Right angle head point toolpath

[K2csq7]

Hello All,

I have X5 and a modified generic 5x fanuc mill post.

Using a right angle head to do some 5x drilling. Everything comes out just the way I would like....

(  0.00 / 90.00 - STATION #   )
(UNLOCK 
(UNLOCK C)
( LOAD T1 M06 )
M00
( CONFIRM T1 H1 D1 DIA =.5 )
G0 G19 G90 G54 Y0. C270. B14.72 S90 M3
G43 H1 X-15.6912 M8
G00 Z1.626
G01 Z-3.374 F50.0
F1. (RESET FEEDRATE TO SAFE VALUE)
G81 G98 X-17.6912 R-16.4412 F110.
C267.15
C264.3

 

I always use a point toolpath for a TLO check on every tool, the point toolpath is first followed by the drilling toolpath (same tool, but force toolchange to get my custom retract)

 

G0 G17 G40 G80 G90 G94 G98
(  0.00 / 90.00 - STATION #   )
M11 (UNLOCK 
M21 (UNLOCK C)
( LOAD T1 M06 )
M00
( CONFIRM T1 H1 D1 DIA =.5 )
G0 G17 G90 G54 Y0. C270. B14.72 S100 M3
G43 H1 X-14.063
G00 Z2.0982
G01 Z-2.9018 F50.0
F1. (RESET FEEDRATE TO SAFE VALUE)
G1 X-15.063 F20.3
M00 (2.0  TLO CHECK )

G00 G91 Z15.
M00
(  0.00 / 90.00 - STATION #   )
(UNLOCK 
(UNLOCK C)
( LOAD T1 M06 )

 

My problem is that I cannot get the point toolpath to use G19...any ideas???

 

TIA

[CJep]

Keith,

The stock mill posts are not equipped to output G18/G19 aggregate head format. The preferred method is to start with a router post and modify it to work in mill. The router post has the functionality to work with the aggregate or the other possibility would be to have a custom mill post written.

 

Here is the header info from the router post:

# Post Name : Generic Fanuc 4X Router.pst

# Product : Router

# Machine Name : Generic

# Control Name : Fanuc

# Description : Generic 4 Axis Router Post

 

Here is how I changed it to work as a mill post:

# Post Name : Generic Fanuc 4X Mill.pst

# Product : Mill

# Machine Name : Generic

# Control Name : Fanuc

# Description : Generic 4 Axis Mill Post

 

Then I made various edits to the router post to match the format for a Haas

[CJep]

sorry, missed this

Using a right angle head to do some 5x drilling.

 

You might want to consider having a custom post setup.

[K2csq7]

Thanks CJep,

The drilling posts out just fine (G19 & all is looking good), it's just my point toolpath for the operator's TLO check that wont work correctly. (an easy fix in cimco, but wanted to get it right outta Mcam). I set up a tplane to get the tool on the right angle (which it does), the only thing I can't get is the G19 for that point toolpath the moves are all correct, but the plane is still G17.

[K2csq7]

Thanks for kicking my brain into gear CJep!!!

I had the new tplane set up with Z parallel to the right angle head spindle, not the machine spindle. All better now

[CJep]

Ah yes, the dreaded Z axis normal gitchagoomey

[K2csq7]

The planes were the easy part, but I could not get it to do what I really wanted.....until I found this. Thank you Colin (if he only had nickel for everytime he heard that )

http://www.emastercam.com/board/index.php?showtopic=28081&st=0&p=196812&hl=+multiaxis%20+point%20+&fromsearch=1entry196812