[Steve Manthey]

I'm trying to edit my spost for 4 axis milling. I'm drilling and tapping holes around a cylinder. After drawing my part, I clicked on NC, 4 axis, Drill, selected the holes, and clicked Done. I then filled in the Tool Information page, and then went to the Cycle Control page to select "Ridgid Tap", filled in the Depth, selected OK, and accepted the tool path. Now, when I go to the Operations Manager to post this 4 axis program, it posts a program, but there is a warning message in the program saying:

M00
!UNSUPPORTED CYCLE PROGRAMMED

Below, I pasted the part of my spost file that caused this:

CIMFIL/ON,CYCLE
CYCTYP=POSTF(7,4)
CASE/CYCTYP
WHEN/ICODEF(LTAP),ICODEF(RIGID),ICODEF(LRIGID),$
ICODEF(CUSTM1),ICODEF(CUSTM2),ICODEF(CUSTM3)
STOP
INSERT/' !UNSUPPORTED CYCLE PROGRAMMED$'
RSLT=POSTF(10,2,14000)
RSLT=POSTF(13)
WHEN/OTHERS
RSLT=POSTF(13)
ENDCAS
CIMFIL/OFF

When I select "Tap" instead of "Ridgid Tap" my program looks just fine, except that it outputs a G84 instead of the required G84.2 In my "Option File Generator" I selected 84.2 in the "High Speed Tapping" window on the "Prep/G Codes" page.

To get around this, I just added at the end of the post, this:

REPLAC/(TEXT/'G84'),(TEXT/'G84.2')

That gets me the code I'm after, but I have to click on "Tap" instead of "Ridgid Tap" on the "Cycle Control" page.

My question is, where is the information given that the post looks at when giving code to a specific operation? In other words, Where does it say
"Tap" = G84
"Ridgid Tap" = G84.2
"Spot Drill"= G81 and so on...

I notice that I'm missing peck commands in my deep hole drilling cycles too. Once I find out how and where to make these changes, I should be good to go.

During my research I came across this:

Type Loc Default Major / Description

Int 3447 841 CYCLE / Rigid Tap G-Code

Int 3448 1 CYCLE / Rigid Tap G-Code decimal location

I have done a lot of reading and looking, but I just can't seem to find where to use these numbers. I just modified an mpost and that was a breeze compared to this spost stuff...


Can anyone shed a little light on this for me (and anyone else interested)?

Thanks,
Steve

[Excelmachine]

I was always interested in learning more about the SPOST abilities because it seemed so powerful but as you said earlier, it's pretty complicated. I'm still struggling trying to learn it myself but I don't have any suggestions on fixing your problem. In the Surfcam help menu, there is quite an extensive breakdown of the commands used, maybe something in there might help.

[sinderal]

Hi steve,


Just For your reference, those I wrote for TNC530 ISO

CIMFIL/ON,CYCLE
XLOC=POSTF(1,3,344)
YLOC=POSTF(1,3,345)
DPTH=POSTF(7,6)
RATE=POSTF(7,8)
CYTYP=POSTF(7,4)
CASE/CYTYP
WHEN/ICODEF(OFF)
RSLT=POSTF(13)
CFLG=0

WHEN/ICODEF(RIGID) $$ CYCLE/RIGID
CHK=POSTF(7,9)
IF(CHK.EQ.ICODEF(DWELL))THEN
DWEL=POSTF(7,10)
CLER=POSTF(7,12)
CLER2=POSTF(7,14)
ELSE
DWEL=0
CLER=POSTF(7,10)
CLER2=POSTF(7,12)
ENDIF
CALL/CANNED
Zloc=DPTH+CLER
DWEL=TEXT/CONVF,DWEL,3,1,0,0,1
PICTH=INTF(RATE)/SPD
PICTH=TEXT/CONVF,PICTH,3,1,0,0,1
INSERT/'G207 Q200=',omit,CLER,'\$'
SEQNO/OFF
INSERT/' Q201=-',omit,DPTH, '\$'
INSERT/' Q239=',omit,PICTH, '\$'
INSERT/' Q203=+',omit,Zloc, '\$'
INSERT/' Q204=+',omit,CLER2, '\$'
INSERT/' Q211=',OMIT,DWEL, '$'
SEQNO/ON
POSTN/IN,X,XLOC,Y,YLOC,M,99
.......
.......
ENDCAS
CIMFIL/OFF