bunch of holes, it drills, retracts, then sits there for about a second before it moves to next hole. Seems insignificant, but when drilling hundreds of holes that only take about 2 seconds each to begin with, that one second pause adds significant cycle time. Any way to eliminate this pause? It's not a big deal, just figured I would see if it's something simple to eliminate it

Post a couple of the G81 lines. I could be that the controller is just figuring out what to do next, dunno.

heres an example

G90 G94 G91.1 G40 G49 G17
G21
G28 G91 Z0.
G90


(DRILL3 4)
M5
M9
T20 M6
S8400 M3
G54
G0 A0.
G0 X154.188 Y170.826
G43 Z15. H20
Z5.
G98 G81 X154.188 Y170.826 Z-10. R-2.8 F300.
X128.588
X102.988
X77.388
X51.788
X26.188
X38.988 Y146.57
X64.588
X90.188
X115.788
X141.388
X166.988
X165.488 Y59.12
X152.988 Y70.355
X140.488 Y59.12
X127.988 Y70.355
X115.488 Y59.12
X102.988 Y70.355
X90.488 Y59.12
X77.988 Y70.355
X65.488 Y59.12
X52.988 Y70.355
X40.488 Y59.12
X27.988 Y70.355
G80
Z15.


G28 G91 Z0.
G90
G28 G91 X0. Y0.
G90
M30

this is a drilling cycle with 25 or so locations. output from fusion 360

Try creating another post and set Use Canned Cycles to No. See if that makes a difference. It will create a huge file, but it takes out G81 and does it all in G1 moves.

Quote:

---

Originally Posted by Jim Dawson

Try creating another post and set Use Canned Cycles to No. See if that makes a difference. It will create a huge file, but it takes out G81 and does it all in G1 moves.

---

Good idea. I bet it would work perfectly, but I'm not seeing it in the post options or in the cam options. The post options do have various "use subroutine" options but they are all set to no already.

looks like theres a post edit i can do. ill try it out

yep, post edit worked fine. just had to add
expandCyclePoint(x, y, z);
return;
after onCylcePoint and it expands canned cycles. havent run it yet, but its all G0 and G1 so im sure it did the trick. Each hole is 4 lines instead of 1, but i dont care. Probably much more with pecking, but ive ran gigantic 3d milling files without issue so its really not a concern. With a little more digging i could probably figure out how to add it as a post option which would be nice since i might want to use cycles in other cases

:cheers: Congratulations!

I looked through a number of different posts, and the only one that I could find that has the Use Canned Cycles option is the Haas Turn post, which is the one I use most often since most of my Fusion work is on the lathe. I'll have to make that edit to the mill post since my Peck cycle drill routine does not work correctly in my mill or lathe software, does a full retract rather than a peck. Need to fix that one day, it's on my to do list.

Quote:

---

Originally Posted by Jim Dawson

:cheers: Congratulations!

I looked through a number of different posts, and the only one that I could find that has the Use Canned Cycles option is the Haas Turn post, which is the one I use most often since most of my Fusion work is on the lathe. I'll have to make that edit to the mill post since my Peck cycle drill routine does not work correctly in my mill or lathe software, does a full retract rather than a peck. Need to fix that one day, it's on my to do list.

---

It's a really quick easy change. Here's where I found it:
https://forums.autodesk.com/t5/fusion-360-manufacture/disable-canned-cycles/td-p/5795297

Just add the line directly below the onCyclePoint line.

I'm getting a bit more confident making post changes. I made a ton of progress on my mill turn post (modified Fanuc turning). I have it working now so that my machine can be left with the horizontal spindle along x axis instead of doing a swap axis. Basically z variables are output in x format and x as z. This requires arcs being disabled since they get funky with x and z swapped, but no big deal. Also had to figure out a work around for horizontal drilling cycles, but I bet disabling canned cycles like done here will work even better than whatever I did. Also had to modify tool changes to use an m6 and standard tool numbers instead of tool plus offset, like t1 m6 instead of t0101. It's getting there. I still have to use 2 separate posts for milling and turning, but I can use manual nc to insert a load and run code at the end of one file to automatically start the next that uses different post. The goal was to do everything 100% in fusion with no manual editing or splicing of gcode for mill turn and I think I'm pretty much there now.

If you add these lines to the post you should get the option for Use Canned Cycles on the setup, it worked for the Mach3 post. Very cool.

// user-defined properties


useCycles: true, // specifies that drilling cycles should be used.






propertyDefinitions = {


useCycles: {title:"Use canned cycles", description:"Enable to output canned cycles.", type:"boolean"},




function onCyclePoint(x, y, z) {
if (!properties.useCycles) {
expandCyclePoint(x, y, z);
return;
}

EDIT: Corrected syntax

Quote:

---

Originally Posted by Jim Dawson

If you add these lines to the post you should get the option for Use Canned Cycles on the setup, it worked for the Mach3 post. Very cool.

// user-defined properties


useCycles: true, // specifies that drilling cycles should be used.






propertyDefinitions = {


useCycles: {title:"Use canned cycles", description:"Enable to output canned cycles.", type:"boolean"},




function onCyclePoint(x, y, z) {
if (!properties.useCycles) {
expandCyclePoint(x, y, z);
return;
}

EDIT: Corrected syntax

---

Awesome! Perfect