machining ellipse in conversational

[rmason]

I need to machine an ellipse .758" x .365" using a .125 e/mill on a milltronics cent 6. I can create the ellipse in bobcad 19 but I get crazy arcs when using cutter comp on the machine. i think it would work fine if I could change all arcs to tiny lines - like vectorizing text.
Another option-Can anyone explain how to create an ellipse using the conversational side of the control (not using a CAD program)?
My original plan was/is to load the dxf of the ellipse in the control using the cad feature on the conversational side and use mill start etc. But if I could just write the program in conversational that would be great. Any help is appreciated. Russ

[ZZZZ]

You can use a couple of TANGS events and an ARC event to approximate an ellipse, but if it has to be more accurate, I think you will need to use a CAM package to generate it.

I'm not familiar with Bobcad, can you break the spline into lines or arcs?

If yes to lines, save as a DXF file and import that.
If yes to arcs but not lines, create lines at arc endpoints, save and import.

I use Mastercam so I just created the ellipse, broke it into arcs, created the lines, exported the DXF, imported the DXF into FastCam, added the Start and End events, and verified the program. It took me about 30 minutes to get the 227 event program.
Its not difficult, just time consuming.

[Andre' B]

I do not know Milltronics conversational but here is one way to do a ellipse in macro B.

It should not be that hard to translate.

#100= 2    (X AXIS RADIUS)
#101= 0.5  (Y SCALE, 1.0 FOR A CIRCLE)
#102= 1    (STEP ANGLE)
(----------------------)

#103= 0    (CURRENT ANGLE)
G1X[#100*COS[0]]Y[#101*#100*SIN[0]]

WHILE [#103 LT 360] DO1
G1X[#100*COS[#103]]Y[#101*#100*SIN[#103]]F10.0
#103=#103+#102
END1
G1X[#100*COS[360]]Y[#101*#100*SIN[360]]
G0X0.0Y0.0

[sportybob]

if you are getting crazy things happening using the cad comp try turning off the cutter comp on either the cam or the control.
using 2 comps or trig help is like having two GF's show up at the same party, it will get intersting but the outcome is seldom good.

the control cuttor comp is controled by a "special flags" parameter. check the programming manual but I belive that setting it to 2 will turn it off.
or was that for trig help.?? better check the manual.

Sportybob

[ZZZZ]

He asked for a conversational program way to get an ellipse.

Here is a parametric program to get the ellipse:

O1746(LEFT COMP ELLIPSE INSIDE)
D1G43H1 (CALL TOOL 1)
P30=4 (X RADIUS)
P31=2 (Y RADIUS)
P140=.1 (CLEARANCE)
P141=-.25 (Z DEPTH)
P145=5 (Z FEEDRATE)
P146=100 (XY FEEDRATE)
P34=10 (DEGREE INCREMENT)
P35=0 (START AT 0 DEGREES)
G0X0Y0 (POSITION O CENTER)
M03 (SPINDLE ON CW)
S1000 (RPM 1000)
GOSUB 2 (DO ELIPSE)
M05 (SPINDLE OFF)
M30 (END OF MAIN PROGRAM)

N2 (SUBROUTINE)

G41G65X[P30]Y-1 (LEFT COMPENSATION)

X[P30]Y0
G1F[P145]Z[P141]

N1 (LOOP UNTIL DONE)

G1F[P146]X[P30*COS[P35]]Y[P31*SIN[P35]]
P35=P35+P34 (INCREMENT ANGLE)
IF P35<=[360+P34] (360=DEGREE OF ELLIPSE)GO TO 1
G31 (Z UP)
G65X[P30]Y1 (G65 NON MOVEMENT)
G40 (COMP OFF)
G0X0Y0 (POSITION RAPID)
RETURN (END OF SUB)

[jpawelk]

if you are getting crazy things happening using the cad comp try turning off the cutter comp on either the cam or the control.
using 2 comps or trig help is like having two GF's show up at the same party, it will get intersting but the outcome is seldom good.

the control cuttor comp is controled by a "special flags" parameter. check the programming manual but I belive that setting it to 2 will turn it off.
or was that for trig help.?? better check the manual.

Sportybob

You are correct Bob, setting the special flags parameter (found under MISC) to a value of 2 will turn off the trip help feature. You can also do this in your program by entering a PB81=2 at the beginining of the program.
When using a cam software to generate programs it is ususally recommended to turn off the trip help. By turning this feature off this will prevent those odd arcs and tool path moves.