Helix bore subprogram

[Brian Pallas]

Is there a way to use the "Helix Bore" toolpath, but have it use a incremental subprogram for each hole in the toolpath?  So the tool would move to the hole position, then call the sub, and repeat for each hole?

Or are there any other ways to accomplish that fairly easily within mastercam?

 

 

[tim_h]

XFORM / TRANSLATE ??

My mistake..

As Frozen stated its : TOOLPATH / TRANSFORM 

 

[FROZEN]

Toolpath/Transform

[AMCNitro]

transform...

[Colin Gilchrist]

Yes, it just requires that you edit your Post to write the motion to the Subroutine, and then call the Sub at each new position, then suppressing the output to the NC File for the Sub, while machining each subsequent hole.

The Transform path is an excellent way to do this as well, but requires that the positions are spaced equally in XY for Translate, or Rotary. You can't just use a 'random' grouping of points with the Transform path.

[Brian Pallas]

Thanks Colin.  It's just kind of a "I wonder if..." right now.  Sometime here it'll be a good side project to see if I can get it working.  

Yeah I was wondering about a solution for irregular spacings.

One thing I'd  like totry for helix boring, or ramping around a contour, is :

 

(  1/2 FLAT ENDMILL   TOOL - 1  DIA. OFF. - 1  LEN. - 1  DIA. - .5 )
G0 G90 X0. Y0. S6000 M3
G43 H1 Z6. M8
Z.1
G1 Z.02 F60.
G43 D1 X.375 
X.75

M98H1L10

G90

G1 G40 X0.
G0 Z6. M5
G00 X0. Y10.M09
M30

N1

G91
G3 X-1.5 Z-.03 I-.75 J0.
X1.5 Z-.03 I.75 J0.
M99

%

 

So only one lap in the sub and then L count for number of loops.  I think I would like to have that option available in mcam , but if I did get something like that able to be output, I would want to come up with a way that verify and backplot in mastercam still works.  This is a recent thought, so I'll think about it a bit here and there and then try something.

 

 

 

 

[Colin Gilchrist]

For the Verify and Backplot, you'd just be verifying and backplotting the normal "Helix Bore" path inside Mastercam. Your normal programming routine wouldn't change, and the path would still appear the same on your screen when checking out the motion of the tool. The only thing we'd be doing in the post is just gathering the "info" from the operation itself, and then performing our own calculations inside the post to give you what you want for output. All the data is passed either in the form of the NCI moves, or by retrieving Parameters from the Operation itself, for use in our own calculations (inside the Post).

You'd just be taking the normal "input" from Mastercam (Helix Bore Tool Path data), and converting the output (NC Code) into a form that you prefer. Instead of a thousand lines of code to machine some bores, you'd have a bunch of G65 Macro calls, with a single Subroutine to perform the Incremental motion of the Boring Cycle. All of the positioning between the holes in done in Absolute.

 

 

[The Cathedral]

I run helix bore macros that are stored in the machines, and I've set up my post so that when I program a helix bore, the post pulls all the important info from the NCI and outputs it as a G65 (or G66) macro line; and since the macro is in the machine there is no subprogram to worry about outputting with the main program. Also, since I switch it on or off using a misc var, it has no effect at all on backplot or verify. So, basically like Colin said, minus the additional sub routine.

[Brian Pallas]

Sound cool, and something I want to look into.  Thanks.  

What do you pass to the macro - diameter of the bore, diameter of cutter, pitch and depth?

[The Cathedral]

2 hours ago, Brian Pallas said:

Sound cool, and something I want to look into.  Thanks.  

What do you pass to the macro - diameter of the bore, diameter of cutter, pitch and depth?

Hole dia, tool dia, depth, pitch, feed plane height, feed. The macro can adjust the feed to compensate using the internal radius reduction formula.

I also do the same this with a threadmill macro.