5 axis drill changing feeds

[[email protected]]

I was using 5 axis drill to hit 3 sides of a part but when it goes to the back side it uses the feeds from the tool definition instead of the ones i defined in paramaters. This is weird because the first two sides of part it does use my defined feed from paramaters. I just changed the tool definitions feed to match for my tap but why is this happening? my tool settings under machine group always has feed calculation "from tool" checked but it only reads what i have defined in paramaters. Please shed some light on this I suddenly feel like a newbie

T4 M6
S3800 M3
G0 G54 G90 X.9005 Y-5.0125 B180. A-90.
T5
G43 H4 Z8.911 /M8
G81 G98 Z2.096 R2.311 F8.
X.2755 Y-5.2675
X-.9305 Y-5.0125
X-1.0255 Y1.563 Z5.554 A0. R5.769
X1.0255
Y-1.563
X-1.0255
G80
Z14.369
B0. A-90.
X.9305 Y-5.0125
Z8.911
G81 G98 Z2.096 R2.311 F25.
X-.2755 Y-5.2675
X-.9005 Y-5.0125 F8.
G80
M9
M5
G0 G28 G91 Z0.
M01


(NO. 17 DRILL FOR 8-32 STI CUT TAP)
(PECKS 8-32 STI HOLES)
T5 M6
S3400 M3
G0 G54 G90 X.9005 Y-5.0125 B180. A-90.
T6
G43 H5 Z8.796 /M8
G83 G98 Z1.734 R2.196 Q.05 F8.
X.2755 Y-5.2675
X-.9305 Y-5.0125
X1.0255 Y1.563 Z5.192 A0. R5.654
X-1.0255
X1.0255 Y-1.563
X-1.0255
G80
Z14.254
B0. A-90.
X-.9005 Y-5.0125
Z8.796
G83 G98 Z1.734 R2.196 Q.05 F4.2
X-.2755 Y-5.2675
X.9305 Y-5.0125 F8.
G80
M9
M5
G0 G28 G91 Z0.
M01


(NO. 8-32 STI CUT TAPRH)
(TAPS 8-32 STI HOLES)
T6 M6
S320 M3
G0 G54 G90 X.9005 Y-5.0125 B180. A-90.
T4
G43 H6 Z8.911 /M8
G84 G98 Z1.846 R2.311 F10.
X.2755 Y-5.2675
X-.9305 Y-5.0125
X-1.0255 Y1.563 Z5.304 A0. R5.769
X1.0255
Y-1.563
X-1.0255
G80
Z14.369
B0. A-90.
X.9305 Y-5.0125
Z8.911
G84 G98 Z1.846 R2.311 F10.
X-.2755 Y-5.2675
X-.9005 Y-5.0125
G80
M9
M5
G0 G28 G91 Z0.
G0 G28 Y0.
G90 A0. B0.
M30

[crazy^millman]

Going to need to see a file to even think about how I can answer this question. No I have not see it if that all you're asking.

[[email protected]]

here you go thanks!

5_AXIS_DRILL.ZIP

[crazy^millman]

37 minutes ago, [email protected] said:

here you go thanks!

5_AXIS_DRILL.ZIP

Took the generic HAAS VF-TR Post and got good code. Need to go back to your reseller and ask them to figure out what is going on with that post.

%
O0000
(D3764295-99)
(DATE=DD-MM-YY - 17-06-21 TIME=HH:MM - 13:53)
(MCX FILE - C:\USERS\RON\DOCUMENTS\MY MASTERCAM 2021\MASTERCAM\PARTS\5_AXIS_DRI)
(NC FILE - C:\USERS\RON\DOCUMENTS\MY MCAM2019\MILL\NC\D3764295-99.NC)
(MATERIAL - ALUMINUM INCH - 2024)
.
.
.
.

(1/4 SPOT DRILL 120 DEGREE EFH 1.0|TOOL - 4|DIA. OFF. - 4|LEN. - 4| DIA. - .25)
(SPOTS 8-32 STI HOLES)
M11
M13
T4 M6
G187 P3 E.001
G0 G54 G90 X.9005 Y-5.0125 B180. A90. S3800 M3
M10
M12
G43 H4 Z8.911 M8
G81 G98 Z2.096 R2.311 F8.
X.2755 Y-5.2675
X-.9305 Y-5.0125
M11
X-1.0255 Y1.563 Z5.554 A0. R5.769
M10
X1.0255
Y-1.563
X-1.0255
M11
X-.9305 Y5.0125 Z2.096 A-90. R2.311
M10
X.2755 Y5.2675
X.9005 Y5.0125
G80
M9
M5
G0 G28 G91 Z0.
M01
G0 G17 G40 G80 G90 G94 G98
G0 G28 G91 Z0.
(NO. 17 DRILL FOR 8-32 STI CUT TAP|TOOL - 5|DIA. OFF. - 5|LEN. - 5| DIA. - .173)
(PECKS 8-32 STI HOLES)
M11
M13
T5 M6
G187 P3 E.001
G0 G54 G90 X.9005 Y-5.0125 B180. A90. S3400 M3
M10
M12
G43 H5 Z8.796 M8
G83 G98 Z1.734 R2.196 Q.05 F8.
X.2755 Y-5.2675
X-.9305 Y-5.0125
M11
X1.0255 Y1.563 Z5.192 A0. R5.654
M10
X-1.0255
X1.0255 Y-1.563
X-1.0255
M11
X.9005 Y5.0125 Z1.734 A-90. R2.196
M10
X.2755 Y5.2675
X-.9305 Y5.0125
G80
M9
M5
G0 G28 G91 Z0.
M01
G0 G17 G40 G80 G90 G94 G98
G0 G28 G91 Z0.
(NO. 8-32 STI CUT TAPRH|TOOL - 6|DIA. OFF. - 6|LEN. - 6| DIA. - .164)
(TAPS 8-32 STI HOLES)
M11
M13
T6 M6
G187 P3 E.001
G0 G54 G90 X.9005 Y-5.0125 B180. A90. S320 M3
M10
M12
G43 H6 Z8.911 M8
G84 G98 Z1.846 R2.311 F10.
X.2755 Y-5.2675
X-.9305 Y-5.0125
M11
X-1.0255 Y1.563 Z5.304 A0. R5.769
M10
X1.0255
Y-1.563
X-1.0255
M11
X-.9305 Y5.0125 Z1.846 A-90. R2.311
M10
X.2755 Y5.2675
X.9005 Y5.0125
G80
M9
M5
G0 G28 G91 Z0.
M01
G0 G17 G40 G80 G90 G94 G98
G0 G28 G91 Z0.

 

[Colin Gilchrist]

So, your error is coming from a "feature" in the Post. (Could be a bug, depends on your point-of-view).

There is a section of code in the Post, which allows you to override the Feed value. This is used "internally" in the Binned portion of the Post Processor, for feed calculations.

The issue is this: When 'Cut Flag = 7', the Post is overriding the value of 'fr_pos$' with the Plunge Feedrate.

So it isn't actually "reading your Tool Defintion"; the issue is that you've got a Plunge Feedrate assigned to the two Drill Ops, where the Plunge Feed is different from the Cut Feed values.

pfd_shft_ovrd   #Overide prior to shift and feed calculation
      if cutflag = 7,
        [
        !fr_pos$
        fr_pos$ = plunge_feed
        ]

That is the code in your Post where this value is being overwritten.

I fixed the issue by opening each of your Tool Definitions, and setting the Cut Feed and Plunge Feed to be equal. I then "Right-clicked" on the Tool Definition, and chose the option for "re-initialize Feed/Speed", and this set the Plunge Values equal to the Cut Feed.

[IGNORE THE 'DEBUG' output. That was just for my testing purposes...]

 

( T4 1/4 SPOT DRILL 120 DEGREE EFH 1.0 )
( T5 NO. 17 DRILL FOR 8-32 STI CUT TAP )
( T6 NO. 8-32 STI CUT TAPRH )
G20
G0 G17 G40 G49 G80 G90
G0 G28 G91 Z0.
(1/4 SPOT DRILL 120 DEGREE EFH 1.0)
(SPOTS 8-32 STI HOLES)

T4 M6
S3800 M3
G0 G54 G90 X.9005 Y-5.0125 B180. A-90.
T5
G43 H4 Z8.911 /M8
DEBUG FEED:  fr_pos$ 8.
G81 G98 Z2.096 R2.311 F8.
DEBUG FEED:  fr_pos$ 8.
X.2755 Y-5.2675
DEBUG FEED:  fr_pos$ 8.
X-.9305 Y-5.0125
DEBUG FEED:  fr_pos$ 8.
X-1.0255 Y1.563 Z5.554 A0. R5.769
DEBUG FEED:  fr_pos$ 8.
X1.0255
DEBUG FEED:  fr_pos$ 8.
Y-1.563
DEBUG FEED:  fr_pos$ 8.
X-1.0255
G80
Z14.369
B0. A-90.
X.9305 Y-5.0125
Z8.911
DEBUG FEED:  fr_pos$ 8.
G81 G98 Z2.096 R2.311 F8.
DEBUG FEED:  fr_pos$ 8.
X-.2755 Y-5.2675
DEBUG FEED:  fr_pos$ 8.
X-.9005 Y-5.0125
G80
M9
M5
G0 G28 G91 Z0.
M01


(NO. 17 DRILL FOR 8-32 STI CUT TAP)
(PECKS 8-32 STI HOLES)
T5 M6
S3400 M3
G0 G54 G90 X.9005 Y-5.0125 B180. A-90.
T6
G43 H5 Z8.796 /M8
DEBUG FEED:  fr_pos$ 8.
G83 G98 Z1.734 R2.196 Q.05 F8.
DEBUG FEED:  fr_pos$ 8.
X.2755 Y-5.2675
DEBUG FEED:  fr_pos$ 8.
X-.9305 Y-5.0125
DEBUG FEED:  fr_pos$ 8.
X1.0255 Y1.563 Z5.192 A0. R5.654
DEBUG FEED:  fr_pos$ 8.
X-1.0255
DEBUG FEED:  fr_pos$ 8.
X1.0255 Y-1.563
DEBUG FEED:  fr_pos$ 8.
X-1.0255
G80
Z14.254
B0. A-90.
X-.9005 Y-5.0125
Z8.796
DEBUG FEED:  fr_pos$ 8.
G83 G98 Z1.734 R2.196 Q.05 F8.
DEBUG FEED:  fr_pos$ 8.
X-.2755 Y-5.2675
DEBUG FEED:  fr_pos$ 8.
X.9305 Y-5.0125
G80
M9
M5
G0 G28 G91 Z0.
M01


(NO. 8-32 STI CUT TAPRH)
(TAPS 8-32 STI HOLES)
T6 M6
S320 M3
G0 G54 G90 X.9005 Y-5.0125 B180. A-90.
T4
G43 H6 Z8.911 /M8
DEBUG FEED:  fr_pos$ 10.
G84 G98 Z1.846 R2.311 F10.
DEBUG FEED:  fr_pos$ 10.
X.2755 Y-5.2675
DEBUG FEED:  fr_pos$ 10.
X-.9305 Y-5.0125
DEBUG FEED:  fr_pos$ 10.
X-1.0255 Y1.563 Z5.304 A0. R5.769
DEBUG FEED:  fr_pos$ 10.
X1.0255
DEBUG FEED:  fr_pos$ 10.
Y-1.563
DEBUG FEED:  fr_pos$ 10.
X-1.0255
G80
Z14.369
B0. A-90.
X.9305 Y-5.0125
Z8.911
DEBUG FEED:  fr_pos$ 10.
G84 G98 Z1.846 R2.311 F10.
DEBUG FEED:  fr_pos$ 10.
X-.2755 Y-5.2675
DEBUG FEED:  fr_pos$ 10.
X-.9005 Y-5.0125
G80
M9
M5
G0 G28 G91 Z0.
G0 G28 Y0.
G90 A0. B0.
M30
%

 

[[email protected]]

Thank you Colin and Millman! I was happy to learn it was originating from the post but then to learn how and why is even better. Can't thank you guys enough!