Heidenhain 151 Post

[huskermcdoogle]

I used update post to update my V9 MPHEID post

(modified to work well) to X from V9.1 . In this process it has seemed to work fine short of one little problem. It won't output the feedrates on drilling and tapping cycles instead it outputs -20. I tried the stock mastercam version and to no success either(seeing if it was my mods). Can anyone shed some light on this? The standard V9 fanuc post updated and works just fine as well. (testing if it was a version problem, no that I need it.)

 

I would contact my reseller if I knew who it was. I am a student and one of our administrators picks up the software. I am not allowed to speak with the reseller without the admin on the line as well. So needless to say I am annoyed by editing posts each time I post a drilling cycle, I have been getting frustrated trying to sort this out, and am losing time on some club parts that need to be made very soon.

 

Husker

[Guest]

If you saved the error log when you updated, then you should go through it and see if there were any error in the update.

 

Good place to start

 

Welcome to the forum

 

If you look through your post you might find errors that look similar to this

code:

---

#CNC<<DUPLICATE>>fmt  X 2 x_tmin     # Total x_min

#CNC<<MSG-ERROR(780)>> Duplicate format assignment

#CNC<<DUPLICATE>>fmt X 2 x_tmax # Total x_max

#CNC<<MSG-ERROR(782)>> Duplicate format assignment

#CNC<<DUPLICATE>>fmt Y 2 y_tmin # Total y_min

#CNC<<MSG-ERROR(784)>> Duplicate format assignment

#CNC<<DUPLICATE>>fmt Y 2 y_tmax # Total y_max

#CNC<<MSG-ERROR(786)>> Duplicate format assignment

#CNC<<DUPLICATE>>fmt Z 2 z_tmin # Total z_min

#CNC<<MSG-ERROR(788)>> Duplicate format assignment

#CNC<<DUPLICATE>>fmt Z 2 z_tmax # Total z_max

#CNC<<MSG-ERROR(790)>> Duplicate format assignment

#CNC<<DUPLICATE>>fmt Z 2 min_depth # Tool z_min

#CNC<<MSG-ERROR(792)>> Duplicate format assignment

#CNC<<DUPLICATE>>fmt Z 2 max_depth # Tool z_max

#CNC<<MSG-ERROR(794)>> Duplicate format assignmen

---

[huskermcdoogle]

Thanks for the advice, no luck. There were no errors in the conversion. Here is the log.

 

1 - 17 Mar 2006 09:07:39 PM - UpdatePost Utility

1 - 17 Mar 2006 09:07:39 PM - ***** Starting update processing *****

2 - 17 Mar 2006 09:07:39 PM - The user has chosen the selected post(s) type as: MILL

3 - 17 Mar 2006 09:07:39 PM - The user has chosen the selected post(s) version as: 9

4 - 17 Mar 2006 09:07:39 PM - Option to create the Machine Definition is: On

5 - 17 Mar 2006 09:07:39 PM - Option to create the Control Definition is: On

6 - 17 Mar 2006 09:07:39 PM - Option to silently overwrite existing files is: Off

7 - 17 Mar 2006 09:07:39 PM - Processing a single post processor file.

8 - 17 Mar 2006 09:07:39 PM - The user is being prompted to overwrite: C:MCAMXMILLPOSTSMPHEID.PST

9 - 17 Mar 2006 09:07:41 PM - The original file: C:MCAM9MILLPOSTSMPHEID.PST

10 - 17 Mar 2006 09:07:41 PM - Copied to: C:MCAMXMILLPOSTSMPHEID.PST

11 - 17 Mar 2006 09:07:41 PM - The user is being prompted to overwrite: C:MCAMXMILLPOSTSMPHEID.TXT_v9

12 - 17 Mar 2006 09:07:45 PM - The original file: C:MCAM9MILLPOSTSMPHEID.TXT

13 - 17 Mar 2006 09:07:45 PM - Copied to: C:MCAMXMILLPOSTSMPHEID.TXT_v9

14 - 17 Mar 2006 09:07:45 PM - The user is being prompted to overwrite: C:MCAMXMILLPOSTSMPHEID.PST_v9

15 - 17 Mar 2006 09:07:52 PM - The original file: C:MCAMXMILLPOSTSMPHEID.PST

16 - 17 Mar 2006 09:07:52 PM - Backed up as: C:MCAMXMILLPOSTSMPHEID.PST_v9

17 - 17 Mar 2006 09:07:52 PM - Initialize processing the post

18 - 17 Mar 2006 09:07:52 PM - Post processor file name: C:MCAMXMILLPOSTSMPHEID.PST

19 - 17 Mar 2006 09:07:52 PM - The post processor file has been successfully opened.

20 - 17 Mar 2006 09:07:52 PM - The post processor file has finished the read process.

21 - 17 Mar 2006 09:07:52 PM - Post version information (input):

22 - 17 Mar 2006 09:07:52 PM - UPDATEPST9 was used to modify this file.

23 - 17 Mar 2006 09:07:52 PM - The post was written to run with Mastercam Version 9.

24 - 17 Mar 2006 09:07:52 PM - The post product type is Mill.

25 - 17 Mar 2006 09:07:52 PM - Initialization of pre-defined post variables, strings, postblocks was successful.

26 - 17 Mar 2006 09:07:52 PM - Search for defined post variables, strings, postblocks was successful.

27 - 17 Mar 2006 09:07:52 PM - Initiate writing the post processor file(s).

28 - 17 Mar 2006 09:07:52 PM - Post version information (output):

29 - 17 Mar 2006 09:07:52 PM - Post processor file name: C:MCAMXMILLPOSTSMPHEID.PST

30 - 17 Mar 2006 09:07:52 PM - UPDATEPOST Version 10. is processing this file.

31 - 17 Mar 2006 09:07:52 PM - The post is targeted to run with Mastercam Version 10.

32 - 17 Mar 2006 09:07:52 PM - The post product type is Mill.

33 - 17 Mar 2006 09:07:52 PM - Writing the post was successful.

34 - 17 Mar 2006 09:07:52 PM - The user is being prompted to overwrite: C:MCAMXCNC_MACHINESMPHEID.control

35 - 17 Mar 2006 09:07:56 PM - The original file: C:MCAMXCNC_MACHINESMPHEID.CONTROL

36 - 17 Mar 2006 09:07:56 PM - Backed up as: C:MCAMXCNC_MACHINESMPHEID.CONTROL.bak

37 - 17 Mar 2006 09:07:56 PM - UpdatePost has created the Control Definition: C:MCAMXCNC_MACHINESMPHEID.control

38 - 17 Mar 2006 09:07:56 PM - The user is being prompted to overwrite: C:MCAMXCNC_MACHINESMPHEID.MMD

39 - 17 Mar 2006 09:07:57 PM - The original file: C:MCAMXCNC_MACHINESMPHEID.MMD

40 - 17 Mar 2006 09:07:57 PM - Backed up as: C:MCAMXCNC_MACHINESMPHEID.MMD.bak

41 - 17 Mar 2006 09:07:57 PM - UpdatePost has created the Machine Definition: C:MCAMXCNC_MACHINESMPHEID.MMD

42 - 17 Mar 2006 09:07:57 PM - ***** End of update processing *****

 

Any other ideas?

 

Husker

[Guest]

How is the feedrate variable formatted

 

like

 

 

fmt F 15 feed #Feedrate

 

Are you using the

 

*feed callout in your cycles?

 

Could you post a cycle or two so we might look at them?

[huskermcdoogle]

# --------------------------------------------------------------------------

# Spindle Speeds & Feedrate output formats

# --------------------------------------------------------------------------

fmt S 4 ss$ # Spindle Speed

fmt 4 spprev # Hold previous selspin value for spin change

fmt 4 cc_sav # Hold previous cc_pos value for comp change

fmt 8 selspin # Spindle Dir

fmt 5 fr$ # Feedrate

fmt 5 fr2 # Feedrate 2

fmt 5 frrapid # Rapid

fmt 4 dirchg$ # Feerate Accel/Decel Flag

 

 

pdrill_calc # Drilling Calculations

setup = abs(refht$) * m_one

peckg = abs(peck1$) * m_one

 

pdrill$ # Canned Drill Cycle

pdrill_calc

n$, sdef, specking,e$

n$, sdef, "1.1", ssetup, setup,e$

n$, sdef, "1.2", sdepth, depth$,e$

n$, sdef, "1.3", speckg, depth$,e$

n$, sdef, "1.4", sdwell, dwell$,e$

n$, sdef, "1.5", strf, *fr$,e$

n$, strl, *initht$, strr, strf, smax, strm,e$

n$, strl, *refht$, strr, strf, smax, smcool,e$

n$, strl, *refht$, strr, strf, smax, sm99,e$

 

ppeck$ # Canned Peck Drill Cycle

pdrill_calc

n$, sdef, specking,e$

n$, sdef, "1.1", ssetup, setup,e$

n$, sdef, "1.2", sdepth, depth$,e$

n$, sdef, "1.3", speckg, peckg,e$

n$, sdef, "1.4", sdwell, dwell$,e$

n$, sdef, "1.5", strf, *fr$,e$

n$, strl, *initht$, strr, strf, smax, strm,e$

n$, strl, *refht$, strr, strf, smax, smcool,e$

n$, strl, *refht$, strr, strf, smax, sm99,e$

 

 

This is what it will output for a drilling cycle. Also it will not put in spindle starts after the first tool.

 

100 BEGIN PGM 0 INCH

110 TOOL CALL 1 Z S5500

120 L R F M06

130 L X+0 Y+0 R F MAX M

140 L X+2.46 Y-1.86 R F MAX M03

150 CYCL DEF 1.0 PECKING

160 CYCL DEF 1.1 SET UP -0.1

170 CYCL DEF 1.2 DEPTH -0.1625

180 CYCL DEF 1.3 PECKG -0.15

190 CYCL DEF 1.4 DWELL 0.

200 CYCL DEF 1.5 F-20

210 L Z0.1 R F MAX M

220 L Z0.1 R F MAX M8

230 L Z0.1 R F MAX M99

240 TOOL CALL 2 Z S950

250 L R F M06

260 L X+2.46 Y-1.86 R F MAX M

270 CYCL DEF 1.0 PECKING

280 CYCL DEF 1.1 SET UP -0.1

290 CYCL DEF 1.2 DEPTH -0.7455

300 CYCL DEF 1.3 PECKG -0.15

310 CYCL DEF 1.4 DWELL 0.

320 CYCL DEF 1.5 F-20

330 L Z0.1 R F MAX M

340 L Z0.1 R F MAX M8

350 L Z0.1 R F MAX M99

360 TOOL CALL 3 Z S300

370 L R F M06

380 L X+2.46 Y-1.86 R F MAX M

390 CYCL DEF 1.0 PECKING

400 CYCL DEF 1.1 SET UP -0.1

410 CYCL DEF 1.2 DEPTH -0.8202

420 CYCL DEF 1.3 PECKG -0.8202

430 CYCL DEF 1.4 DWELL 0.

440 CYCL DEF 1.5 F-20

450 L Z0.1 R F MAX M

460 L Z0.1 R F MAX M8

470 L Z0.1 R F MAX M99

480 L R F M25

490 END PGM 0 INCH

 

Feed shouldn't be -20 in cycle def 1.5 in fact they should all be different and 5 ipm 8 ipm and 6 ipm. Feed of 5 ipm is a value of 50 in heidenhain conversational code.

[Don S at Barefoot CNC South]

In your post look for this, this is were your problem is:

code:

---

pfr         # Feedrate

if fr$ >= zero, fr2 = fr$

if gcode$ = zero, fr2 = zero

if fr2 > zero, strf, fr2

if fr2 = zero, strf, smax

---

[huskermcdoogle]

What do you do to fix it?

[huskermcdoogle]

Anyone have any idea?

[Allan Brown]

in pdrill$ and other drill cycle post blocks search for *fr$

 

on the line before that, add

 

fr$ = fr_pos$

 

and see if that works