drill hole with disabled center drill and champfer in default tool settings milling. It will not let me make a tool path. Is this a software problem. Need help Please.
drill hole with disabled center drill and champfer in default tool settings milling. It will not let me make a tool path. Is this a software problem. Need help Please.
that's the problem, no file yet, just 1 hole....seems like my tool setup files are corrupted, I only have one file. any body have the *.tpatt files for win7 64 bobcam v25. I doesn't help reinstalling.
OK, here is a V25 file for you to try
Drill Test Setup.zip
.tpatt file here
ToolPattern.zip
Here is the code as output from a modified Fanuc Post Processor I have
(BEGIN PREDATOR NC HEADER)
(MACH_FILE=BOXFORD_VMC300.MCH)
(MTOOLT1S4D4.H83.A118.C0.DIAM_OFFSET 1= 2.)
(SBOX X-50. Y-50. Z-10. L100. W100. H10.)
(SSTL MILLDRILL TEST SETUP.STL)
(END PREDATOR NC HEADER)
(WORK SHIFT - G54 = X-50., Y-50., - Z????)
%
O0001(MILLDRILL TEST SETUP)
(POST - BOXFORD- VMC300)
(DATE - FRI. 08/10/2012)
(TIME - 06:08AM)
G90G80G40G21G17
N01G00G91G28Z0.
N11G91G28X0.Y0.
(JOB 1 HOLE RANDOM POINT PATTERN)
(FEATURE DRILL HOLE)
(TOOL - T01 DRILL Dia 4. Length 83.)
N21T01M06
N31M3S400
N41G4P2
N51G90G54X-32.48Y18.794S460M03
N61 G43H01Z1.5
(TOOL - T01 DRILL Dia 4. Length 83.)
N71G83G98X-32.48Y18.794Z-7.202R1.5Q2.F33.95
N81X19.758Y15.903
N91G80
N101M09
N111M05
N121G49
N131G00G91G28Z0.
N141G91G28X0.Y0.
(END OF FILE)
(END OF PROGRAM)
N151M30
%
Hope that helps
Regards
ok guys, if I load this file I can then make my own holes without center drill, or chamfer. The file works good even after changing post processor.
If I then try to load the *.tpatt file, it gives me error, "invalid argument", I even tried to save on new.tpatt, but can't load that either. Would windows updates have anything to do with this...?
The file will work OK regardless of the Post processor used, the Post only generates the G code, doesn`t affect the creation of the toolpaths at all so I would say that file is all you need, just do a "save feature" and any time you want to do any holes without centre and/or chamfer just do a "load feature" and change the selected points, tooling and parameters to suit the new drilling job and you are finished, very quick, very easy to do
If the file works OK for you then in all probability your .tpatt file is OK so I wouldn`t bother trying to change it.If I then try to load the *.tpatt file, it gives me error, "invalid argument", I even tried to save on new.tpatt, but can't load that either. Would windows updates have anything to do with this...?
Please create a drilling job from scratch, Zip it up and post it here and I or someone will take a look at it and see if it will work on my/their PC
I assume you are on Build 678 of V25 ? If not then download and install the update 678
Regards
hi guys, for the life of me I can't recreate this same situation, drilling is going fine....thanks for you time....
hi guys, I'm back, with a different problem now, my post processor will not put a g80 into the program when switching to a different tool or cycle. I am using fenuc0 processor, I do not know how to modify, help please....everything else is good ...
Wouldn`t expect you to need a G80 after every tool change, only after canned cycles, anyway try the solution below.
If you are using the standard Fanuc 0M V25 post then open it in Notepad and go to line #80, it should look like this:-
80. Drill canned cycle cancel.
n,cancel_drill_cycle
If not then alter it to the above and give it a try.
Just for your further info if you didn`t already know, line #26 in your post is:-
26. Set debug.
debug_off
If you set it to debug_on and save then re-post your code, your code will then show which line # in your post is doing which job, very useful for tracking down where to make the changes in the post.
Regards
thank you, this worked, again...