[Potatohead908]

I am having issues getting started with my first cuts. I have a new to me 1999 VMC 15. I think I have set my tool offsets correct and fixture offsets correct. I also think I have origin and post processing correct in Fusion 360. However, somewhere I am having an issue. Please review the attached pictures and let me know what you see wrong.

I used a 2" gauge block that has a plunge dial indicator, placed on the table of the mill to get the tool length offset. I used the same tool placed on top of the stock to get the fixture offset in Z. I gathered the data in that order too.

If there is more info needed, please ask away!

Tool length offset


Fixture offset E1/G54


Facemill operation from Fusion 360

[vanaheim]

Your links dont work. I have a Fanuc 6m controller and here is my basic facemilling program, Note it is G21 (mm) and is for a 63mm diameter index facemill tool with a 1mm cut. The program starts and finished with a G49 code which cancels all tool offsets from memory. Dont know if this is significant but it makes sense. I note that your G+M codes are not capitalised or have the 0 preceding the second numeral. Again it may be Fanuc thing. My advice would be to go through each line of code and do the dance to see what you are asking the machine to do actually works. If you need a list of what the G+M codes are have a look here https://www.cnccookbook.com/g-code-m...ist-cnc-mills/

This is my facemill code generated by Edgecam software. Hope it helps

%
:0502
(FACEMILL)
N1 G21 G90 G40 G80 G49 G54
N2 (DEFINE OPERATION : FACE MILL OPERATION)
N3 M05
N4 G91 G28 Z0.0
N5 G91 G28 X0.0 Y0.0
N6 T05 M06 (USER DEFINED)
N7 M01
N8 S1200 M03
N9 G90 G00 G54 X40.5 Y-25.0
N10 G43 Z5.0 H05 M08
N11 Z4.5
N12 G01 Z-1.0 F600.0
N13 X-260.0
N14 G00 Z5.0
N15 M05
N16 M09
N17 G91 G28 Z0.0
N18 G91 G28 X0.0 Y0.0
N19 T01 M06
N20 G49
N21 G90
N22 M30
%

Note T01 is my edgefinder and that lives in the machine. All my tool offsets are in relation to the bottom edge of the edge finder. I never set tool offsets against the work face.

[Potatohead908]

I don't know why but when I pasted the code in the message it looked fine. Then when it posts it jacks with the caps. Plus the links work for me and were uploaded to this site....IDK. My brain is fried at the moment. I have a breakdown of all the G and M codes used by my Fadal and can't see what the issue with the code is. Thank you for the reply Van. I have a feeling it is something to do with my offsets....which can be seen in the images....that I hope others can see.

[Potatohead908]

Lets try this again.

%
O1001 (FACING TEST)
(T1 D=2. CR=0. - ZMIN=-0.05 - FACE MILL)
N1 G90 G94 G17
N2 G20
N3 G28 G91 Z0.
N4 G90


(FACE1)
N5 M9
N6 T1 M6
N7 S2500 M3
N8 G4 P72
N9 M8
N10 G0 G54 X6.5 Y-1.975
N11 G43 Z0.6 H1
N12 Z0.2
N13 G1 Z0.15 F30.
N14 G18 G3 X6.3 Z-0.05 I-0.2
N15 G1 X5.2
N16 X-0.2
N17 G17 G2 Y-0.7675 J0.6038
N18 G1 X5.2
N19 G18 G2 X5.4 Z0.15 K0.2
N20 G0 Z0.6
N21 G17


N22 M9
N23 G28 G91 Z0.
N24 G90
N25 G0
N26 G53 X0. Y0.
N27 M30
%

[Potatohead908]

I will come back tomorrow after I verify my issue. I think what I have done is stacked my offsets on top of each other. Since I used the top of the table as my measuring "base" for the tool table, what I think I need to do is identify the difference between the top of the stock and the table, then enter that as a positive value in the Fixture Offset for Z.

[vanaheim]

I dont use a fixture (work? or stock?) offset versus tool lengths. T01 is my edge finder and the bottom face is set to Z=0 in my tool length data table for T01. All tool lengths are as variations to T01 Z=0. in the tool length library.

Work G54 Z height is set as a relationship to T01. All tools are thus set to automatically be correct lengths irrespective of work height.

I don't worry about about vice height in relation to tool lengths. As long as the work Z is higher than the vice depending upon the deepest cut made (as measure by a ruler) I dont see what entering the vice height into the program will actually do for you.

[Potatohead908]

I'm seeing there are at least 2, I th in n maybe 3 ways people do these offsets. This is a response to my question on another site and is the way I I was working toward in my noodle. I may change it later once I have a better grasp of everything.

"leave your most commonly used tools in pocket 1~15 put anything else in 16~21 set them all off the table surface and use positive fixture offset measured distance from table up the jaws or fixture that way you can usually leave all tools intact in the carousel"

[rodney247]

First off your working on a Fadal not a fanuc everyone trys to solve Fadal issues with Fanuc procedures. Number one if your just using 1 fixture you dont need a fixture offset G54 or E1 easist thing is to just leave that out or all zeros in that fixture offset and just do a SETX SETY SETZ or if your at the position do a SETH. And check how the SETP is setup are you Format1 or Format2(Fanuc Compatible) So Now at this point your "home is set" Now if you have the UT command set your tools. and they all will be a negative number T1 -4.567, T2 -6.234, T3 -12.567.... etc etc. so your H will get the tip of the tool to where the Zzero is. And your ready to go. Hit Auto good to go

you would have more success if your program looked more like

%
O1001 (FACING TEST)
(T1 D=2. CR=0. - ZMIN=-0.05 - FACE MILL)
N1 G90 G17 G0 G80




(FACE1)

N6 T1 M6
G90G0GG17G80
N7 S2500 M3

N10 G0 G54 X6.5 Y-1.975 (dont need the G54 but if it posts make sure in the DF page the xyz are all zero
N11 Z0.6 H1M8
N12 Z0.2
N13 G1 Z0.15 F30.
N14 G18 G3 X6.3 Z-0.05 I-0.2
N15 G1 X5.2
N16 X-0.2
N17 G17 G2 Y-0.7675 J0.6038
N18 G1 X5.2
N19 G18 G2 X5.4 Z0.15 K0.2
N20 G0 Z0.6
N21 G17
M9

G0G90
N23 G53 Z0.



N26 G53 X0. Y0.
N27 M30
%

[Potatohead908]

Thanks Rodney, I will sit down in a bit and process all you wrote. I am running Format 2. I do have two vises on the table and intend to use them both, in the same program, once I get my head wrapped around this more.

I officially just made my first chips on this machine. I used the process in my last post. There is also another active thread on this Fadal forum where the author describes the same process better than I have here. Pretty damn excited!