Problem- 4th axis machining

[jayroach]

Have a round part 6 inch in diameter with a series of angled pockets on the OD. running on Hass 4th axis. I have one pocket roughed and finished out using multiaxis 5 with a 4 axis output and paralell finishing and it looks pretty good, but i cant seem to rotate the part to the next degree callout and duplicate the same pocket. xform translate with a rotation i have tried but the tools seem to stay in 3 axis instead of 4 after the first pocket is complete. not much success with rotating the planes. any ideas for rotating the part and copy'n toolpath operations for the other pockets? Running X4

[Superman]

use Transform operation
-Rotate (type)
-toolplane (method)
-select ops to transform
-group by Op type ( if more than 1 op )
-no checks
-maintain ( offset numbering)
rotate tab
-origin
-3 steps
-start 90
-rotate 90
-Right ( rotation view )

[jayroach]

Glitch withing mastercam using transform when you are using 5 axis toolpath with a 4 axis output. ended up having to rotate planes. Mastercam confirmed

[Superman]

-Rotate (type) -toolplane (method) <------plane -select ops to transform

that's what I said here.

Not aware there was a bug

[jayroach]

yeah for some reason it would not repeat the pockets consistantly. one pocket would always be wrong in the rotation

[Smrtman5]

So in this approach youre rotating the WCS right? The workpiece remains stationary and the tool rotates around the part in the 4th axis?

[WallyL7]

Originally Posted by Smrtman5 So in this approach youre rotating the WCS right? The workpiece remains stationary and the tool rotates around the part in the 4th axis?

Toolplane is rotating as superman stated a few times...not wcs. That is how you do normal 4th stuff. Rotating the wcs will give you new offsets, instead of just an A-axis move.

[gunaydinemre]

it is easy for me to do this job 4axis ferforje (wrought iron)
you can watch it

YouTube - Mastercam www.cadcamcmm.com

[Smrtman5]

So i figured out the rotation part by rotating the toolpath.

However, the code output contains changing work offsets, which i do not want.

Im cutting 50 slots in the face of a part, but im cutting 25 evenly spaced, then another 25 evenly spaced (yes, there is a logical reason for this).

The code for the 1st 25 slots (Op 2 in Mcam) change the work offset with each A axis index. The code for the 2nd 25 slots (Op 3) only change the offset once.
I tried both "off" and "maintain source ops" but it still produces this issue. I could just delete the G54, G55, etc etc on each line, but Id like to know why this is happening.


Op 2(...
N2770 G90 G126 X-.5322 Y1.0224 Z.01 A316.8
N2780 M98 P0001
N2890 G90 G127 X-.5322 Y1.0224 Z.01 A331.2
N2900 M98 P0001
N3010 G90 G128 X-.5322 Y1.0224 Z.01 A345.6
N3020 M98 P0001
N3130 G90 G54 X-.5322 Y1.0224 Z.01 A360.
N3140 M98 P0001 )

Op 3(N3250 G90 G129 X-.5322 Y1.0224 Z.01 A367.2
N3260 M98 P0001
N3370 G90 X-.5322 Y1.0224 Z.01 A381.6
N3380 M98 P0001
N3490 G90 X-.5322 Y1.0224 Z.01 A396.
...)



As a side note, i would like to write the indexing with macros or another subroutine and clean up the code a bit if possible, but im not that familiar with that.

[Aquatic]

Originally Posted by jayroach yeah for some reason it would not repeat the pockets consistantly. one pocket would always be wrong in the rotation

Now it all makes sense. Had the same trouble a while back.
I found if you rotated more than 1 instance, that's when there were issues.

I did a separate Rotate operation for each of the 5 "wings" I was cutting. This worked.