I'm trying to use G13 parameter

[PcRobotic]

Hello everyone,

I'm having a day off and I would love to use it wisely while staying home. I would like to use CIRCLE MILL to generate G13 codes instead of LONG CODES. I tried to look for parameter numbers for CIRCLE MILL, ROUGH, FINISH, DEPTH inside the CIRCLE MILL and not success through out the PARAMETER PDF file. Is there another hint that I can get somewhere or in this forum?

 

I suppose to have 300 finish holes need to be milled with CIRCLE MILL function and this function really KILLS my equipment's memory. I think only G13 can do it well with much less codes.

 

below here is how G13 works, please help. Thank you

 

T1 M06

G00 G43 H01 D11 <-- ASSUMING OFFSET11 FOR YOUR DIA.

G00 X0 Y0 Z.5

S1200 M03

M08

G01 Z-.5 F200.

G13 I1.49 K1.5 Q.01 F5.

G01 Z.5 F200.

M09

...

...

...

 

Not sure if your manual describes the proper useage for your control, but on a HAAS it is as such:

 

D - Tool diameter/radius offset selection

I - Radius of first circle, or finish if K is omitted

K - Radius of finished circle

L - loop count for repeated deeper cuts

Z - depth of cut or increment [when used with L]

Q - Radius increment [must be used with K]

F - feedrate within cycle

 

 

ps: here is how G13 works

[Guest]

I did this once back a LONG time ago so the code is long gone but here's the jist;

 

I used a Custom Drill Cycle. Most of what you need is already there. On a scale of 1-10 on difficulty, this would be probably a 3 or 4 for someone that has made basic edits on posts before.

 

The downside to this method is you won't be able to see it backplot.

[PcRobotic]

Thanks for the tip, Foghorn Leghorn. At least I know where to start.

[crazy^millman]

I did this once back a LONG time ago so the code is long gone but here's the jist;

 

I used a Custom Drill Cycle. Most of what you need is already there. On a scale of 1-10 on difficulty, this would be probably a 3 or 4 for someone that has made basic edits on posts before.

 

The downside to this method is you won't be able to see it backplot.

 

Foghorn this one has been going on for almost a year now. I have provided link after link for him to do it and here we are still a year later back to the same place. Sorry PC, but you keep beating this dead horse and like he said been many years since I did it as well. Maybe our new super star will come in here and do it all for you.

[kennebec]

see your reseller...

[PcRobotic]

Hi Crazy Milman,

I got stuck part of it and tried to get the idea. Sorry for asking this repeatedly and honestly it makes me looks bad but really, really I had no choice other than "ask". Once again thanks to Crazy Millman and Foghorn.

[crazy^millman]

PcRobtic sorry to call you out, but like I have said many time before you are going about this all wrong. You have come back many times to using a circle mill cycle and many times I have pointed you to the custom drill cycle to control this. I have all but done it for you and yet here we are. Have your company pay someone to do it for you.

[BrianP.]

Subprogram will work as well as a G13 for saving on memory. There are a couple of different ways to get what you need. If the holes are in a pattern transform will work just fine.

 

 

 

T1 M6
G0 G54 G90 X-.005 Y0. S1069 M3
G43 H1 Z.1
M8
M97 P0001
G0 G90 X1.495
M97 P0001
G0 G90 X2.995
M97 P0001
G0 G90 X4.495
M97 P0001
G0 G90 X5.995
M97 P0001
G0 G90 X7.495
M97 P0001
G0 G90 X8.995
M97 P0001
G0 G90 X10.495
M97 P0001
G0 G90 X11.995
M97 P0001
G0 G90 X13.495
M97 P0001
M9
M5
G28 G91 Z0.
G0 G53 G90 Y0.
M30
 
N0001
G91
G1 Z-.6 F6.4
G41 D1 X.0732 Y-.0732
G3 X.1768 Y.0732 I.0732 J.0732
I-.245 J0.
X-.1768 Y.0732 I-.1036 J0.
G1 G40 X-.0732 Y-.0732
Z.6
G0 X.005
G1 Z-.6
G41 X.0732 Y-.0732
G3 X.1768 Y.0732 I.0733 J.0732
I-.25 J0.
X-.1768 Y.0732 I-.1035 J0.
G1 G40 X-.0732 Y-.0732
Z.6
M99

[Peter - Avivi CNC Solutions]

Okay, since our local Mr.Dr.Prof.PhD. 97% had no chance and probably time to visit this topic to share some cool ideas with us, I feel then it's my job to tell the rest 3%..........

 

1, Look for "opcode$ = 2 & tool_op$ = 18" in "ptlchg$" and "ptlchg0$" postblocks

2, Output G12/G13 line based on operation depth, diameter, refpoint, stock etc parameters

3, In prapidout postblock look for G0 - (next)G1 lines to grab arc center at next-next G2/G3 line

4, Output arc center as position.

5, Switch "subout$" from zero to different output to release circles output to the air

6, Back to zero with "subout$" for the next hole

7, Order a beer for me, cus I just simply deserve

 

This should be the process, but roughly, during the workaround, some issues may turn out as always...

[Guest]

Is this what you are looking for?

 

You'll have to set up your retracts and secondary cuts but I "assume" you can do all of that

 

#---------------------------------------------------------------------------

# Misc Variables

#---------------------------------------------------------------------------

 

fmt "D" 2 tool_dia

fmt "I" 2 circle_rad

fmt "K" 2 finish_rad

fmt "L" 4 loop_count

fmt "Z" 2 z_doc

fmt "Q" 2 rad_inc

 

pg13cycle

 

#D - Tool diameter/radius offset selection

#I - Radius of first circle, or finish if K is omitted

#K - Radius of finished circle

#L - loop count for repeated deeper cuts

#Z - depth of cut or increment [when used with L]

#Q - Radius increment [must be used with K]

#F - feedrate within cycle

tool_dia = peck1$

circle_rad = peck2$

finish_rad = peckclr$

loop_count = retr$

z_doc = dwell$

rad_inc = shftdrl$

pdrlcommonb

pcan1, pbld, n$, "G13", tool_dia, circle_rad, [if peckclr$ > 0, finish_rad], [if retr$ > 0, loop_count], z_doc, rad_inc, feed, e$

pcom_movea

 

 

[drill cycle 9]

1. "G13 Milling Cycle"

3. "Depth"

4. ""

5. ""

6. ""

7. "Tool Dia/Radius"

8. "1st Rad/Fin Rad"

9. "Fin Rad"

10. "Loop #"

11. "Rad INC w/K"

[The Cathedral]

I just got done doing this for my own post, using Helix Bore to pull the parameters and insert them into a single line of code--we use a helix bore macro that I wrote a long time ago on the floor. I didn't want to use a custom drill cycle inside mastercam because I wanted the toolpath and simulation to accurately reflect how the tool would be moving and cutting.

 

Here is how my output looks:

 

N19 (  1/4 FLAT ENDMILL )
G0 G40 G80 G90 G55 S7609 M3
G43 H19 X.095 Y2.03 Z1. M8
Z-.935
G65 H.427 T.25 D-1.25 R-.935 C.015 F10.
Z1.
M9

 

instead of mastercam doing the whole helix. Obviously the macro is unique, but all the numbers are pulled from the actual helix bore cycle and not a work around.

[Guest]

I guess I won't post any more "work arounds"

[The Cathedral]

I guess I won't post any more "work arounds"

 

Don't take things so personally, man. What you posted looks great, but you can't deny that it doesn't reflect the actual tool motion inside mastercam. That's all I meant. 

[PcRobotic]

Hi,

  I tried with JParis and it worked fine. Thank you JParis.

 

Is there away that I use value as DEPTH, RETRACT in the LINKING PARAMETER instead it having its in the CUT PARAMETER page?

[PcRobotic]

Hi Peter,

   Would you please be more detail about your ideals of G13?  Honestly, I think I need more words from you in order to do it.  Would you please explain more?  Thanks, Peter.

 

1, Look for "opcode$ = 2 & tool_op$ = 18" in "ptlchg$" and "ptlchg0$" postblocks

2, Output G12/G13 line based on operation depth, diameter, refpoint, stock etc parameters

3, In prapidout postblock look for G0 - (next)G1 lines to grab arc center at next-next G2/G3 line

4, Output arc center as position.

5, Switch "subout$" from zero to different output to release circles output to the air

6, Back to zero with "subout$" for the next hole

7, Order a beer for me, cus I just simply deserve

 

This should be the process, but roughly, during the workaround, some issues may turn out as always...

[Guest]

Hi,

  I tried with JParis and it worked fine. Thank you JParis.

 

Is there away that I use value as DEPTH, RETRACT in the LINKING PARAMETER instead it having its in the CUT PARAMETER page?

Just use the variables in the correct places

 

depth$

retr$