I’m relatively new to CAM on a lathe and stuck trying to get the top of this queen cut. Does anyone have any resources to point me towards to help me understand this part? It seems like fusion made some changes recently because all of the videos I’ve found reference settings that aren’t present anymore. Therfore:
Well, it has been ages but I wanted to post an update to this thread. Ultimately, my resolution to this problem was to lie to everything under all circumstances and hack my way through it. I could have thrown some money at this problem but I opted to throw time at it instead.
The $ version of this resolution would have been to buy a face grooving tool similar to Face Grooving Products or use a lolipop cutter and cut this top on the mill.
The video below will give a detailed account of how I approach this, as presented (live) to my local MakerSpace. Since this video was posted I did add some FOR loops to the gcode program in order to automate the automatic advance of this tool path. I will post that when I have a minute to gather my notes on that edit.
Solution
I started with one of our button insert lathe tools (SRDCN 06-2J) and then hand ground in some relief.
Then I lied to PathPilot about what I was expecting of it, then tossed half of the generated gcode and had to manually advance the Z axis for each cut.
Feel free to ask me questions.
Here is the WHILE loop that I added to the program to make this work in an automated fashion. I added this to the rook since I was already done with the queen but I have used this technique a few times for non-chess parts.
#1 = 10 (Roughing Passes)
#2 = 2 (finishing passes)
#3 = [#1 + #2] (total passes)
#4 = 0.013 (Rough DOC)
#5 = 0.004 (Fine DOC)
#6 = [[#1 * #4]+[#2*#5]] (total material removed)
#7 = 0 (Z holding place value)(DEBUG, #1 = num rough)
(DEBUG, #2 = num fine)
(DEBUG, #3 = total passes)
(DEBUG, #6 = material to remove)M1
(----- Start of G-code -----)
()G7 (Dia. Mode)
G18 (XZ Plane)
G90 (Absolute Distance Mode)
G40 (Turn Cutter Compensation Off)
G91.1 (Arc Incremental IJK)
G20 (units in inches)
G54 (Work Offset)G30 (Park Tool)
T2828
G96 S 351 D 2000
G95 F 0.0120 (Units per Revolution Mode)M8 (Flood Coolant ON)
M3 (Spindle ON, Forward)G0 z0.5 (go to known position)
G10 L20 P1 Z[0.5 -#6] (move enough for total material removal)o101 while [#3 GT 0]
G0 X1.3000 ( go to safe X, then start Z before issuing G71)
G0 Z0.2600
(G71 P1192 D0.0100 F0.0120 J0.0060 L6 I0.0030 K0.0030 R0.0100 E1)(Finish Pass)
G96 S 351 D 2000
G95 F 0.0020 (Units per Revolution Mode)
G0 X1.3000 ( go to safe X)
G0 Z0.2600 ( go to start Z)
G42 (Cutter compensation - on)
G0 X0.0000 Z0.2600
G1 X0.0000 Z0.0000
G1 X0.1185 Z-0.1310
G2 X1.0923 Z0.0000 I0.1051 K0.5795
G1 X1.2000 Z0.0000
G40 (cutter compensation - off)
G1 X1.3000 ( go to safe X)G0 Z0.400 ( go to safe Z)
o103 IF [#1 LT 2] (check to see if that was the last roughing pass or any finish pass)
M1G10 L20 P1 Z[0.4+ #5]
#2=[#2-1](DEBUG, #1 = num rough)
(DEBUG, #2 = num fine)o103 ENDIF
o102 IF [#1 GT 1] (check to see if still roughing after this)
(DEBUG,#1)
M1G10 L20 P1 Z[0.4+ #4]
#1=[#1-1]
(DEBUG, #1 = num rough)
(DEBUG, #2 = num fine)
o102 ENDIF#3 = [#1 + #2] (total passes)
(DEBUG, #3 = total passes)o101 endwhile
(“o-code subroutine for profile”)
(Note: all profile subroutine code is in parenthesis)
(o1192 SUB)
( G1 X0.0000 Z0.2600)
( G1 X0.0000 Z0.0000)
( G1 X0.1185 Z-0.1310)
( G2 X1.0923 Z0.0000 I0.1051 K0.5795)
( G1 X1.2000 Z0.0000)
(o1192 ENDSUB)M9 (All Coolant Off)
M5 (Spindle OFF)G30 (Park Tool)
()
(----- End of Profiling -----)M30 (end program)
