[IlFincoITA]

Hi! I'm trying to edit an old .GPP file for a deckel Fp4MA. Everithing is working just fime but since this machine need that z compensation must be wrote after any z changes i've discovered a mistake. It puts the D+ code after Z changes but it does this change aven after a x or y change and i can't discover where is the problem into the .GPP file. Could someone check this .GPP file? Thanks a lot...

[G00Z0]

Hi,
would you like to give a short example where I can see the NC code directly from the actual GPP file.
Please mark the mistakes or how it should work correctly.

Sorry, I didn't open the attached picture.

I will have a look.

[G00Z0]

Try this:

{[' X'xpos], [' Y'ypos], [' Z'zpos,' D+'tool_number]} <- insert here
if save_feed <> feed or change(feed) then
m_feed_flag = true
endif
if m_feed_flag eq true then
m_feed_flag = false
{' F',feed,' D+'tool_number} <- delete this

[IlFincoITA]

OK I have solved that part in this way:

if m_feed_flag eq true then
m_feed_flag = false
{' D+'tool_number' F',feed} <== putting ' D+'tool_number just befor ' F'

Now the problem comes here

@move_xy

gcode = 0

if first_rapid_move eq true then
{nb,'G'gcode,[' X'xpos], [' Y'ypos]}
call @start_tool
{' M08'}
{nb,'G'gcode,[' Z'zpos],' D+'tool_number}
first_rapid_move = false
else
{nb,'G'gcode [' X'xpos], [' Y'ypos], [' Z'zpos],' D+'tool_number} <===i've put the compensation here!
endif

endp

This works but effect X and Y too... besides Z must be in a new block lonely with d+ compensation.
Her's what I get:

N0010 G00 X-163400 Y+22510 S+2000 M08
N0020 G00 Z+10000 D+01 <== Good Here
N0030 G00 Z+2000 D+01 <== Good Here
N0040 G01 Z-25500 D+01 F500
N0050 G02 X-152470 Y+34400 I+36400 J-22510 F1000
N0060 G02 X-152040 Y+34600 I+730 J-980
N0070 G01 X-143720 Y+36700
N0080 G02 X-142910 Y+34400 I+300 J-1190
N0090 G03 X-163400 Y+10560 I+15910 J-34400
N0100 G00 Z+10000 D+01 <== Good Here
N0110 G00 Y-22510 D+01 <== BAD HERE
N0120 G00 Z+2000 D+01 <== Good Here
N0130 G01 Z-25500 D+01 F500

I've tryed to but D+ inside [' Z'zpos] but it mess up the things too:

N0010 G00 X-163400 Y+22510 S+2000 M08
N0020 G00 Z+10000 D+01
N0030 G00 Z+2000 D+01
N0040 G01 Z-25500 D+01 F500
N0050 G02 X-152470 Y+34400 I+36400 J-22510 F1000
N0060 G02 X-152040 Y+34600 I+730 J-980
N0070 G01 X-143720 Y+36700
N0080 G02 X-142910 Y+34400 I+300 J-1190
N0090 G03 X-163400 Y+10560 I+15910 J-34400
N0100 G00 Z+10000 D+01
N0110 G00 Y-22510 Z+10000 D+01 <== It goes with Z but move Z into Y line
N0120 G00 Z+2000 D+01
N0130 G01 Z-25500 D+01 F500

Anyone hase a solution please... thanks a lot...

[G00Z0]

N0110 G00 Y-22510 Z+10000 D+01 <== It goes with Z but move Z into Y line

Is this the only mistake ? When "yes", you have to set a flag for the "D+01" output. Is it so ? Every sentence with single axis output in Z must have the "D+01" ?

Try something like that:

if ( (change(xpos) eq false) and (change(ypos) eq false) and (change(zpos) eq true) then
{'D+',tool_number}
endif

[IlFincoITA]

Is this the only mistake ? When "yes", you have to set a flag for the "D+01" output. Is it so ? Every sentence with single axis output in Z must have the "D+01" ?

Try something like that:

if ( (change(xpos) eq false) and (change(ypos) eq false) and (change(zpos) eq true) then
{'D+',tool_number}
endif

GREAT! IT HELPS ME THANKS A LOT

[IlFincoITA]

GREAT! IT HELPS ME THANKS A LOT

[IlFincoITA]

Hi! It is a last thing that i don't understand...

@call_proc
integer_def_f = BLKNUM_F

{nb,'L1 N*'start_line}
{' N*'end_line}


integer_def_f = INTEGER_DEF_F
endp

this suppose to repeat blocks of program.... but it doesn't work. I didn't see any repetition in my generated G code. What is activating this procedure? I've seen in .MAC file that "loop_exist = Y".

[G00Z0]

This section is important if you use subprograms.

look at this lines in *.MAC:

gen_procs = N
gen_internal_proc = Y

[IlFincoITA]

Hi! I've check it out and the setting are as you wrote in .MAC file but still no L01 repetition in my G Code...

It suppose to generate something like this:

N0481 L01 N0081 N0401

Is there any setting that I must flag into solidcam operation idalog boxes or general machine setting... I can't figure out what it is?

[G00Z0]

Do you want to get sub programs or not ?

If not, just write

gen_internal_proc = N

in the *.MAC

If "yes", why ?

[IlFincoITA]

Of course I want to use subprogram... the memory on FP4MA is very small... I need to short the program as much as possible.

I mean sub program is when a piece of program is repeated inside the main program... for example a toolpath that is equal but has a different Z depth: Because what I see is that Solidcam generates the full G code repeating the complete toolpath aven wen it is the same ad the only thig different is the Z depth. That wath I need to avoid...

You see (this is generated with gen_internal_proc = Y) :

N0010 G00 X-129500 Y+0 S+1000 M08
N0020 G00 Z+10000 D+05
N0030 G00 Z+1000 D+05
N0040 G01 Z-6000 D+05 F33
N0050 G01 Y-5500 F100
N0060 G03 X-129500 Y-5500 I+0 J+5500
N0070 G01 Y+0
N0080 G01 Z-11000 D+05 F33
N0090 G01 Y-5500 F100
N0100 G03 X-129500 Y-5500 I+0 J+5500
N0110 G01 Y+0
N0120 G01 Z-16000 D+05 F33
N0130 G01 Y-5500 F100
N0140 G03 X-129500 Y-5500 I+0 J+5500
N0150 G01 Y+0
N0160 G01 Z-21000 D+05 F33
N0170 G01 Y-5500 F100
N0180 G03 X-129500 Y-5500 I+0 J+5500
N0190 G01 Y+0
N0200 G01 Z-22000 D+05 F33
N0210 G01 Y-5500 F100
N0220 G03 X-129500 Y-5500 I+0 J+5500
N0230 G01 Y+0
N0240 G00 Z+10000 D+05

[G00Z0]

So is your sequence in *.MAC:
gen_internal_proc = Y

Then in *.GPP you need the sections:


@proc -> this calls the sub programm in main programm
@call_proc -> start sequence from sub program
@end_proc -> end sequence from sub program

Where is still your problem ?

[IlFincoITA]

In my .GPP I only find...

@call_proc
integer_def_f = BLKNUM_F

{nb,'L1 N*'start_line}
{' N*'end_line}


integer_def_f = INTEGER_DEF_F
endp


@proc
flag_start_job = true
endp

What is wrong is this

N0080 G01 Z-11000 D+05 F33
N0090 G01 Y-5500 F100
N0100 G03 X-129500 Y-5500 I+0 J+5500
N0110 G01 Y+0
N0120 G01 Z-16000 D+05 F33
N0130 G01 Y-5500 F100--------------------------------->This is a repetiion
N0140 G03 X-129500 Y-5500 I+0 J+5500----------->This is a repetition
N0150 G01 Y+0
N0160 G01 Z-21000 D+05 F33
N0170 G01 Y-5500 F100--------------------------------->This is a repetiion
N0180 G03 X-129500 Y-5500 I+0 J+5500----------->This is a repetiion
N0190 G01 Y+0
N0200 G01 Z-22000 D+05 F33
N0210 G01 Y-5500 F100--------------------------------->This is a repetiion
N0220 G03 X-129500 Y-5500 I+0 J+5500----------->This is a repetiion
N0230 G01 Y+0

Why it doesn't writhe those blocks under
L01

Like this

N0200 G01 Z-22000 D+05 F33
N0201 L01 N0170 N0190

and so on...

See attached file...

[G00Z0]

I think at this point I have to see the PP.
If you would mind, send me the *.GPP and *.MAC and I will have look.

[IlFincoITA]

You're so kind... here it is...

[IlFincoITA]

You're so kind... here it is...

I'm sorry I did a mistake... don't which file a was looking at but after a double check i found

gen_internal_proc = Y was set to N

Now I've chage it and everything is just fine.

Sorry to have bother you guys out there... you have helped me a lot...

[G00Z0]

Everything is fine now ?
The thread is closed ?

Thanks for the conversation,

Bye

[IlFincoITA]

I'm trying the G Code this morning... i'll confirm that everithig is OK within today...

Thnaks a lot...

[IlFincoITA]

Nope there is still onothe issue. The line after L01 mess up the Z this is a simple program:

;SPALLA ALBERO MOTORE
;
%
(&P01/0000)
T07
;
; Fresa Piatta Ø14 mm.
;
; --------------------
;
; F-CONTOUR7 - PROFILE
;
; --------------------
;
N0010 G00 X-129500 Y+0 S+1250 M08
N0020 G00 Z+10000 D+07
N0030 G00 Z+2000 D+07
N0040 G01 Z-7000 D+07 F500
N0050 L01 N0180 N0220
N0060 G01 X-129500 Y+0 Z-14000 D+07 F500 ========>Z must go into a separate block
N0070 L01 N0180 N0220
N0080 G01 X-129500 Y+0 Z-18500 D+07 F500========>Z must go into a separate block
N0090 L01 N0180 N0220
N0100 G01 X-129500 Y+0 Z-19000 D+07 F500========>Z must go into a separate block
N0110 L01 N0180 N0220
N0120 G00 X-129500 Y+0 Z-19000========>Z must go into a separate block ==>Where is Dz Compensation?
N0130 L01 N0230 N0270
N0140 G00 X-129500 Y+0 Z+10000========>Z must go into a separate block==>Where is Dz Compensation?
N0150 M09
N0160 G00 Z+150000 D+07
N0170 M30
N0180 F750
N0190 G41 D+57 G47 A+1000 X-129500 Y-17000 G01 G60 M61
N0200 G03 X-129500 Y-17000 I+0 J+17000 F750
N0210 G40 D+57 G47 A+1000
N0220 G01 Y+0
N0230 F750
N0240 G41 D+57 G47 A+1000 X-129500 Y-17500 G01 G60 M61
N0250 G03 X-129500 Y-17500 I+0 J+17500
N0260 G40 D+57 G47 A+1000
N0270 G01 Y+0
?
0000