Transformed Toolpath Not Posting Right??

[Namliek_J@TheeCircle™]

I have a cylinder that I need to mill 8 helical slots in that are 45 deg. apart from one another. So I draw one, go and do a transform toolpath, rotate it starting at 45 deg. withn 45 deg increments using right side for my view. Well, it verifys correctly, but when I try to machine the part, it runs the first contour correctly, but when it goes on to do the second, third, etc... It just remachines the same slot as the first. The part doesn't move the 45 deg. to the next slot. Any idea why?

[Guest]

ON your transform page do you have methed toolplane and type rotate checked?

[Jack Neelands™]

check to make sure you have toolplane checked and not coordinate in your transform

[Namliek_J@TheeCircle™]

it is set to toolplane

[deckerc]

sounds to me like you need it set to coordinate, not toolplane

[Mgrenier]

quote:

---

sounds to me like you need it set to coordinate, not toolplane

---

+1

[Jack Neelands™]

odd .....does it work with coodinate?

[Kannon]

when you post it.. are you seeing a rotary move in your program?

[Guest]

Rotate without Tplane methiod should not generate any rotary axis movement.

 

It needs the T plane to know it supposed to rotate.

[Namliek_J@TheeCircle™]

Type: Rotate

Method: Tool Plane

[deckerc]

Are you using a rotary axis, or do you just want to rotated the toolpath 45 degrees? If you're using a rotary axis and want to reposition your part then use toolplane. if the part is not being rotated and you want to move the toolpath then use coordinate.

[Namliek_J@TheeCircle™]

i am using a rotary axis.

[Jim Evans from CNC Software]

Is the source operation you are tyring to rotate an Axis substituion toolpath??? If so then what you need to do is a translate toolpath as the post does the calcualtions from a linear toolpath to wrtap the part and output code.

[Jack Neelands™]

with my rotary axis i select tool plane......for a simple contour ...rotate around side view (#5)

 

 

 

 

 

 

 

 

and i get this posted

 

 

N2 ($.MIN%) (DATE=DD-MM-YY - 29-06-06 TIME=HH:MM - 09:38 )

N4 G15 H1 G90 G17

N6 (TOOL - 0 DIA. OFF. - 0 LEN. - 0 DIA. - 1.)

N8 G0 G90 X-.5 Y0. A0. M15 S1500 M3

N10 G56 H0 Z5.

N12 Z2.6

N14 G1 Z0. F15.

N16 G3 X0. Y-.5 I.5 F25.

N18 X.5 Y0. J.5

N20 X0. Y.5 I-.5

N22 X-.5 Y0. J-.5

N24 G1 Z.1 F500.

N26 G0 Z5.

N28 X0. Y.5

N30 Z2.6

N32 Z10.000

N34 A90. M15

N36 X0. Y.5

N38 Z2.6

N40 G1 Z0. F15.

N42 X-.5 F25.

N44 G3 X-1. Y0. J-.5

N46 X0. Y-1. I1.

N48 X1. Y0. J1.

N50 X0. Y1. I-1.

N52 X-1. Y0. J-1.

N54 X-.5 Y-.5 I.5

N56 G1 X0.

N58 Z.1 F500.

N60 G0 Z5.

N62 Z10.000

N64 A180. M15

N66 X-.5 Y0.

N68 Z5.

N70 Z2.6

N72 G1 Z0. F15.

N74 G3 X0. Y-.5 I.5 F25.

N76 X.5 Y0. J.5

N78 X0. Y.5 I-.5

N80 X-.5 Y0. J-.5

N82 G1 Z.1 F500.

N84 G0 Z5.

N86 X0. Y.5

N88 Z10.000

N90 A270. M15

N92 X-.5 Y0.

N94 Z5.

N96 Z2.6

N98 G1 Z0. F15.

N100 G3 X0. Y-.5 I.5 F25.

N102 X.5 Y0. J.5

N104 X0. Y.5 I-.5

N106 X-.5 Y0. J-.5

N108 G1 Z.1 F500.

N110 G0 Z5.

N112 X0. Y.5

N114 Z10.000

N116 G0 G30 P1

N118 M02

%

[Namliek_J@TheeCircle™]

the contour is an axis substitution toolpath

[Jack Neelands™]

wow i just tried that and crashed it when i went from the mirror back to rotate and yeah its doing something funky here...my tool just went through my part on the rotated side when i chose Coordiante...when i chose toolplane it looks good but doesnt post out the second toolpath in the right spot...it starts over in the same spot as the first one

[Jack Neelands™]

so no axis subbies for me ....lol

[Jack Neelands™]

did you want to try a 5 axis curve and then rotate it?

[Namliek_J@TheeCircle™]

no, didn't try that.

[Jack Neelands™]

that workes here ..i use that all the time....even though i have a 4 axis ...im used to 5 axis machining and well...maybe its a personal thing ...but i dont roll the tool too much or use the rotary functions unless i really have to...put a snippet on the ftp site and we can compare notes if you wish

[Jim Evans from CNC Software]

Do not use Transform ROTATE of an Axis Substitution toolpath!!! Read the post and it explains that Axis Substitution must be programmed from the flat. That doesn't mean program the first one from the flat and then rotate it using transform

 

Rotary subprograms of rotary substitution is really messy. Toolplanes and rotary sub logic start to interfere. There is no way to know what you are intending to do, or which angle calculation should win out.

 

It's much better to do a translational transformation of the "unwrapped" geometry. Instead of a transofrm rotate, do a translate and calcualte the linear shift to acheive the same rotation.

 

Works like a champ.

[Jack Neelands™]

ahhhhhh...ok then so flatten the part with a hammer till its nice and smooth on the screen and the run a cutter along it?...then it will rotate around properly in the transform...gotcha!!

[Kannon]

can someone please get jack a hammer?

[Jack Neelands™]

 

 

found one!!!!!!!!!!

[Jean Paul]

May be all you have to do is to change this line in the post processor. because a value of 3 always makes the first point of the subroutine to be the same as the first run

 

#Subprogram variables

mr_rt_actv : 0 #Flag to indicate if G51/G68 is active

#0=Off, 1=Toolchange, 2=Subprogram call/start, G68

#3=Absolute start, both