multiple set-up

[mold100]

Hey hows everyone doin,I got a little problem,mill level 3,v8.We just got an erowa pallet system,and on one of the plates i mounted 4 electrode holders.I am using a Makino snc64 with a fanuc 16i control pro a.I a have them stored as g54-g57,what is the best way to make my program cut all four locations without copying my geometry to the locations or the toolpath,Is this where i should use subprogramming,in which with mastercam I have never tried.Thanks ahead,and sorry about the lengthy post

[Jack K]

Try going into your operations manager the going to toolpath/transform from there you a can run mulitple workstations without coping or transforming as you know it.

[gcode]

I'd download the subrep post on this website and use it.

Use the MISC box on your first OP to tell it how many repeats you want.

 

It will break your program into subroutines

and call them using G54, G54 etc.

[Michael Reynolds]

I'm sure Gcode meant to say "mpmaster" post.

 

Mike R.

[Jim Evans from CNC Software]

Mold100,

 

You can accomplish this using Mastercam and the Transform operation, however your post processor must be set up to handle Mastercam's subprogram output. MPFAN will handle this as will MPMASTER.

 

The transform operation has many options that you should become familar with. I suggest doing an example of what you are trying to do and experiment with the settings such as copy source, work offset and output order. Make sure your tranform method is toolpane.

 

Give it a try and if you have any questions, just holler!

Jim

[gcode]

No,

I meant the Multiple Offsets post on the post page

on this web page. Its name is mpsubrep.pst

Try it, it works very well!

[Greg Williams]

Mold 100

 

If I have 4 electrodes all the same I remove the G54 from the program replace the M30 with M99, Making the program a subprogram, then I write a simple main program like

 

G90G80G40G17

G91G28Z0

G28X0Y0

G54

M198P1

G55

M198P1

G56

M198P1

G57

M198P1

G91G28Z0

M30.

 

M198 will call the program from the hard drive of a Makino professional 3 controller(Not sure about a Pro A). If you don't have the Hard drive option use M98

[Jack K]

Again, I think transforming is the way to go!

Set T/C Plane - tool plane in your parameter page to 1

Operation manager / toolpath / tansform

page type & methods

type= translate

method = tool plane

group nci output by = operation type

copy source operation

diable posting in selected operation

subprogram

work offset numbering = assign new

start = 1 (g54)

increment= number of offsets

translate

change x & y spacings and steps to suit!

This works nice and simple no editing no programs to write longhand.

[mold100]

Thanks to all who replied and I have been pretty busy and havent had much time to spend here.But hopefully youll hear more from me.If I can throw my .02$ in anywhere.

[gary dunn]

just set each position as an offset number ie (G54, G55, etc.) in the machine and make the program a sub program and call it on each position. simple and clean.

we use erowa fixtures. but we also get the offset of the part from the center of the fixture.

 

using transform toolpath doesn't always work unless we add the offset to each position.

[Allan Brown]

Pointing out a related thread:

 

http://www.emastercam.com/cgi-bin/ultimate...ic;f=1;t=001807

 

Not sure if the FTP link is still valid. I'll try to update it.

[cadcam]

Hi dave, i tred the link from this old page took me rith ti the FTP .

How about you.are you at all able to get to the FTP?

[Allan Brown]

Outside of our firewall, yes. From within our firewall, no.

[Bob B]

hi all,

i need to download the multiple offset post but am running version9. i noticed the posts page only has version7 & 8, what do i do?-is it possible to use the ver8 in my ver9?

thanks for any help in advance. take care.

-bob

[Allan Brown]

Check for a V9 update. Really the "new method" the most up to date way to handle this.

[gcode]

Bob,

Run the V8 post through the V9 update chook.

[Bob B]

thanks dave, gcode!

i'm going to try to figure another way around my offsets problem before i go screwing up the good post we're using here.

thanks again.

-bob

[gcode]

Bob,

The V9 post you require is available here.

 

http://www.emastercam.com/posts/

[Bob B]

got it, thanks gcode.

 

-bob