Fadal bolt circle: what a pita

- P
- Proctologically ViolatedÂ©Â®
  
  Contact options for registered users
posted
14 years ago

Wed, Sep 16, 2009 8:49 PM

Awl --

Just how unintuitive can they make it? Much simpler: just specify circle center, #holes, radius. They make you specify # holes AND the angle AND the starting position -- not ito of angle, but the actual circumference coordinates, req'g and i,j's. AND, g68 don't seem to work with bolt circles. NOW you gotta calc i,j's, for a rotated pattern, AND muck around with the starting position as well. goodgawd....

I have to rotate a 3 hole bolt pattern, due to other-hole conflicts, for these lathe chucks ahm still struggling with. Proly shoulda just drilled a 6 hole pattern. Still might, iffin I cain't get shit to work.

Yeah, the plight of the cadcamless. Thank gawd for spreadsheets and fadal's miserable variables'n'shit....

- U
- Uhh Clem
  
  Contact options for registered users
Vote on answer
posted
14 years ago

Wed, Sep 16, 2009 11:26 PM

formatting link

- L
- larryrozer
  
  Contact options for registered users
Vote on answer
posted
14 years ago

Thu, Sep 17, 2009 1:04 AM

formatting link

Fadal's macro

Here is a user Fadal macro program that machines a bolt hole pattern. First, let's look at an example calling program

O0008 (Main program) * N005 G54 G90 S800 M03 T02 (Select coordinate system, absolute mode, start spindle, get next tool ready) * N010 G00 X3.0 Y2.5 (Rapid to center of bolt hole pattern) * N015 G43 H01 Z.1 (Instate tool length compensation, rapid up to workpiece) * N020 #V1=3D3.0 =91Assign argument V1 * N025 #V2=3D2.5 =91Assign argument V2 * N030 #V3=3D0 =91Assign argument V3 * N035 #V4=3D1.75 =91Assign argument V4 * N040 #V5=3D45.0 =91Assign argument V5 * N045 #V6=3D8.0 =91Assign argument V6 * N050 #V7=3D5.0 =91Assign argument V7 * N055 #V8=3D81. =91Assign argument V8 * N060 #V9=3D0.75 =91Assign argument V9 * N065 M98 P1008 (Machine entire bolt hole pattern with drilling cycle) * N070. . . .

Note that as with any user created canned cycle, the macro will only be doing the machining once a tool has been loaded, the spindle started, tool length compensation is instated, and so on.

The variable assignments (V words) must be set and the M98 command calls the macro. Variables representations are as follows:

V1 - Position in X for center of bolt hole pattern * V2 - Position in Y for center of bolt hole pattern * V3 - Surface in Z into which holes are machined * V4 - Radius of bolt hole pattern * V4 - Starting angle (0 is three o'clock position, plus is ccw) * V5 - Depth of holes * V6 - Number of holes * V8 - Cycle type (81 is for drilling, 84 for tapping, etc.) * V9 - Feedrate for machining

Now, here's the actual macro (program O1008).

O1008 (Macro to machine bolt hole circle) * #V21=3D1 =91Initialize counter * #V22=3DV5 =91Initialize current angle to V5 * #V23=3D360 / V6 =91Constant for incremental angular distance between holes * #R4=3DV7 =91Set R4 to feedrate * #R5=3DV8 =91Set R5 to cycle type * #R6=3DV3 + 0.1 =91Constant for rapid approach plane * #R7=3DV3 - V9 =91Constant for Z bottom position of hole * #:LOOPBEGIN =91Beginning point of loop * #IF [V21 > V6] THEN GOTO :EXIT =91Test if loop is finished * #R8=3DV1 + COS(V22) * V4 =91Calculate X position for current hole based on current angle * #R9=3DV2 + SIN(V22) * V4 =91Calculate Y position for current hole based on current angle * G+R5 X+R8 Y+R9 R0+R6 Z+R7 F+R4 (Machine current hole) * G80 (Cancel cycle) #V21=3DV21 + 1 =91Step counter * #V22=3DV22 + V23 =91Step current angle * #GOTO :LOOPBEGIN =91Go back to test at loop beginning * #:EXIT =91End of loop * M99 (End of macro)