Set Tool Offsets in NC Program??

[alfalfa]

Is there a way to set tool offsets to the control from an NC program? Also, along the same line, is it possible to do the same for part offsets (G54-G58??)? This would allow me to save all tool and part offsets with the NC file and they would be automatically downloaded to the control each time the part file is run. I had minimal success with part offsets, it would set the number, but then the machine would proceed to move to each offset location.

Desired result:

Sym Pin.nc

(Tool) (Descr) (Length)
T1 1" EM -14.35
T2 1/4 Drill -12.25
(Offsets)
G54 X-2.7 Y-7.12 Z0
%
(Sym Pin for Buzzwheel)
10 G1 X-10 Y...........

Thanks,
AL

[psychomill]

Most machine controls have a way of doing this. The most common is using whats called a "G10" line. This is an example for Fanuc controls:

code:

%
G90
G10L2P1X-2.7Y-7.12Z0. (SETS G54 OFFSETS)
G10L2P2X-5.4Y-7.12Z0. (SETS G55 OFFSETS)

G10L10P1R-14.35 (SET TOOL LENGTH FOR T1)
G10L10P2R-12.25 (SET TOOL LENGTH FOR T2)
.
.
(PROGRAM)
.
.
M30
%

The "L" designates what you want to control (offsets, tool length, tool wear, parameters, etc)

The "P" designates the controling variable (tool number, parameter number, offset number etc)

Not too sure if this would apply to camsoft...

HTH.....

[Ben Olson]

the G10 code in Camsoft is the one code that lets my machine feed properly

( I'm still not convinced that G01 actually works properly in CNC Plus.???... G10 is another feed code in Camsoft and on my machine it operates the way G01 should work , and lets me make parts )

needless to say the use of G10 in your example on a Fanuc control won't be the same on a Camsoft ( but I've been wrong before..... )

[alfalfa]

Thanks guys,

I am using Camsoft Plus. I have not had any obvious problems with G1.

It is installed on an OKK MCV500. It is in production, I am just wanting to make it more user friendly and idiot-proof (impossible?? :-) ). If anyone needs code for a similar machine, let me know. The tool change routine is at about 90%.

_____________________
De Oppresso Liber - Is 61

[Ben Olson]

odd coincidence...... my Camsoft retrofit is also an OKK MCV 500....it makes parts but is nowhere close to what I consider idiot proof...( could just be me ) nice solid machine though

if you don't mind sharing I'd like to see what you did as far as tool changing goes
and did you keep the Mitsubishi servo drives?

[alfalfa]

Re the original drives: they went up in flames. (Something got really hot in the cabinet.) Hence the retrofit. We ended up going to A-M-C DC Servos w/ original motors. The spindle was a bit more picky so we put on an AC drive/motor, this also allowed us to bump the max speed.

As far as the ATC code, the boss is a little bit hesitant to just give it away (it took us several weeks to get it right), but if you have something that might be helpful to us.... Otherwise, I would be happy to go over generalities on it. We finally used a limit switch to replace to prox switch for counting, that made all the difference as it was losing magazine position.

Are you using any sort of handheld pendant? I have tried a gamepad, but its not great...yet. How about feed/speed override pots?

[Ben Olson]

I am still using the original Mitsu Drives ( no flames yet, knock on wood ) and the original DC spindle motor/drive ( it took a little thinking to get that working .... )

and you'd be hard pressed to upgrade the original servo motors... those things are stout

I fully understand on the ATC code... the frustration\success ratio in camsoft can be a little lopsided at times...

I got the handheld pendant from Camsoft... the feed and speed override pots work... just not in real time ( ie: you adjust the spindle speed pot and the NEXT line of Gcode it actually takes effect, same with the feed override )

[intrusion]

I have used the CamSoft handheld controller and the feed/speed pots work as advertised. I even saw this work at their office in California. The feed pot adjusts in real time an so does the speed pot. If your code does not work then I suggest you restore the handheld default file to get the original code from the I/O file. You must have made some changes that are interfering with its normal operation.

Frustration usually comes from not asking for assistance, this I know! and everybody needs assistance at some point whether it's electrical in nature, mechanical in nature or software in nature.
When a problem like that arises it is always best to call the software vendor and ask for assistance before too long, its probably something real simple.

intrusion

[alfalfa]

Still looking for help on the original problem (set Tool offsets and fixture offsets from .nc program). I'm sure it can be done, I just haven't figured it out yet. Camsoft is quite flexible, but like any computer, it will only do what you tell it to do.

[camsoft]

Alfalfa,

The specific answer is based on which product and version you have.

If you're using CNC professional, refer to the explanation at:
QUESTION 180

How do we set up fixture offsets, tool clearance heights and tool length offsets?

If you look at the OFFSET command in the manual which is the back bone of customizing G54 thru G59 you'll notice several optional parameters that allow you to set up the fixture offset values directly from a G code program. The current Default.CBK is pre-set this way, so if you have a new version you simply enter:

G54 X1.1 Y2.2 Z 3.3

This example sets these values into the fixture offset table on the TOOL PARAMETER screen. Open the window after running the G code program to see the values forced into these boxes automatically.

To use G54 - G59 in a program after the offsets have been entered this way or typed in directly to the boxes on the TOOL PARAMETER screen simply place a G54, G55, G56, G57, G58, G59 on a G code line.

To clear the offsets enter G53

Tech Support
CamSoft Corp.
(951) 674-8100
support@camsoftcorp.com
www.cnccontrols.com

[intrusion]

To get back on track here!

In the case of CNC Plus and I believe and you should verify with CamSoft directly, but you can use almost any G-code other than G1, G2, G3, G10 and any canned/modal cycle codes. Refer to the CamSoft manual for default G-code actions. Or you can use any M-Code just like psychomill suggested and include the offset values to store into the control using other letters of the alphabet like L, P or R. I do not have the time to give a full illustration, however look at the following commands in the manual.

ISTHERE
TOOLHEIGHT
TOOLSIZE

The ISTHERE command is used in the G or M code logic to check for any instance of text in the program. Use this to capture the values you want to store into variables then use the same variables with the TOOLHEIGHT and TOOLSIZE with the SAVE parameter to enter the values into the tool parameters page.