[Wyrks Tool]

Hello.

I have posted about this already on here and I got no replies at all. Am I asking wrong, or is this something no else has run into?
I will try again and hopefully someone with more experience than myself will be able to point me in the right direction.

I am having a problem in v24. I generate a drawing for a hole and then select ‘contour ramping’ in 2 axis milling to interpolate the hole. I am using a Fanuc 18 post processor that I downloaded from Bobcad. When I post the program, it gives me all of my circular moves to make the hole, but no ‘z’ move to move the tool down into the part. So, I wind up with a bunch of lines of code that are I’s and J’s only. When I run it on my machine it moves to the top of the part and proceeds to do the number of revolutions that are programmed without moving down any further.
If I draw a rectangle and do the same thing, the code posts perfectly. I get an x, y and z move on each line.
I get the same result (no z move) when I try to do thread milling.
What I am (obviously) trying to accomplish is helical interpolation to produce holes with a cutter. Am I trying to use the wrong cycle? Do I have a parameter set wrong?
Any help/suggestions would be greatly appreciated.

Thanks
Scott

[magicniner]

You could try posting with a couple of alternate post processors, if that produces Z moves on the same job then it looks like being your Post Processor

[jrmach]

Take your .bbcd file and a copy of your post processor and upload them here in a .zip file.
Otherwise it's just a lot of back and forth and a lot of time goes by.

[The Engine Guy]

It will most likely be the Post Processor you are using, I downloaded one of the Fanuc 18i processors and it didn`t generate the Z moves, best one to use is probably the BC_3X_Mill.MillPst, I have zipped one up in the attached file for you to try, shouldn`t need much if any "tweaking" to get it how you need it

I have run a Helical cut in a hole using both Standard and Contour Ramping, worked fine with all the Z moves present and correct

Regards
Rob
:rainfro: :rainfro: :rainfro:

P.S. Here is the code as generated, Bobcad file also attached :-

%
O0100 (PROGRAM NUMBER)
(PROGRAM NAME - HELICAL TEST)
(POST - MACH3 4-AXIS BOXFORD)
(DATE - THU. 07/10/2014)
(TIME - 08:37PM)
N01 G17 G40 G49 G80 G21 G90
N02 G00
N03 G28 G91 Z0
N04 G28 G91 X0 Y0
(FIRST CUT - FIRST TOOL)
(TOOL #1 - 12.700 Dia. 0.000 CRad. 4 Fl.38.100 CL)
N05 T1 M06
N06 G00 G90 G54 X8.65 Y0. S1252 M03
N07 G43 H1 Z2. M08
N08 G01 Z0. F254.583
N09 G17 G03 X8.65 Y0. Z-4. I-8.65 J0.
N10 X8.65 Y0. Z-8. I-8.65 J0.
N11 X8.65 Y0. Z-12. I-8.65 J0.
N12 X0. Y-8.65 Z-15. I-8.65 J0.
N13 X8.65 Y0. I0. J8.65 F496.436
N14 X0. Y-8.65 I-8.65 J0.
N15 G00 Z2.
N16 M09
N17 M05
N18 G91 G28 Z0.
N19 G91 G28 Y0.
(END OF FILE)
(END OF PROGRAM)
N20 M30
%

[Wyrks Tool]

Thanks for the file. I tried it and it worked.
I also modified the post processor I am using (Fanuc 18) on the advice of a user on a different forum. I had to add a z value on one of the lines in the post processor. If anyone would like this information, just let me know.
Forums like this are awesome. It is great that people are willing to help, even though we may be competing in the same industries.
Keep up the good work.