sub-programs

[cnc@gci]

I'm trying to implement subprograms to make things easier. How do you make your toolpaths a subprogram?

[cnc@gci]

It seems real easy for drill paterns, but I don't see anything like that for contouring or pocketing.

[chris m]

Don't completely understand where you are going, but if you mean that you have a bunch of pockets [for example] across your part and you want to use subs to machine them, use Toolpath-Transform and select "create subprograms" or whatever the checkbox says

[cnc@gci]

I just want to be able to make my toolpath a subprogram. I don't want to dublicate my toolpath.

[Guest CNC Apps Guy 1]

So your main you tant the following (essentially)

 

N1T1M6

G0G90G54X0Y0S10000M3

G0G43H1M8

M98P1001

G91G28Z0M9

M1

.

.

.

.

 

O1001(SUB)

G1X1.

M99

 

So on and so forth?

[cnc@gci]

Thanks.

[MACHINEMASTERG]

use the mpsubrep post it works for us

[cnc@gci]

Where can I get that?

[chris m]

Go to the POSTS link at the top of the page and click on Application Specific Posts

[cnc@gci]

I got it downloaded but it says I have to convert it. I'm using version X3, how can I convert it?

[cnc@gci]

I previewed the sample output and thats exactly what I'm looking for.

[cnc@gci]

I went in to run user application and ran updatepostdll but the log stated that it was aborted. Can you not update this post?

[Guest CNC Apps Guy 1]

I just updated an MPSubrep post today. I'm adding on all the High Speed Machining Stuff, tool breakage detection, etc... ad infinitum. I'm bored and I'm babysitting a long cycle.

[Rick46]

is this mpsubrep post that you updated going to be availaible for public use as well just curious as I use the current one available for D/L and it works pretty sweet but always up for new things my post can do for me..

[cnc@gci]

I just got the mpsubrev post to work and it seems to output the way I needed it to. Thanks guys.

[bigjohn]

I have a question. How do you get the program to rotate your subprogram around the centre in a radial array as in an impeller? Using this post of course.

 

 

John

[dolphin1]

do a xform rotate with subprogram operation after the operation that does the machining.

[Guest CNC Apps Guy 1]

quote:

---

...is this mpsubrep post that you updated going to be availaible for public use?

---

Right now it's machine specific (Toyoda HMC with a full 4th) so I don't imagine it would work for everyone so in a word no, it's not for public consumption. If a reseller were to contact me and request it for one of their customers I would happily part with it but end users... no sorry.

[Bob W.]

What exactly are sub-programs and what are the applications? It sounds interesting and I would like to learn more about them. Could someone please give a brief description.

 

Thanks,

Bob

[Guest CNC Apps Guy 1]

A sub program is a segment of code that is called from a Main Program via M98 or M198 for an external device such as a memory card or Dataserver.

 

See below;

 

code:

---

%

O1000 (T-OP01)

(MCX FILE - POST TEST.MCX)

(POST - MPSUBREP_TOYODA)

(MATERIAL - ALUMINUM INCH - 2024)

(PROGRAM - T-OP01.NC)

(DATE - JUN-019-2009)

(TIME - 09:014 PM)

(PROGRAMMER - JOE MAMMA)

 

(******************************)

(X ZERO IS ....................)

(Y ZERO IS ....................)

(Z ZERO IS ....................)

(B ZERO IS ....................)

(******************************)

 

M1

 

(***** TOOL LIST START *****)

(T1 * 1/2 FLAT VARIMILL ENDMILL * CONTOUR....)

(T8 * 1.8MM COOLANT FED DRILL - NO. 50 * DRILL/CBORE)

(T15 * NO. 8-32 TAPRH * TAP........)

(T13 * 3/64 FLAT ENDMILL * CONTOUR....)

(***** TOOL LIST END ******)

 

 

N1(OUTER PROFILE)

G0G40G49G80G90

T1(1/2 FLAT VARIMILL ENDMILL)

M6

G17

G54G90B0.(FRONT TOOL PLANE)

G0G90X1.7689Y.5859S1220M3T8

G43H1Z.25M8

G5P10000

M198P1001(CALLS SUB PROG O1001)

M5

G5P0(HPCC OFF)

G91G28Z0.M9

G49

G90

M75

G65P9863Z5.(TOOL BREAKAGE DETECTION)

M1

 

N8(DRILL CORNERS)

G0G40G49G80G90

T8(1.8MM COOLANT FED DRILL - NO. 50)

M6

M75

G17

G54G90B0.(FRONT TOOL PLANE)

G0G90X-.7419Y.9319S6735M3T15

G43H8Z.1M12

M198P1002(CALLS SUB PROG O1002)

M5

G91G28Z0.M9

G49

G90

M75

G65P9863Z5.(TOOL BREAKAGE DETECTION)

M1

 

N15(TAPL OUTER CORNERS)

G0G40G49G80G90

T15(NO. 8-32 TAPRH)

M6

M75

G17

G54G90B0.(FRONT TOOL PLANE)

G0G90X-.7419Y.9319S1024M3T13

G43H15Z.1M8

M198P1003

M5

G91G28Z0.M9

G49

G90

M75

G65P9863Z5.(TOOL BREAKAGE DETECTION)

M1

 

N13(EDGE BREAK)

G0G40G49G80G90

T13(3/64 FLAT ENDMILL)

M6

M75

G17

G54G90B0.(FRONT TOOL PLANE)

G0G90X.6361Y.1328S5570M3T1

G43H13Z.25M8

G5P10000

M198P1004(CALLS SUB PROG O1004)

M5

G91G28Z0.M9

G5P0(HPCC OFF)

G65P9863Z5.(TOOL BREAKAGE DETECTION)

G90

M99

 

 

O1001(T1 * 1/2 FLAT VARIMILL ENDMILL * CONTOUR)

G0G90X1.7689Y.5859

Z.25

Z.1

G1Z0.F10.

X1.2689

G3X.7689Y.0859I0.J-.5

Z.1

G0Z.25

M99

 

 

O1002(T8 * 1.8MM COOLANT FED DRILL - NO. 50 * DRILL/CBORE)

G0G90X-.7419Y.9319

Z.1

G99G81Z-1.R.1F2.83

X.5189

Y-.7601

X-.7419

G80

G0Z.1

M99

 

 

O1003(T15 * NO. 8-32 TAPRH * TAP)

G0G90X-.7419Y.9319

Z.1

M5

M19

M33S1024

G99G84Z-1.R.1F.0313Q.125

X.5189

Y-.7601

X-.7419

G80

G0Z.1

M99

 

 

O1004(T13 * 3/64 FLAT ENDMILL * CONTOUR)

G0G90X.6361Y.1328

Z.25

Z.1

G1Z0.F3.

X.5893

G3X.5424Y.0859I0.J-.0469

Z.1

G0Z.25

M99

%

---

HTH

[bigjohn]

quote:

---

do a xform rotate with subprogram operation after the operation that does the machining.

---

Thanks Dolphin1

[Rick46]

quote:

---

 

 

quote:

--------------------------------------------------------------------------------

...is this mpsubrep post that you updated going to be availaible for public use?

--------------------------------------------------------------------------------

 

Right now it's machine specific (Toyoda HMC with a full 4th) so I don't imagine it would work for everyone so in a word no, it's not for public consumption. If a reseller were to contact me and request it for one of their customers I would happily part with it but end users... no sorry.

---

just thought I would ask. thanks anyways cnc apps guy ..

[B.Srinivas Rao IME Traing sdn bhd]

Hi Guys,

 

The subprograming codes are ISO standerdised so any machines they are same, the codes G98 is for Calling suprogram and G99 End of subprogram.

So the main program will have M98 with program no. and noof repets.

 

You can out put sub programs in mastercam for countur/pkts also by just clicking the icon onthe Depthcuts -> check the botton on for sub programs you can see the codes.

 

The Advantage of subprograming is to reduce the length of the program.

 

Hope this info is usefull.

 

Rao

[B.Srinivas Rao IME Traing sdn bhd]

Hi Guys, please refer G98/G99 as M98 and M99

 

Rao

[Guest CNC Apps Guy 1]

Hey Rick, another reason it's not for public distribution right now is the post is not ready for prime time. There's a lot of errors (so far nothing affecting the ourput I need) but definitely someting I need to go line by line on when I get some time to do some serious debug time. It's probably going to need a few more hours.