All, The IJ is absolute and G2/3 are the correct directions, proven by running a program without tool comp. The controller does not use the D number unlike a Fanuc etc G40 works correctly and is being used.
I think John Morris is on the right line. This controller is very old and probably does not apply tool comp to the start of the profile in the "usual way". Once the tool comp is started it then works correctly and even finishes in the way everyone would expect with a G40. Here is a longer section of the program N9 G0 X-11 Y25 N10 Z25 M8 N11 Z21 F1500 N12 G1 Z15 F300 N13 G41 X0 F1500 ****** program moves to x-6 y31 not x-6 y25 N14 Y40 N15 G17 G2 X10 Y50 I10 J40 N16 G1 X90 N17 G2 X100 Y40 I90 J40 N18 G1 Y10 N19 G2 X90 Y0 I90 J10 N20 G1 X10 N21 G2 X0 Y10 I10 J10 N22 G1 Y25 **** program moves correctly to x-6 y25 as the next line contains G40 N23 G40 X-11 N24 Z10 F300 N25 G41 X0 F1500 ****** program moves to x-6 y31 not x-6 y25 N26 Y40 N27 G2 X10 Y50 I10 J40 N28 G1 X90 N29 G2 X100 Y40 I90 J40 N30 G1 Y10 N31 G2 X90 Y0 I90 J10 N32 G1 X10 N33 G2 X0 Y10 I10 J10 N34 G1 Y25 **** program moves correctly to x-6 y25 as the next line contains G40 N35 G40 X-11 Nigel Webb Industrial Plastic Fabrications Ltd Tel 01992 893231 www.ipfl.co.uk -----Original Message----- From: Michael Senack [mailto:[EMAIL PROTECTED] Sent: 08 July 2003 15:56 To: Nigel Webb Subject: RE: [mfg-smartcam] Centroid tool compensation I entered the program into SC using the absolute I and J center co-ordinates and it looks fine on the screen. The only thing I could suggest is using an R for the arc definition instead of the I and J, if the control recognizes an R. Another thought is to set the parameters on the control to use incremental I and J values...if the control is capable. I'm presuming that you're canceling your CDC with a lead off line using a G40 command? -----Original Message----- From: Nigel Webb [mailto:[EMAIL PROTECTED] Sent: Tuesday, July 08, 2003 6:59 AM To: [EMAIL PROTECTED] Subject: RE: [mfg-smartcam] Centroid tool compensation Bill, I tried the following (12mm Dia tool) N7 G0 X-11 Y23 N8 Z25 M8 N9 Z21 F1500 N10 G1 Z15 F300 N11 G41 Y14 F1500 N12 G17 G3 X0 Y25 I-11 J25 N13 G1 Y40 This went wrong! It should be a move down and then a 90 deg CCW arc to the edge of the profile except it moved down and then done a CW arc! It is explained by observing the first move down to Y14, it ended up with the centre of the tool at X-5. It applied the comp to the first line rather than at the end of the first line! It is a rather old (and odd) controller!! Nigel Webb Industrial Plastic Fabrications Ltd Tel 01992 893231 www.ipfl.co.uk -----Original Message----- From: Bill Payter [mailto:[EMAIL PROTECTED] Sent: 08 July 2003 10:21 To: Nigel Webb; Subject: Re: [mfg-smartcam] Centroid tool compensation Nigel, What happens if the third line is an arc move instead of G1 Y50? Regards, Bill Payter. ----- Original Message ----- From: "Nigel Webb" <[EMAIL PROTECTED]> To: <[EMAIL PROTECTED]> Sent: Tuesday, July 08, 2003 9:13 AM Subject: [mfg-smartcam] Centroid tool compensation > I'm having problems making a post processor for a :- > > Centroid CNC4-B24-MD3 > > The main problem is applying tool compensation G41/G42 > Most controllers if you do the following will apply comp OK > > Example 12mm Dia tool > G0 X11 Y25 (tool moves to x11 y25) > G1 G41 X0 Y25 (tool moves to x-6 y25) > G1 Y50 (tool moves up y axis) > > > If I do the same with the Centroid > > G0 X11 Y25 (tool moves to x11 y25) > G1 G41 X0 Y25 (tool moves to x-6 y31) ***DIFFERENT*** > G1 Y50 (tool moves up y axis) > > Has anybody solved this or does anybody have a post for a Centroid CNC4? > > Nigel Webb > Industrial Plastic Fabrications Ltd > Tel 01992 893231 > www.ipfl.co.uk <http://www.ipfl.co.uk> > > > ====================================================================== > To find out more about this mailing list including how to unsubscribe, > send the message "info mfg-smartcam" to [EMAIL PROTECTED] > ====================================================================== > > > > ====================================================================== To find out more about this mailing list including how to unsubscribe, send the message "info mfg-smartcam" to [EMAIL PROTECTED] ====================================================================== ====================================================================== To find out more about this mailing list including how to unsubscribe, send the message "info mfg-smartcam" to [EMAIL PROTECTED] ====================================================================== ====================================================================== To find out more about this mailing list including how to unsubscribe, send the message "info mfg-smartcam" to [EMAIL PROTECTED] ======================================================================
