Rotate your job

[Farmers Machine]

I set a 4" thick plate on the cutting table and it was not perfect square to the X and Y axis, and at 7000 lbs it was to heavy to square up with a bar. Is there an easy way to insert a G or M code in your program before it starts to cut telling the machine how much to rotate the G code to fit the part to the plate. most of my parts are simple compared to a milling job and the program is hand written in G code and mostly never fills the MDI editor square up. The Cam Soft manual has Rotate in it but there has to be more to it than that. On the Milltronics mill control to rotate it has a conversational set up page where you answer the rotation point and the degrees of rotation you want relative to where you are or to 0 degrees being at the 3:00 Position in the X axis.

Thank You
The Farmer

Similar Threads:

• Need Help!- Rotate
• Need Help!- dmu 50 rotate B i C
• Problem- rotate?
• Rotate G68

[Karl_T]

Farmer,

This could be a bit of a job to do after your gcode is written, Unless the Camsoft techs know a a trick I'm unaware of.

For simple parts, I draw the toolpath in Draftsight X64 (free) then use NCplot to post the Gcode and view the toolpath. Both very simple softwares to use. (Another option is the AS3000 CAD program) You could have these right on your control computer if you aren't networked.

Karl

[camsoft]

There are a few different ways to rotate , scale or tilt the G code program.

The 2 most common are:
G68 to rotate the part at an angle around a user defined X,Y pivot position
-or-
G140 for 2D & 3D part rotation and plane tilting.

See the manual and macro files for examples:
G68 U0 V0 A45
G140 U0 V0 W1 R45

Also see

G141 Mirror/Scale for X only. Negative value mirrors G141 L#

G142 Mirror/Scale for Y only. Negative value mirrors G142 L#

G143 Mirror/Scale for Z only. Negative value mirrors G143 L#


[FANUC G68]' G68 U0 V0 A45 ' U & V are the XY pivot rotation position and A is the Angle
[FANUC G69]' Cancels part rotation


NOTE: normally most CBK files use G68 canned cycle to mill out the interior of a rectangular pocket with user defined corner radius. You can change G68 to be used for rotation instead or else call the [FANUC G68] macro from another G code number if you wish to keep the function of both features. If you wanted to see graphics and/or be prompted to enter the pivot point and angle you can use the matrix logic command to do this conversationally. Although having the values saved and kept with the G code program would be better. See MATRIX below.

Other related macros

[Probe 2 points to align part rotation]
[Auto Align Start Probe]

MATRIX logic command
This command will rotate, scale and tilt the G code cutting motion in 3D until cancelled. You may use any or all of the parameters of MATRIX in a G code program of just a few for an exclusive action such as scaling a single axis to tilt the part up, rotate in 3D, elongate circles, shift it's center point etc

There are ten possible parameters to affect the tilt in 3D, clockwise rotation and the individual scale factor of each axis. The first three parameters represent a vector direction to tilt the part in 3D. To cancel this tilt, enter 0;0;0. The fourth parameter represents any clockwise rotation around the Z axis you would like. This is cancelled by zero. The next three parameters represent the individual scale factor of the X, Y and Z axes independently. Scaling is cancelled by using the value 1. The last three parameters are optional 3D pivot point coordinates to rotate the matrix around. You can obtain a normalized vector from your CAD/CAM system, the VECTOR logic command or vector from the PLANE3PTS logic command.


Tech Support
CamSoft Corp.
support@camsoftcorp.com
PH 951-674-8100
Fax 951-674-3110
PC Based CNC Controller For The Machine Tool CNC Retrofit And CNC Controller OEM market

[Farmers Machine]

Thank You
I was reading the whistles and bells on a burning machine literature and it said that to square a job to a twisted part, you touched off on the corner, then moved to the next corner, and entered the distance to move to touch the corner and then it worked its magic, this sounds very much like touch two points to align part rotation, I will check in the macro files on the control and see if I have this feature.

Thank You
Farmers Machine

[Karl_T]

WOW, I've only used Camsoft sense 2002 and didn't know about this powerful feature.

Of course, I did just learn its no big deal to engrave on a cylinder 4rth axis too

Karl

[vero77]

nice,, good effort to learn camsoft