[watchman]

Hi,
I'm new to EMC2 and have a problem. I don't understand how I can use a subroutine in the g-code supported by EMC. What I am trying to do is grind a part which is mounted vertically on a rotary table ('C' axis) and I want to grind a diameter, step down nearly the width of the grinding wheel and repeat the grinding to diameter a number of times (there is a good reason for wanting to do it this way rather than turning the diameters!). So, what I would like to create is a subroutine which would take care of the grinding to diameter part (and preferably be able to accept different final diameters). Reading the EMC2 documentation I guess that G81 wouldn't do but that some form of 'O' routine might - the only problem is that I don't understand how the 'O' routine is supposed to work or how it is called from the main program - other documentation seems to suggest G98 but this doesn't seem to be supported by EMC2. Can anyone offer (simplified) words of wisdom please? Thanks, Ian

[Dan Falck]

Try something like this:

%
(SUBROUTINE EXAMPLE)

o100 sub
G02 X-.5 Y-0 I-.5 J0
G02 X.5 Y-0 I.5 J0
o100 endsub

G54
G01 X.5 Y0 Z1. F50.


G1 Z-.25
o100 call
G1 z-.5
o100 call
G1 z-.75
o100 call


G0 Z1.
M30
%

Notice that I put the subroutine at the top of the program. I read in the user's manual (page 153) that subs had to preceed the code that calls them.
I hope this helps you out.
Dan

[cyclestart]

Hi,
G98 but this doesn't seem to be supported by EMC2.

EMC2 does support G98, at least with code G81. Just loaded a drill program to double check. Not sure if there is a problem with G98/G99 with other canned cycles. Maybe the problem is with the height of the initial approach movement or the use of G90/G91 ?

Edit/ Took the time to read the post more closely. This isn't a job for a canned cycle.

[watchman]

Thanks,
I did find a bit more in the EMC WIKI and made a script as below..
%
#1 = 0.2 (finished diameter)
#2 = 0.05 (feed step size)
#3 = 1 (total depth)
#4 = 0.1 (safe X)
#5 = 1.4 (stock diameter)
#6 = 0.5 (grinding disk thickness)
#7=#6
#8 = [[[#5-#1]/2]/#2] (no. of turns of A axis to final diameter)
#9 = [#3/#6]+1 (no. of steps down to finished depth)
#10 = [#3/#9] (step size)
#11 = 0 (counter)

o100 do
G0 Z[0 - #10]
G0 A[#8*360] X[[[#5] - [#1]] /2]
G0 X[#4]
#11 = [[#11] + 1]

o100 while [[ #11 * #10] LT #3]


o200 sub
G0 Y5.0
G0 X-0.565
G1 Y-5.0 F 3.0
G0 A180
G1 Y5.0 F3.0
G0 Y0.000
G1 A180 F15
o200 endsub

N001 G21 G90 G40 G49
N002 o100 call [0.20] [0.04] [1.00]
N003 o100 call [0.27] [0.05] [2.00]
N004 G0 Z-3.3
N005 o200 call
N006 G0 Z-3.8
N007 o200 call
N008 G0 X0.1
N009 G0 Z-3.47
N010 o100 call [0.27] [0.05] [2.74]
N011 M0
N012 G0 Z-6.23
N013 o200 call
N014 o100 call [0.20] [0.04] [1.00]
N015 o100 call [0.1] [0.04] [0.5]
N016 G0 X40
%

I do have a problem with this, however, that I can't understand..
When I try to load it into EMC2, I get an error message saying 'Bad character near line 34' - this appears to be the line numbered N002 - the first subroutine call. I copied the format of this line directly from the WIKI and I've looked at it many times without seeing the problem - any ideas? Thanks, Ian

[lerman]

I believe you can't have line numbers on lines with o-words.

Ken

[watchman]

Thanks Ken - you are correct. I removed them from the script and EMC2 loaded it - then wouldn't run - just sat there looking stupid....dohhhh!!
Ian

[cyclestart]

There might be a problem with your use of the while loop. That program tries to load here in axis but seems to get caught in some type of infinite loop. Probably it either it doesn't have a break or can't reach it. My best guess being not much of a script writer.

I've written a few parametrics but not with the type of loops and conditionals found in the wiki.

[acondit]

Thanks,
I did find a bit more in the EMC WIKI and made a script as below..
%
#1 = 0.2 (finished diameter)
#2 = 0.05 (feed step size)
#3 = 1 (total depth)
#4 = 0.1 (safe X)
#5 = 1.4 (stock diameter)
#6 = 0.5 (grinding disk thickness)
#7=#6
#8 = [[[#5-#1]/2]/#2] (no. of turns of A axis to final diameter)
#9 = [#3/#6]+1 (no. of steps down to finished depth)
#10 = [#3/#9] (step size)
#11 = 0 (counter)

o100 do
G0 Z[0 - #10]
G0 A[#8*360] X[[[#5] - [#1]] /2]
G0 X[#4]
#11 = [[#11] + 1]

o100 while [[ #11 * #10] LT #3]


o200 sub
G0 Y5.0
G0 X-0.565
G1 Y-5.0 F 3.0
G0 A180
G1 Y5.0 F3.0
G0 Y0.000
G1 A180 F15
o200 endsub

N001 G21 G90 G40 G49
N002 o100 call [0.20] [0.04] [1.00]
N003 o100 call [0.27] [0.05] [2.00]
N004 G0 Z-3.3
N005 o200 call
N006 G0 Z-3.8
N007 o200 call
N008 G0 X0.1
N009 G0 Z-3.47
N010 o100 call [0.27] [0.05] [2.74]
N011 M0
N012 G0 Z-6.23
N013 o200 call
N014 o100 call [0.20] [0.04] [1.00]
N015 o100 call [0.1] [0.04] [0.5]
N016 G0 X40
%

I do have a problem with this, however, that I can't understand..
When I try to load it into EMC2, I get an error message saying 'Bad character near line 34' - this appears to be the line numbered N002 - the first subroutine call. I copied the format of this line directly from the WIKI and I've looked at it many times without seeing the problem - any ideas? Thanks, Ian

%

o100 sub [1] [2] [3]
(#1 = 0.2) (finished diameter)
(#2 = 0.05) (feed step size)
(#3 = 1) (total depth)
#4 = 0.1 (safe X)
#5 = 1.4 (stock diameter)
#6 = 0.5 (grinding disk thickness)
#7=#6
#8 = [[[#5-#1]/2]/#2] (no. of turns of A axis to final diameter)
#9 = [#3/#6]+1 (no. of steps down to finished depth)
#10 = [#3/#9] (step size)
#11 = 0 (counter)
o101 do
G0 Z[0 - #10]
G0 A[#8*360] X[[[#5] - [#1]] /2]
G0 X[#4]
#11 = [[#11] + 1]

o101 while [[ #11 * #10] LT #3]
o100 endsub

o200 sub
G0 Y5.0
G0 X-0.565
G1 Y-5.0 F 3.0
G0 A180
G1 Y5.0 F3.0
G0 Y0.000
G1 A180 F15
o200 endsub

N001 G21 G90 G40 G49
N002 o100 call [0.20] [0.04] [1.00]
N003 o100 call [0.27] [0.05] [2.00]
N004 G0 Z-3.3
N005 o200 call
N006 G0 Z-3.8
N007 o200 call
N008 G0 X0.1
N009 G0 Z-3.47
N010 o100 call [0.27] [0.05] [2.74]
N011 M0
N012 G0 Z-6.23
N013 o200 call
N014 o100 call [0.20] [0.04] [1.00]
N015 o100 call [0.1] [0.04] [0.5]
N016 G0 X40
%

I made a couple of changes in your code. It still has a problem that I haven't taken the time to fix. It is reporting a divide by zero error in line 11. You hadn't specified O100 as a subroutine. So I changed your do while loop to O101 and wrapped it in a O100 sub -- endsub pair. You specified three parameters in your calling sequence, but didn't specify the formal parameters in the sub routine. I moved the variables 1 thru 11 inside the subroutine and I commented out #1, #2 and #3 since they are passed in to the subroutine. If they are needed, you need to change them so they don't conflict with the parameters that are passed in at the call.

Alan

[watchman]

Thanks, I'll try Alan's amended routine as soon as I get a minute.. Ian

[cyclestart]

Thanks, I'll try Alan's amended routine as soon as I get a minute.. Ian

So how did you get on with this?

This thread was an eye opener for me. Like a 2 year old with a newly learned word, just can't resist trying to show off.
**while the more senior members snicker no doubt**

As I haven't quite grasped what you're doing, I expanded on Dan Falck's post.

The way I would have done this orginally

%
#100= 1000 (RPM)
#101= 1    (CIRCLE RADIUS)
#102= .375    (CUTTER RADIUS)
#103= 30   (FEED)
#104= 2    (X CENTER)
#105= 2    (Y CENTER)
#106= -.25 (DEPTH)


o100 sub
#107= [#101+#102] (PATH OF CUTTER)
G00 X#104 Y[[2*#102]+[#107+#105]]
G01 Z#106 F#103
G03 X#104 Y[#107+#105] R#102
G02 X[#107+#104] Y#105 R#107
X#104 Y[[-1*#107]+#105] R#107
X[[-1*#107]+#104] Y#105 R#107
X#104 Y[#107+#105] R#107
G03 X#104 Y[[2*#102]+[#107+#105]] R#102
o100 endsub

S#100 M03
G54 G00 X#104 Y[[2*#102]+[#107+#105]]
Z.1
o100 call
#101=.8
o100 call
#106=-.5
#101=1
o100 call
#101=.8
o100 call
G00 Z2
M02
%

using the "while" conditional trick

%
([1=first_cut.r] [2=cutter.r] [3=feed] [4=x center] [5=y center] [6=depth] [7=stepover] [8=finish.r])
o100 sub
o101 while [#8 LE #1]
#10= [#1+#2] (PATH OF CUTTER)
G00 X#4 Y[[2*#2]+[#10+#5]]
G01 Z#6 F#3
G03 X#4 Y[#10+#5] R#2
G02 X[#10+#4] Y#5 R#10
X#4 Y[[-1*#10]+#5] R#10
X[[-1*#10]+#4] Y#5 R#10
X#4 Y[#10+#5] R#10
G03 X#4 Y[[2*#2]+[#10+#5]] R#2
#1=[#1-#7]
o101 endwhile
o100 endsub

S1000 M03
G00 Z1
o100 call [1] [.375] [30] [0] [0] [-.25] [.1] [.8]
o100 call [1] [.375] [30] [0] [0] [-.5] [.1] [.6]
G00 Z2
M02
%

These programs are probably buggy as hell, but sure were fun to write.

Maybe there's something you can use in above somehow.