Radius??

[Tuz]

Thanks I will try it.
The alarm I was getting was ARC out of tollerance

[ProProcess]

Originally Posted by Tuz Thanks I will try it. The alarm I was getting was ARC out of tollerance

that means that the starting, ending and center call outs do not "fit".


follow dcoupar's advice and remove the center callouts and replace with radius.
this will force the control to fit the commanded radius into the starting and ending points.
Good luck

[FZR1000]

hello

i created a macro program tot mill a given radius on a straiht line
in case you dont want to use a concave or convex mill
the sub progr. calculates the distance of each step in y and z
if it has to be a smooth surface you take a one degree step or
more for faster results

i start at the top of the workpiece and mill then from left to right
calculate a new y and z and go from right to left and so on
until i reach a rotation of 90 degrees

start is at Z0 and finish is at Z-5
it works without radius compensation!!
i am using a 20 mm mill with 0.8mm radius on the edge

and i work in mm not in inches, but that must be no problem

is this wat you have in mind ??

sorry for the bad writting

%
O0310(PARAM.RAD 5MM)
G1902B100D100H25I0J50K0

G0G91Z0M19
T17
M6

M03S1500
G00G90G54X-20Y-10
G0G90G43H17D17Z50

Z0
G01Y-10

G65 P9060 A1 B5 (a= degrees B=radius)

M09
G0G91G28Z0M5
G91G30X0Y0P3M9
G90M37
M12
M30
%


here folows the subprogram



%
O9060(SUB310)
#3=0+#1
N1
IF[#3 EQ #3]THEN#3=#3+#1
IF[#3 EQ 90]GOTO10
#25=#2*COS[#3]
#24=#2*SIN[#3]
#26=5-#24
#27=5-#25
G01X-20

Y#26
Z-#27
X125
IF[#3 EQ #3]THEN#3=#3+#1
IF[#3 EQ 90]GOTO10
#25=#2*COS[#3]
#24=#2*SIN[#3]
#26=5-#24
#27=5-#25

Y#26
Z-#27
G01X-20
GOTO1
N10
M99
%

greetings fzr1000