[mhackney]

+1 MikeC8. I've been doing this long enough that I know the routine! I wouldn't care at all about the wasted Z movements for a one off. My goal is to "internalize" how BC works so I can pick the best strategies for a particular geometry and result without having to do a lot of test cutting. I was at that level with VCarvePro - but it is a lot less sophisticated program and maybe easier to get to that point. But I'm getting there.

[jrmach]

One thing,,,if you had crap for laser quality,,then they had crappy laser

For small runs,it can be a toss up.

Find someone with a quality laser and check them out,,,,,,thing is,you can be making money doing something else,while the laser cuts it

Guess it depends on workload

I use to use water jet,,,but a local shop bought a Mazac at right about a million dollars,,,,,un-believable,absloutely un-believable

So,keep that in mind,,,sometimes it makes business sense,,,playing musical clamps is not fun,,,,either is the fact you either leave a few thousandth on the bottom and have to deburr it off and or put a waste board underneath.

If I have other work I could be doing,I will avoid the above,just not efficient or fast,,,my .02

[MikeC8]

I would consider making a jig for your first opp and drill those by hand with some drill bushing guides.

And for your roughing profiles, have you tried contour ramping? That will keep it from lifting up between z height passes, if you are taking multiple depth cuts.

And breaking up your profile cuts to save on rapid time does make sense, I have done that to move around clamps before.

[mhackney]

Rob, I was traveling for work earlier this week and now that I'm home I installed your post and tried out the features. It looks great, thank you very much! I haven't cut any metal yet but I read through the gcode and it looks like it's doing exactly what I want, when I want it! Brilliant!

cheers,
Michael

OK, sorry for the delay, first day of decent weather for weeks here so I have been outside working on the old homestead

Anyway, see the attached files for a new Advanced MillPst and the associated files it needs to work, the 3 files are all together in one Zip file so you only need to open it and simply "copy and paste" all 3 files into your V28 Mill Post Folder, don`t do a "save as", just "copy and paste".

The second Zip file contains a BobCAD test file for you to play with, once you open it in V28 you will be able to go to every feature and select what I hope is exactly what you want at every level whether it be a Stop, a Tool Change Reminder/Spindle OFF or a Hold Downs reminder, it will be a case of "mix and match" as required by what you are doing, there is also full Tool info at every operation and a Spindle ON reminder so once you get used to running it you should have everything right at you fingertips.
Because you said you needed it to be "all things to all jobs" that is what I have tried to do but I have had to do a little mixing of User Comments and Advanced Posting

As you also said that you don`t have your spindle under Mach3 control I have left out all the normal spindle On/Off/Speed commands as I am assuming you will be setting the Spindle rpm for each operation at the Mach3 control screen, anyway I was guessing a bit on that so hope I got it right

If it works (It is a bit rushed !!!) then enjoy, if it doesn`t then the usual caveats apply, use at your own risk

P.S. As I think you will be setting each new tool at the start of it`s particular operation (I normally pre-set all my tools in the tool library) I have set the PP so that it re-sets the Work Offset Coordinates (G54, G55 etc) at each change so the program should re-start at the correct place for you, the Mach3 "start from here" is notoriously dodgy and best avoided at all costs

Regards
Rob
:rainfro: :rainfro: :rainfro:

[The Engine Guy]

Rob, I was traveling for work earlier this week and now that I'm home I installed your post and tried out the features. It looks great, thank you very much! I haven't cut any metal yet but I read through the gcode and it looks like it's doing exactly what I want, when I want it! Brilliant!

cheers,
Michael

OK, enjoy

If you need any further "tweaks" let me know or have a go youself just for fun

Regards
Rob
:rainfro: :rainfro: :rainfro:

[mhackney]

@The Engine Guy, looks like I'm going to have to go through your post and make some edits. I attempted to use an output gcode file this weekend and got an odd "can't perform 2 g-codes" (paraphrasing) error on line N20 here:

(BEGIN PREDATOR NC HEADER)
(MACH_FILE=MICHAEL-MILL.MCH)
(MTOOL T120 S1 D.5 H3. A0. C0. DIAM_OFFSET 120 = .25)
(SBOX X-1.497 Y-.625 Z-1. L2. W1.25 H1.)
(END PREDATOR NC HEADER)

%
O0001 (YBALLNUTMOUNT.NC)
(PROGRAM NUMBER)

(FIRST MACHINE SETUP - Machine Setup - 1)
(PROGRAM NAME - YBALLNUTMOUNT.NC)
(POST - DESKTOP MILL)
(DATE - SAT. 04/23/2016)
(TIME - 02:49PM)

N10 G90 G80 G40 G20 G17

N20 G00 G91 G28 Z0
N30 G91 G28 X0. Y0.

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

My Post does this:

%
(YBALLNUTMOUNT-NEW.NC)
(File created: SAT. 04/23/2016 - 03:15PM)
(Post: MACH 3 MILL NO ATC)
(Stock: L = 2. W = 1.25 H = 1.)
(Tools used
(120 = 1/2 FLAT ENDMILL - STANDARD)
(------------------------------------------)
(Machine Setup - Machine Setup - 1)
(------------------------------------------)
N10 G00 G49 G40 G20 G70 G17 G80 G90 G91.1
(~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~)
(Machine Setup - 1 Profile Finish)
(FEATURE 2 AXIS)
(~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~)
(Tool: 1/2 FLAT ENDMILL - STANDARD)
N20 T120 M6
N30 S3880 M03
N40 G90 G54 X.1875 Y0.
N50 G43 H120 Z1. M08
N60 Z.2
N70 Z.1

I should be able to sort out. I don't have home switches hooked up right now either. In any event, this line seems odd to me!

[The Engine Guy]

Hi Michael

This is the Block in the PP that outputs those lines of code :-

2. Start of file Standard
"(PROGRAM NAME - ",prog_name,")"
"(POST - ",machine_make,machine_model,")"
"(DATE - ",output_date,")"
"(TIME - ",output_time,")"

" "
n,absolute_coord,cancel_drill_cycle,"G40",inch_mod e,"G17"
" "
n,rapid_move,incremental_coord,"G28","Z0"
n,rapid_move,incremental_coord,"G28","X0.","Y0."
" "
system_comment
feature_name_comment
comment_start"TOOL #",list_tool_number, "-",(tool_label),comment_end
n,t,
n,"M00"
user_comment_10
n,rapid_move,absolute_coord,work_coord,force_x,xr, force_y,yr,rotary_xyr_angle,
n,rapid_move,length_offset,coolant_on

Just remove the two lines in Blue and you should be fine, they are actually "safety" moves that would normally move the machine back to it`s Homed position, but, as you don`t have limit switches and haven`t homed the machine they shouldn`t be there

Also Block 5 in the PP which outputs the end of the file has them in so remove them as shown in Blue again below, should be fine after those little "tweaks"

5. End of file for non-zero tool
n,coolant_off
n,spindle_off
n,rapid_move,incremental_coord,"G28","Z0"
n,rapid_move,incremental_coord,"G28","X0.","Y0."

Regards
Rob
:rainfro: :rainfro: :rainfro:

[mhackney]

Ok, thanks I'll make the edits and test it out. I really appreciate the help!