Missing feed rate in NC file

[bogusmill]

Using MCX5 on 5 axis parts for the first time. Post is Generic HAAS VF-TR series 5Xmill.pst with VF-2 & a TC-5 head. I have been running for a day & 1/2 just fine then today a new toolpath comes to a stop because of no feedrate output. It's a 5ax flow path, I will paste the code below but the feed callout is missing on line 138, just before going to inverse time. What can be changed to correct this?

 

%

O0001 ( PROGRAM - 09-0128-0400-03-AJPL10039 )

N100 ( DATE - 04-01-11 TIME - 10:35 )

N102 G20

N104 G0 G17 G40 G49 G80 G90

N106 G0 G28 G91 Z0.

N108 ( .030C BALL STUB TOOL - 12 DIA. OFF. - 12 LEN. - 12 DIA. - .03 )

N110 M11

N112 M13

N114 T12 M6

N116 G0 G54 G90 X-.0038 Y-5.1161 B97.995 A69.475 S7500 M3

N118 G43 H12 Z2.2129 M8

N120 Z2.0629

N122 G1 X-.0015 Y-5.1339 Z1.9646 F10.

N124 G0 Z2.0629

N126 X-.0039 Y-5.1161

N128 Z2.2129

N130 Z2.2308

N132 X-.016 Y-5.1361

N134 B97.659 A69.291

N136 Z2.0808

N138 G1 X-.0154 Y-5.13 Z1.9809

N140 G93 X-.0147 Y-5.1304 Z1.9795 B97.689 A69.307 F999.99

N142 X-.0126 Y-5.1314 Z1.9758 B97.766 A69.35 F976.58

N144 X-.0106 Y-5.1322 Z1.9725 B97.833 A69.386 F976.31

[gcode]

do a search for "F0".. this problem came up in the last week or so .. and a solution was posted by CNC Software

[spade117]

do a search for "F0".. this problem came up in the last week or so .. and a solution was posted by CNC Software

No results come up for that term.

[gcode]

a search for "inverse time" found it

 

F0 with Haas 5X post

 

hope it helps

[Mr. Wizzard]

shouldn't it default to the last IPM feedrate on line #122 as F10. ?

The G93 doesn't come on till line #140, so it would be IPM until that happens.

I'm just guessing, i'm not a pro...

[gcode]

Mr Wizzard is right.. that code should run .. though there should be a the safety block

[bogusmill]

That's what I was thinking too but somehow the machine knew different & the only way I can win a disaggrement with it is to cheat & lie.

[gcode]

Will it run right if you put a G94 in N116

 

 

[bogusmill]

Yes, G94 right beside G90 and it runs. So how do I get it there with the post?

[gcode]

try putting *sgfeed, in your saftey block line.

 

ptlchg$ #Tool change

#Cancel check in case missed in ptoolend

if prv_n_tpln_mch <> n_tpln_mch, pg69

 

##### Custom changes allowed below #####

 

pbld, n$, "M01", e$

pbld, n$, *sg00, *sgplane, *sg40, "G80", *sg90, *sgfeed, *sg98, e$

 

 

[bogusmill]

No good, what you suggest is exactly how my post reads now.

[Mr. Wizzard]

T1 M06 (.750 X 1.625 LOC ONSRUD )

(MAX - Z2.)

(MIN - Z0.)

G00 G17 G90 G54 X-2.825 Y1.8124 S5900 M03

G43 H1 Z2.

Z.15

G94 G01 Z0. F85.

X2.45

G02 X2.6148 Y1.6476 I0. J-.1648

 

I'm not sure why or where it is in the post, but I am using a tweaked MPMaster for my Tm-2 with a 4th axis and the G94 is forced out when there isn't a G93 in the feedrate. This sample comes out in the first feedrate movement, but sometimes it comes out on a line by itself directly below the G43.

[Mr. Wizzard]

any luck so far, Bogus?

[bogusmill]

any luck so far, Bogus?

 

Not yet, been playing with the post debugger though but too much going on to concentrate on it.

[Mr. Wizzard]

Not necessarily what you would want to do, but i messed with the post you are using and placed a * before all the sgfeed calls it gave me "G94" on every line of code that was a feed move. I don't have any inverse time feedrates in the program i was using, but assume it would do the same.

I'm not post expert, but I'm trying to find why the MPMaster outputs it only when necessary and see if those lines can be added to the 5-axis post. One thing i'm not sure of is the .psb file. The .psb file is the encrypted part of the post that "we" can't mess with. There may be something in there that triggers it.

[bogusmill]

I had the exact same code that Gcode said I should. So what did you change to get the G94 to post at every line with a feed. Cant I have it force an Feedrate at every line with a G01?

[Mr. Wizzard]

Please use caution with this because I am NOT a post expert! I would definitely recommend checking with someone who knows more than I do.

What i did was search the post for all "sgfeed" calls. I think there was only 3 or so in the .pst file. This leads me to believe there are more in the .psb file, since the MPMaster I'm using for my TM-2 has many, many more called in the post.

________Back up the post first, or save a copy in another folder before you mess with it, though!________

I replaced the "sgfeed" and "`sgfeed" calls with "*sgfeed" and it forced the G94 to be output on every feed line. My program did not have any inverse feedrates in it, so I had no G93 feedrates come out. Double check to see that you get the correct (G93 or G94) output on the correct lines.

Again, please note, this is only a guess and I cannot guarantee this will not mess things up with your post. I'm trying to help, but please verify this with someone who knows posts.

By default the Haas machine is in G94 mode. The MPMaster from Mastercam posts out a G94 after my tool changes if the feed moves are IPM and G93 if inverse. I think Mastercam would be able to add this logic to the post you are using since they are supplied with the software.

 

Another thought,......

Your program begins in G94 and switches to G93 without a toolchange. What Gcode suggested would work on a toolchange, but yours is changing on a null toolchange. Maybe before trying my suggestion, try what Gcode suggested, but make the changes in the tool change and null tool change sections of your post.

I hope something works out for you. The post stuff has been confusing to me, but it's one of those things I'm determined to figure out. I can't stand being stumped on things....

[bogusmill]

I like to figure these things out too but sometimes there just isn't enough hours in the day. I know the most about computers & software here so I am the guinea pig when new software is installed. I have to get mine working first so the others don't encounter problems.

 

Your last post says you replaced sgfeed with sgfeed? Your replaced a word with the same word and now it works?

[Mr. Wizzard]

No, you have to have it read *sgfeed with the asterisk * in front. That forces output of the feed code (G93 or G94) instead of only outputting it when it changes.

[bogusmill]

I will try that & let you know.