posting/programming question

[Bruce]

MC ver8.1

Machine - Bridgeport Mill

Controller - Heidenhain TNC370

Programming - Conversational

 

Have any of you come across this problem.

 

What would cause a program to change its format while being downloaded to a machine?

The universal drilling cycle (203) looks fine in the CIMCO editor (as it would, if I programmed it on the machine) but once it is downloaded to the machine it is not being recognized as a drill cycle but as separate lines of comments with the ; symbol in front. I am unable to delete this symbol, as it seems linked to the line number. The only why to remove it to delete to whole line and this is not what I want.

 

Is there something in the post that would cause this or is it more likely to be in the controller???

 

Thanks in advance

Bruce

[Reece L Gibson]

Have you ever had problems with it before?

[Bruce]

Millturn

 

No, this is the first time. However I have only started to mofify this post to do some of the more unusal canned cycles that the TNC370 controller is capable of.

 

Bruce

[Claus@Cimco]

Hi

You probely forgot the " ~ " after every line

 

17 L Z+10, R F MAX M

18 CYCL DEF 203 UNIVERSAL DRILL ~

Q200=10, SET-UP CLEARANCE ~

Q201=-10, DEPTH ~

Q206=30, FEED RATE FOR PLUNGING ~

Q202=2, PLUNGING DEPTH ~

Q210=0, DWELL TIME AT TOP ~

Q203=0, SURFACE CORDINATE ~

Q204=10, 2. SET-UP CLEARANCE ~

Q212=0, DECREMENT ~

Q213=0, BREAKS ~

Q205=0, MIN. PLUNGING DEPTH ~

Q211=0, DWELL TIME AT BOTTOM ~

Q208=0, FEED RATE REVERSE ~

Q256=0.25 REV BREAKS

19 L X-76,523 Y+49,231 R FMAX M

20 L Z+10, R FMAX M99

 

Claus@cimco

[pip]

We have had this problem intermitently, with our Heidenhain 430 controll. Because it was intermitent, we have not been able to track it down.

Sorry cant help you, but you are not alone.

[Guest CNC Apps Guy 1]

The problem is that your control is a Heidenhein. Throw it out and get a Fanuc.

 

But seriously, if the problem has just recently appeared and you recently made some post modifications, that would be the first place I would look. Double check what you modified and look for the obvious stuff first like maybe you forgot, to add a "," after a call, or as was stated earlier make sure you have the "~" character where it is required. Make sure all of your quotes are closed. Make sure you did not accidently put a carriage return before a "#" breaking up a postblock, etc...

 

JM2C

[Claus@Cimco]

James

 

How do you turn the coordinate system on a Fanuc? ;-)

 

10 CYCL DEF 19.0 WORKING PLANE

11 CYCL DEF 19.1 A+24,814 B+0, C-35,417 F9999

 

Fanucs are Ok and 15i/16i are fast, but Heidenhains are not that bad, but you have to learn a different language. It's like here, I prefere to write in Danish, but you guys wouldn't understand a word, eller tager jeg fejl.

 

Claus@Cimco

 

[ 03-22-2002, 11:15 AM: Message edited by: Claus@Cimco ]

[cadcam]

quote:

---

eller tager jeg fejl.

---

What you say?

 

[ 03-22-2002, 11:29 AM: Message edited by: cadcam ]

[Claus@Cimco]

eller tager jeg fejl -> or am I wrong

Claus@cimco

[Jim Evans from CNC Software]

Bruce,

 

If this is a problem that just started after making modifications to the post, you should back track your changes and check all your syntax. I'm willing to bet it's something simple associated with the cahnges you made to the post.

 

Jim

[Christian Raebild]

IIRC, the Q### line after a line ending with a "~" must start with one or more space characters (ASCII 32). When I write post processors for Heidenhain controls, I use three space characters. You should also remember, that the last Q### line describing the cycle must not have a "~" character at the end of the line.

[Bruce]

Thanks for all the replies but as yet no success.

I ran the original post and got the same result, therefore this error has always been in the post, or the controller is unable accept the 203 drilling cycle, other than if you program via the machine. I hadn’t noticed this fault/error before, as I had not run that cycle with this post before.

Are there any “post editors” on this forum operating out of Brisbane Australia? If so it might time to make contact.

[Christian Raebild]

Copenhagen is pretty far from Brisbane, so a personal visit from me is unlikely, but I do know Heidenhain controls fairly well. If cycle 203 works on the control, then it should also work from the post processor. If you can post a sample of the output from the post processor, then I can most likely see what is wrong with the output from the post processor.

[Bruce]

Christian

 

The first two sample programs show the output from two different posts as seen in the text editor, the third program is what they both look like, once downloaded to the machine.

Note the comment marks " ; " in line 7 & 8 of the third progam. It is these that I can only remove by deleting the whole line, which kills the drill cycle.

 

0 BEGIN PGM PTEST MM

1 BLK FORM 0.1 Z X.00 Y.00 Z-25.00

2 BLK FORM 0.2 X300.00 Y200.00 Z.00

3 TOOL DEF 3 L+0 R6.00

4 TOOL CALL 3 Z S1909

5 L M6

6 ;12. DRILL

7 CYCL DEF 203 UNIVERSL DRILLNG

Q200=-5 Q201=-28.605 Q206=458.16 Q202=10 Q210=25 Q203=0 Q204=5 Q212=3 Q213=2 Q205=3 Q211=25 Q208=0

8 L X200.00 Y144.00 R0 FMAX M3

9 L Z5.00 FMAX

10 L Z5.00 FMAX M99

11 L X150.00 Y94.00 FMAX M99

12 L X200.00 Y44.00 FMAX M99

13 L Z5.00 FMAX

14 M25

15 END PGM PTEST MM

 

0 BEGIN PGM PTEST MM

1 BLK FORM 0.1 Z X.00 Y.00 Z-25.00

2 BLK FORM 0.2 X300.00 Y200.00 Z.00

3 TOOL DEF 3 L+0 R6.00

4 TOOL CALL 3 Z S1909

5 L M6

6 ;12. DRILL

7 CYCL DEF 203 UNIVERSL DRILLNG

Q200=-5

Q201=-28.605

Q206=458.16

Q202=10

Q210=25

Q203=0

Q204=5

Q212=3

Q213=2

Q205=3

Q211=25

Q208=0

8 L X200.00 Y144.00 R0 FMAX M3

9 L Z5.00 FMAX

10 L Z5.00 FMAX M99

11 L X150.00 Y94.00 FMAX M99

12 L X200.00 Y44.00 FMAX M99

13 L Z5.00 FMAX

14 M25

15 END PGM PTEST MM

 

0 BEGIN PGM PTEST MM

1 BLK FORM 0.1 Z X+0 Y+0 Z-25

2 BLK FORM 0.2 X+300 Y+200 Z+0

3 TOOL DEF 3 L+0 R+6

4 TOOL CALL 3 Z S1909

5 L M6

6 ;12. DRILL

7 ; CYCLDEF203UNIVERSLDRILLNG

8 ; Q200=-5Q201=-28.605Q206=458.16Q202=10Q210=25Q203=0Q204=

9 L X+200 Y+144 R0 FMAX M3

10 L Z+5 FMAX

11 L Z+5 FMAX M99

12 L X+150 Y+94 FMAX M99

13 L X+200 Y+44 FMAX M99

14 L Z+5 FMAX

15 M25

16 END PGM PTEST MM