[Jamespvill]

Hello Gentlemen,

I'm having some issues with figuring out how to get mach 3 and bobcad to play nicely when it comes to tool offsets...

I have a series of 3 endmills I want to use; Rougher, finish, finish. Of course each is a different height and I can't figure out how to offset them properly then have Mach know their heights. I've added the tool heights in the "Offsets" tab on Mach, but when I run the code Mach doesn't switch tools after my roughing operation.

I'm assuming I need to tinker with something in BobCad but don't know where to go.

Thanks folks!
James

[KSky]

Hello Gentlemen,

I'm having some issues with figuring out how to get mach 3 and bobcad to play nicely when it comes to tool offsets...

I have a series of 3 endmills I want to use; Rougher, finish, finish. Of course each is a different height and I can't figure out how to offset them properly then have Mach know their heights. I've added the tool heights in the "Offsets" tab on Mach, but when I run the code Mach doesn't switch tools after my roughing operation.

I'm assuming I need to tinker with something in BobCad but don't know where to go.

Thanks folks!
James

Which post-processor are you using? Not all of the Mach3 ones do the G43 after the tool change. So for tool 5, apply the offset for tool 5.

T5 M6
G43 H5

[magicniner]

Set your Offsets for your tools in MACH-3, select the tool number in BobCAD.
I'm using the "Mach3 No ATC" post and that deals with the tool numbers,

- Nick

[Jamespvill]

I am using "Mach3-Mill-NoATC.MillPst".

I'm using TTS tooling and am measuring the tool height with a height gauge, then entering those into the Mach 3. In BobCad I'm using tools "1, 2, and 3". Which are the tools I want in Mach.

I suppose I am confused about how I should be entering the tool values and which tool I should be setting my Z zero.

[magicniner]

I have an edge finder with a spacer sleeve on the shank to give me a suitable fixed repeatable length which I use as to set my Z zero in Mach3, from there I can work out and enter the offsets for my other tools and enter them in the tool offsets table.
This will explain the rest better than I can -

Tool Change w/ Height Offset

Perhaps there's a good Mach3 Post out there that deals with the required H-word for the tool offset after the Work offset, (there really ought to be as BobCad are a Mach3 reseller) but you could easily edit your code to add in the Tool Offset H-Word,
Regards,
Nick

[Jamespvill]

Okay, So I have to manually edit the Gcode to tell specify that I want it to stop and change tools?

I realized that I need make all the offsets relative to my 0 tool (Duh...) So since my 0 tool is the longest, all of my others are the negative difference...Does that sound right?

I run into an issue when I zero my 0 tool in mach, then change to my 1 tool, at first it gives me the right offset, but as soon as I click Cycle start on mach, it changes my tool 1 to zero right away....Here is a quick example since a picture is worth a thousand words.

Here is the code itself, I'm not seeing anything to do with tool changes so I would guess that is the root of my problem.

(BEGIN PREDATOR NC HEADER)
(MACH_FILE=HAAS - 3XVMILL.MCH)
(MTOOL T1 S1 D.375 H2.5 A0. C0. DIAM_OFFSET 1 = .1875)
(MTOOL T2 S1 D.375 H2.5 A0. C0. DIAM_OFFSET 2 = .1875)
(SBOX X0. Y0. Z-2. L2. W2. H2.)
(END PREDATOR NC HEADER)

%
O100
(PROGRAM NUMBER)
(PROGRAM NAME - BIOHAZ.TAP)
(POST - MACH 3 MILL NO ATC)
(DATE - FRI. 01/02/2015)
(TIME - 01:28PM)

N01 G20 G40 G49 G54 G80 G90 G91.1
;N02 G53 Z0.

(Machine Setup - 1 Profile Rough)
(FEATURE 2 AXIS)

;N03 T1 M6
N04 S3000 M03
N05 G00 G90 G54 X.9271 Y2.2476
;N06 G43 H1 Z1. M08
N07 Z.2
N08 Z.1
N09 G01 Z-.25 F45.
N10 Y1.9976 F9.5
N11 G17 G03 X1.0755 Y1.9976 I.0742 J0.
N12 G01 Y2.2476
N13 G00 Z.2
N14 X.8463
N15 Z.1
N16 G01 Z-.25 F45.
N17 Y1.9976 F9.5
N18 G03 X1.1563 Y1.9976 I.155 J0.
N19 G01 Y2.2476
N20 G00 Z.2
N21 X.7655
N22 Z.1
N23 G01 Z-.25 F45.
N24 Y1.9976 F9.5
N25 G03 X1.2371 Y1.9976 I.2358 J0.
N26 G01 Y2.2476
N27 G00 Z.2
N28 X.6846
N29 Z.1
N30 G01 Z-.25 F45.
N31 Y1.9976 F9.5
N32 G03 X1.318 Y1.9976 I.3167 J0.
N33 G01 Y2.2476
N34 G00 Z.2
N35 X.6038
N36 Z.1
N37 G01 Z-.25 F45.
N38 Y1.9976 F9.5
N39 G03 X1.3988 Y1.9976 I.3975 J0.
N40 G01 Y2.2476
N41 G00 Z.2
N42 X2.2494 Y1.0734
N43 Z.1
N44 G01 Z-.25 F45.
N45 X1.9994 Y1.0737 F9.5
N46 G03 X1.9994 Y.9253 I-.0001 J-.0742
N47 G01 X2.2494 Y.9256
N48 G00 Z.2
N49 X2.2495 Y1.1542
N50 Z.1
N51 G01 Z-.25 F45.
N52 X1.9995 Y1.1545 F9.5
N53 G03 X1.9995 Y.8445 I-.0002 J-.155
N54 G01 X2.2495 Y.8448
N55 G00 Z.2
N56 X2.2496 Y1.235
N57 Z.1
N58 G01 Z-.25 F45.
N59 X1.9996 Y1.2353 F9.5
N60 G03 X1.9996 Y.7637 I-.0003 J-.2358
N61 G01 X2.2496 Y.764
N62 G00 Z.2
N63 X2.2497 Y1.3159
N64 Z.1
N65 G01 Z-.25 F45.
N66 X1.9997 Y1.3162 F9.5
N67 G03 X1.9997 Y.6828 I-.0004 J-.3167
N68 G01 X2.2497 Y.6831
N69 G00 Z.2
N70 X2.2498 Y1.3967
N71 Z.1
N72 G01 Z-.25 F45.
N73 X1.9998 Y1.397 F9.5
N74 G03 X1.9998 Y.602 I-.0005 J-.3975
N75 G01 X2.2498 Y.6023
N76 G00 Z.2
N77 X1.0755 Y-.25
N78 Z.1
N79 G01 Z-.25 F45.
N80 Y0. F9.5
N81 G03 X.9271 Y0. I-.0742 J0.
N82 G01 Y-.25
N83 G00 Z.2
N84 X1.1563
N85 Z.1
N86 G01 Z-.25 F45.
N87 Y0. F9.5
N88 G03 X.8463 Y0. I-.155 J0.
N89 G01 Y-.25
N90 G00 Z.2
N91 X1.2371
N92 Z.1
N93 G01 Z-.25 F45.
N94 Y0. F9.5
N95 G03 X.7655 Y0. I-.2358 J0.
N96 G01 Y-.25
N97 G00 Z.2
N98 X1.318
N99 Z.1
N100 G01 Z-.25 F45.
N101 Y0. F9.5
N102 G03 X.6846 Y0. I-.3167 J0.
N103 G01 Y-.25
N104 G00 Z.2
N105 X1.3988
N106 Z.1
N107 G01 Z-.25 F45.
N108 Y0. F9.5
N109 G03 X.6038 Y0. I-.3975 J0.
N110 G01 Y-.25
N111 G00 Z.2
N112 X-.25 Y.9253
N113 Z.1
N114 G01 Z-.25 F45.
N115 X0. F9.5
N116 G03 X0. Y1.0737 I0. J.0742
N117 G01 X-.25
N118 G00 Z.2
N119 Y.8445
N120 Z.1
N121 G01 Z-.25 F45.
N122 X0. F9.5
N123 G03 X0. Y1.1545 I0. J.155
N124 G01 X-.25
N125 G00 Z.2
N126 Y.7637
N127 Z.1
N128 G01 Z-.25 F45.
N129 X0. F9.5
N130 G03 X0. Y1.2353 I0. J.2358
N131 G01 X-.25
N132 G00 Z.2
N133 Y.6828
N134 Z.1
N135 G01 Z-.25 F45.
N136 X0. F9.5
N137 G03 X0. Y1.3162 I0. J.3167
N138 G01 X-.25
N139 G00 Z.2
N140 Y.602
N141 Z.1
N142 G01 Z-.25 F45.
N143 X0. F9.5
N144 G03 X0. Y1.397 I0. J.3975
N145 G01 X-.25
N146 G00 Z.2
N147 Z1.
N148 M09
N149 M05
;N150 G53 Z0.
;N151 G53 X0. Y0.
N152 M00

(Machine Setup - 1 Profile Finish)
(FEATURE 2 AXIS)

;N153 T2 M6
N154 S3000 M03
N155 G90 G54 X.8388 Y1.9976
;N156 G43 H2 Z1. M08
N157 G00 Z.2
N158 Z.1
N159 G01 Z-.25 F45.
N160 Y2.2476 F7.
N161 G17 G03 X.5888 Y1.9976 I0. J-.25
N162 X1.4138 Y1.9976 I.4125 J0.
N163 X1.1638 Y2.2476 I-.25 J0.
N164 G01 Y1.9976
N165 G00 Z.2
N166 X1.9995 Y1.162
N167 Z.1
N168 G01 Z-.25 F45.
N169 X2.2495 Y1.1617 F7.
N170 G03 X1.9998 Y1.412 I-.25 J.0003
N171 X1.9998 Y.587 I-.0005 J-.4125
N172 X2.2495 Y.8373 I-.0003 J.25
N173 G01 X1.9995 Y.837
N174 G00 Z.2
N175 X1.1638 Y0.
N176 Z.1
N177 G01 Z-.25 F45.
N178 Y-.25 F7.
N179 G03 X1.4138 Y0. I0. J.25
N180 X.5888 Y0. I-.4125 J0.
N181 X.8388 Y-.25 I.25 J0.
N182 G01 Y0.
N183 G00 Z.2
N184 X0. Y.837
N185 Z.1
N186 G01 Z-.25 F45.
N187 X-.25 F7.
N188 G03 X0. Y.587 I.25 J0.
N189 X0. Y1.412 I0. J.4125
N190 X-.25 Y1.162 I0. J-.25
N191 G01 X0.
N192 G00 Z.2
N193 Z1.
N194 M09
N195 M05
;N196 G53 Z0.
;N197 G53 Y0.
N198 M30

(END OF PROGRAM)
%

[fidia]

Okay, So I have to manually edit the Gcode to tell specify that I want it to stop and change tools?

I realized that I need make all the offsets relative to my 0 tool (Duh...) So since my 0 tool is the longest, all of my others are the negative difference...Does that sound right?

I run into an issue when I zero my 0 tool in mach, then change to my 1 tool, at first it gives me the right offset, but as soon as I click Cycle start on mach, it changes my tool 1 to zero right away....Here is a quick example since a picture is worth a thousand words.

Here is the code itself, I'm not seeing anything to do with tool changes so I would guess that is the root of my problem.

(BEGIN PREDATOR NC HEADER)
(MACH_FILE=HAAS - 3XVMILL.MCH)
(MTOOL T1 S1 D.375 H2.5 A0. C0. DIAM_OFFSET 1 = .1875)
(MTOOL T2 S1 D.375 H2.5 A0. C0. DIAM_OFFSET 2 = .1875)
(SBOX X0. Y0. Z-2. L2. W2. H2.)
(END PREDATOR NC HEADER)

%
O100
(PROGRAM NUMBER)
(PROGRAM NAME - BIOHAZ.TAP)
(POST - MACH 3 MILL NO ATC)
(DATE - FRI. 01/02/2015)
(TIME - 01:28PM)

N01 G20 G40 G49 G54 G80 G90 G91.1
;N02 G53 Z0.

(Machine Setup - 1 Profile Rough)
(FEATURE 2 AXIS)

;N03 T1 M6
N04 S3000 M03
N05 G00 G90 G54 X.9271 Y2.2476
;N06 G43 H1 Z1. M08
N07 Z.2
N08 Z.1
N09 G01 Z-.25 F45.
N10 Y1.9976 F9.5
N11 G17 G03 X1.0755 Y1.9976 I.0742 J0.
N12 G01 Y2.2476
N13 G00 Z.2
N14 X.8463
N15 Z.1
N16 G01 Z-.25 F45.
N17 Y1.9976 F9.5
N18 G03 X1.1563 Y1.9976 I.155 J0.
N19 G01 Y2.2476
N20 G00 Z.2
N21 X.7655
N22 Z.1
N23 G01 Z-.25 F45.
N24 Y1.9976 F9.5
N25 G03 X1.2371 Y1.9976 I.2358 J0.
N26 G01 Y2.2476
N27 G00 Z.2
N28 X.6846
N29 Z.1
N30 G01 Z-.25 F45.
N31 Y1.9976 F9.5
N32 G03 X1.318 Y1.9976 I.3167 J0.
N33 G01 Y2.2476
N34 G00 Z.2
N35 X.6038
N36 Z.1
N37 G01 Z-.25 F45.
N38 Y1.9976 F9.5
N39 G03 X1.3988 Y1.9976 I.3975 J0.
N40 G01 Y2.2476
N41 G00 Z.2
N42 X2.2494 Y1.0734
N43 Z.1
N44 G01 Z-.25 F45.
N45 X1.9994 Y1.0737 F9.5
N46 G03 X1.9994 Y.9253 I-.0001 J-.0742
N47 G01 X2.2494 Y.9256
N48 G00 Z.2
N49 X2.2495 Y1.1542
N50 Z.1
N51 G01 Z-.25 F45.
N52 X1.9995 Y1.1545 F9.5
N53 G03 X1.9995 Y.8445 I-.0002 J-.155
N54 G01 X2.2495 Y.8448
N55 G00 Z.2
N56 X2.2496 Y1.235
N57 Z.1
N58 G01 Z-.25 F45.
N59 X1.9996 Y1.2353 F9.5
N60 G03 X1.9996 Y.7637 I-.0003 J-.2358
N61 G01 X2.2496 Y.764
N62 G00 Z.2
N63 X2.2497 Y1.3159
N64 Z.1
N65 G01 Z-.25 F45.
N66 X1.9997 Y1.3162 F9.5
N67 G03 X1.9997 Y.6828 I-.0004 J-.3167
N68 G01 X2.2497 Y.6831
N69 G00 Z.2
N70 X2.2498 Y1.3967
N71 Z.1
N72 G01 Z-.25 F45.
N73 X1.9998 Y1.397 F9.5
N74 G03 X1.9998 Y.602 I-.0005 J-.3975
N75 G01 X2.2498 Y.6023
N76 G00 Z.2
N77 X1.0755 Y-.25
N78 Z.1
N79 G01 Z-.25 F45.
N80 Y0. F9.5
N81 G03 X.9271 Y0. I-.0742 J0.
N82 G01 Y-.25
N83 G00 Z.2
N84 X1.1563
N85 Z.1
N86 G01 Z-.25 F45.
N87 Y0. F9.5
N88 G03 X.8463 Y0. I-.155 J0.
N89 G01 Y-.25
N90 G00 Z.2
N91 X1.2371
N92 Z.1
N93 G01 Z-.25 F45.
N94 Y0. F9.5
N95 G03 X.7655 Y0. I-.2358 J0.
N96 G01 Y-.25
N97 G00 Z.2
N98 X1.318
N99 Z.1
N100 G01 Z-.25 F45.
N101 Y0. F9.5
N102 G03 X.6846 Y0. I-.3167 J0.
N103 G01 Y-.25
N104 G00 Z.2
N105 X1.3988
N106 Z.1
N107 G01 Z-.25 F45.
N108 Y0. F9.5
N109 G03 X.6038 Y0. I-.3975 J0.
N110 G01 Y-.25
N111 G00 Z.2
N112 X-.25 Y.9253
N113 Z.1
N114 G01 Z-.25 F45.
N115 X0. F9.5
N116 G03 X0. Y1.0737 I0. J.0742
N117 G01 X-.25
N118 G00 Z.2
N119 Y.8445
N120 Z.1
N121 G01 Z-.25 F45.
N122 X0. F9.5
N123 G03 X0. Y1.1545 I0. J.155
N124 G01 X-.25
N125 G00 Z.2
N126 Y.7637
N127 Z.1
N128 G01 Z-.25 F45.
N129 X0. F9.5
N130 G03 X0. Y1.2353 I0. J.2358
N131 G01 X-.25
N132 G00 Z.2
N133 Y.6828
N134 Z.1
N135 G01 Z-.25 F45.
N136 X0. F9.5
N137 G03 X0. Y1.3162 I0. J.3167
N138 G01 X-.25
N139 G00 Z.2
N140 Y.602
N141 Z.1
N142 G01 Z-.25 F45.
N143 X0. F9.5
N144 G03 X0. Y1.397 I0. J.3975
N145 G01 X-.25
N146 G00 Z.2
N147 Z1.
N148 M09
N149 M05
;N150 G53 Z0.
;N151 G53 X0. Y0.
N152 M00

(Machine Setup - 1 Profile Finish)
(FEATURE 2 AXIS)

;N153 T2 M6
N154 S3000 M03
N155 G90 G54 X.8388 Y1.9976
;N156 G43 H2 Z1. M08
N157 G00 Z.2
N158 Z.1
N159 G01 Z-.25 F45.
N160 Y2.2476 F7.
N161 G17 G03 X.5888 Y1.9976 I0. J-.25
N162 X1.4138 Y1.9976 I.4125 J0.
N163 X1.1638 Y2.2476 I-.25 J0.
N164 G01 Y1.9976
N165 G00 Z.2
N166 X1.9995 Y1.162
N167 Z.1
N168 G01 Z-.25 F45.
N169 X2.2495 Y1.1617 F7.
N170 G03 X1.9998 Y1.412 I-.25 J.0003
N171 X1.9998 Y.587 I-.0005 J-.4125
N172 X2.2495 Y.8373 I-.0003 J.25
N173 G01 X1.9995 Y.837
N174 G00 Z.2
N175 X1.1638 Y0.
N176 Z.1
N177 G01 Z-.25 F45.
N178 Y-.25 F7.
N179 G03 X1.4138 Y0. I0. J.25
N180 X.5888 Y0. I-.4125 J0.
N181 X.8388 Y-.25 I.25 J0.
N182 G01 Y0.
N183 G00 Z.2
N184 X0. Y.837
N185 Z.1
N186 G01 Z-.25 F45.
N187 X-.25 F7.
N188 G03 X0. Y.587 I.25 J0.
N189 X0. Y1.412 I0. J.4125
N190 X-.25 Y1.162 I0. J-.25
N191 G01 X0.
N192 G00 Z.2
N193 Z1.
N194 M09
N195 M05
;N196 G53 Z0.
;N197 G53 Y0.
N198 M30

(END OF PROGRAM)
%

I think your problem is in Mach. There is I think a check box to auto zero the axes on cycle start. Check Genral Config. I haven't got it open but I will ckeck in the morning. Best way to set tools in Mach. Just put the tool in the spindle. Use a gauge block off say the table. Bring the tool in contact with the block and zero the z axis. Then put next tool in. Touch gauge block. Then on offsets page click the tool offset button on bottom right of screen making sure the value in the box is zero. Then continue till all tools are done. Then just set the part z zero and your good to go.

[Jamespvill]

I think your problem is in Mach. There is I think a check box to auto zero the axes on cycle start. Check Genral Config. I haven't got it open but I will ckeck in the morning. Best way to set tools in Mach. Just put the tool in the spindle. Use a gauge block off say the table. Bring the tool in contact with the block and zero the z axis. Then put next tool in. Touch gauge block. Then on offsets page click the tool offset button on bottom right of screen making sure the value in the box is zero. Then continue till all tools are done. Then just set the part z zero and your good to go.

Thanks for the input, Although I'm not seeing anything that has an auto zero on cycle start check box, I may be not looking hard enough. Here's a copy of my general configs...

[magicniner]

Your lines with the required H-Word as referenced in the linked thread to the MACH3 support forum are commented out (start with a semi-colon which instructs MACH3 to disregard and not interpret the line),
(Dare I say Duh? :-) )
Nick

[Jamespvill]

Sorry! Thick skull and slow learner. It would behoove me to pick up and read some literature about CNC programming. Here I was thinking that this would be easy to learn!

What I'm getting from your provided link is that...

N2 T1 M06
N3 G43 H1

Basically means...Tool 1, Change tool (stop and move for tool installation), then G43 calls for a tool offset and H1 specifies what offset. Does that sound about right?

[JEST]

Basically means...Tool 1, Change tool (stop and move for tool installation), then G43 calls for a tool offset and H1 specifies what offset. Does that sound about right?

Not quite... There is no "stop" command issued... Code as written, assumes ATC and will not "stop"... You will need a stop or pause command (M00/M01) if changing tool manually. I would also advise moving to a neutral or at least a position clear of part (room to change tool)

[KSky]

I use the Tormach_PCNC_1100_Rev1 post and that seems to work pretty well with Mach. I measure my tools using the TTS granite block and height gauge and put that into Mach. I don't put any offsets into BobCad. I use a spreadsheet to make sure my tool #X in Mach is tool #X in BobCad.

[Jamespvill]

I use the Tormach_PCNC_1100_Rev1 post and that seems to work pretty well with Mach. I measure my tools using the TTS granite block and height gauge and put that into Mach. I don't put any offsets into BobCad. I use a spreadsheet to make sure my tool #X in Mach is tool #X in BobCad.

Whoo!! I switched to that post and now It's doing exactly what I want! Thank you KSky for the suggestion.

And thank your to everyone else for their assistance, I've learned a lot about Gcode. I order a CNC programming book to get some further knowledge too.

One last question before I call this one a wrap; When mach calls for a tool change, it only rises 1 inch above the part, then at the end of the program it rise quite high and tries to go way off westward. Which lines dictate these heights? And is this something that I can modify perminitly in the post?

(BEGIN PREDATOR NC HEADER)
(MACH_FILE=3XVMILL.MCH)
(MTOOL T1 S1 D0.375 C0. A0. H2.5 DIAM_OFFSET1 =0.1875)
(MTOOL T2 S1 D0.375 C0. A0. H2.5 DIAM_OFFSET2 =0.1875)
(SBOX X0. Y0. Z-2. L2. W2. H2.)
(END PREDATOR NC HEADER)

%
O100 (PROGRAM NUMBER)
(PROGRAM NAME: BIOHAZ.TAP)
(POST: TORMACH PCNC1100)
(DATE: SAT. 01/03/2015)
(TIME: 03:21PM)

N01 G90 G80 G40 G20 G17

(FEATURE 2 AXIS)
( TOOL # 1 0.375 ENDMILL ROUGH)
N02 T1 M06
N03 S3000 M03
N04 G00 G90 G54 X0.9271 Y2.2476
N05G43 H1 D1 Z1.
N06 M08
N07 Z0.2
N08 Z0.1
N09 G01 Z-0.25 F45.
N10 Y1.9976 F9.5
N11 G03 X1.0755 Y1.9976 I0.0742 J0.
N12 G01 Y2.2476
N13 G00 Z0.2
N14 X0.8463
N15 Z0.1
N16 G01 Z-0.25 F45.
N17 Y1.9976 F9.5
N18 G03 X1.1563 Y1.9976 I0.155 J0.
.........
N127 Z0.1
N128 G01 Z-0.25 F45.
N129 X0. F9.5
N130 G03 X0. Y1.2353 I0. J0.2358
N131 G01 X-0.25
N132 G00 Z0.2
N133 Y0.6828
N134 Z0.1
N135 G01 Z-0.25 F45.
N136 X0. F9.5
N137 G03 X0. Y1.3162 I0. J0.3167
N138 G01 X-0.25
N139 G00 Z0.2
N140 Y0.602
N141 Z0.1
N142 G01 Z-0.25 F45.
N143 X0. F9.5
N144 G03 X0. Y1.397 I0. J0.3975
N145 G01 X-0.25
N146 G00 Z0.2
N147 Z1.

N148 M09 M05
(FEATURE 2 AXIS)
( TOOL # 2 0.375 ENDMILL FINISH)
N149 T2 M06
N150 S3000 M03
N151 G90 G54 X0.8388 Y1.9976
N152G43 H2 D2 Z1.
N153 M08
N154 G00 Z0.2
N155 Z0.1
N156 G01 Z-0.25 F45.
N157 Y2.2476 F7.
N158 G03 X0.5888 Y1.9976 I0. J-0.25
N159 X1.4138 Y1.9976 I0.4125 J0.
N160 X1.1638 Y2.2476 I-0.25 J0.
N161 G01 Y1.9976
N162 G00 Z0.2
N163 X1.9995 Y1.162
N164 Z0.1
N165 G01 Z-0.25 F45.
N166 X2.2495 Y1.1617 F7.
N167 G03 X1.9998 Y1.412 I-0.25 J0.0003
N168 X1.9998 Y0.587 I-0.0005 J-0.4125
N169 X2.2495 Y0.8373 I-0.0003 J0.25
N170 G01 X1.9995 Y0.837
N171 G00 Z0.2
N172 X1.1638 Y0.
N173 Z0.1
N174 G01 Z-0.25 F45.
N175 Y-0.25 F7.
N176 G03 X1.4138 Y0. I0. J0.25
N177 X0.5888 Y0. I-0.4125 J0.
N178 X0.8388 Y-0.25 I0.25 J0.
N179 G01 Y0.
N180 G00 Z0.2
N181 X0. Y0.837
N182 Z0.1
N183 G01 Z-0.25 F45.
N184 X-0.25 F7.
N185 G03 X0. Y0.587 I0.25 J0.
N186 X0. Y1.412 I0. J0.4125
N187 X-0.25 Y1.162 I0. J-0.25
N188 G01 X0.
N189 G00 Z0.2
N190 Z1.
N191 M09
N192 M05
N193 G91 G28 Z0.
N194 G91 G28 X0. Y0.
N195 G90
N196 M30
%

Thanks folks!

[fidia]

You can edit the post processor to add the following G Code to your post

G00 G53 Y0 Z0

This will bring the Y to the home position and the Z to the home position. If your Y home is to the back of the machine then just use Z0.

See below:

3. Tool change
n,coolant_off
n,spindle_off
n,"G53","Z0."
n,optional_stop
" "
system_comment
feature_name_comment
" "
n,"M06",t
n,s,spindle_on
n,rapid_move,absolute_coord,work_coord,force_x,xr, force_y,yr,rotary_xy_angle
n,rapid_move,length_offset,coolant_on
output_rotary_angle

[Jamespvill]

You can edit the post processor to add the following G Code to your post

G00 G53 Y0 Z0

This will bring the Y to the home position and the Z to the home position. If your Y home is to the back of the machine then just use Z0.

See below:

3. Tool change
n,coolant_off
n,spindle_off
n,"G53","Z0."
n,optional_stop
" "
system_comment
feature_name_comment
" "
n,"M06",t
n,s,spindle_on
n,rapid_move,absolute_coord,work_coord,force_x,xr, force_y,yr,rotary_xy_angle
n,rapid_move,length_offset,coolant_on
output_rotary_angle

Awesome! Thank you sir, time to tinker with some gcode!