Restart in the Middle of a Program to Run One Operation

[wlcoopercan]

In Fusion 360 Manufacturing, how can I use the Circular Cutting Strategy to rough out a pocket, then Bore the pocket for high accuracy. I want the Mill (HAAS Minimill) to lift the spindle to home (G53 Z0) then stop the spindle, input M00, and allow for me to measure before proceeding with Boring. After Boring, I want to adjust the controller's Tool Diameter Offset, then Only run the Boring Cycle. I can do this with editing the G-Code, but how can I do this in Fusion 360. Shouldn't there be a "send home and pause" operation, but I can't find it.  Would also be useful for clearing chips at certain phases. Thank you. 

[engineguy]

Have you tried using the HAAS "Program Restart" to run the Boring operation again ??

Setting 36 in your HAAS control to ON (Think this works with Pre NGC and NGC Controls as far as I know)

Set the "Optional Stop" to Yes at point of posting and you should get a G53 G0 Z0 and an M1 in your code after each operation so the machine stops, you check your bore, do your tool offset, use the "Program Restart" in the control to start again from the beginning of the Boring operation.

You can in Fusion use the "Manual NC" to insert a G53 G0 Z0 followed by an M00 by using the "Pass through" option to generate the code you need to do what you want but if you need to do more than one tool offset on the bore then I would personally do it with the HAAS control, you are standing at the machine anyway, just use the machine control options 🙂 🙂 🙂

Note: Check out how to do this properly in your HAAS Manual and try it out carefully 🙂

[johnswetz1982]

For both original poster and your suggestion about the manual NC, M01 is for option stop to do things and check sizes, etc. You had correct usage in your first example.
M00 is end program and rewind to beginning. You program will not get further past that point if you use M00.

[programming2C78B]

What you need to do is either do a passthrough, or separate entries for "g00 g90 g53 z0; M00; (stop) then Force Tool Change. You'd then measure, change offset, and hit cycle start for it to run the 2nd (duplicate?) bore operation with the new tool offset. 

[iporter6]

"M00 is end program and rewind to beginning. You program will not get further past that point if you use M00."

Sorry to be that guy, but the above statement is wrong.

M00 will stop the program.  Then you just have to press cycle start to carry on.  Perfect for this type of situation.  It WILL NOT return to start of program.  That is M30.

M01 is for "optional Stop" press optional stop on the control and it will stop. Press cycle start to continue.

The easiest solution for the this request is to select "safe start all operations" and also "optional stop" in the post processor properties and press optional stop on the control.  After the roughing the machine will go to Z home and stop the spindle.  You can then clear swarf etc.  Press cycle start and it will bore the hole and go home in z and stop the spindle.  If you have to re-run the bore, just start it at the bore cycle because it will have all the required code for a safe start.  Very simple.

no manual edit or pass through required.

best of luck. let us know how it goes.

[johnswetz1982]

Its oks to be that guy because you are right and I was wrong in my usage. Having not run a machine for the past year and a half I got it incorrect. And by doing so the next one who reads it will have better information.