[venomgrrrl]

Not shure if this is an appropriate quetion, but i could use an example of a circular interpolation, with Fanuc 0-M, My programming skils are a tiny bit rusty and i need to make a 2" hole in a bracket. I do recall I,J,K's but with no recolection of how to apply.

[dcoupar]

(PUT RADIUS OF CUTTER IN D51)
G00 G90 X0 Y0 (MOVE TO ABSOLUTE CENTER)
G01 Z-0.5 F2.5 (PLUNGE FEED TO DEPTH)
G41 G91 X1.0 D51 F5.0 (FEED +1.0 IN X & TURN ON COMP)
G03 I-1.0 (CUT FULL CIRCLE BACK TO START - CENTER -1.0 AWAY IN X)
G01 G40 G91 X-1.0 (FEED BACK TO CENTER &CANCEL COMP)
G00 G90 Z0.1 (RAPID OUT OF HOLE)

[venomgrrrl]

It seems that i do not have a D51, in my controls...for that matter no way that I
know to set any tool dia's

[Geof]

It seems that i do not have a D51, in my controls...for that matter no way that I
know to set any tool dia's

Omit the G41 D51 and simply subtract the radius of the cutter onto your X move and the I value. This means you cannot adjust the size by using a wear value you have to edit the X and I for adjustment.

[venomgrrrl]

I was under the assumtion that I could just program in D#, correct me if im wrong (my brain is set on "monday")

[CNCRim]

http://www.box.net/shared/23bqyxhzxm

This manual give you mental pix and explain..... all you need to know about CNC programming.

[HuFlungDung]

I hope someone familiar with this control will chime in, but it could be the case that your older control does not have seperate H and D offset registers. They might all be in one register (H?)

In that case, when you need to store a radius value for a tool, you'll need to do it further down the list. For example, if you have a 20 tool magazine, then you can store the H offset from tool1 to tool 20 in the first 20 positions in the offset register, then store tool diameter (or radius) values from 21 to 40 in the offset register.

You'll have to keep this in mind when programming, so that you call H1 for tool 1 length offset, and (perhaps) H21 for radius offset for T1. Someone who knows, please add your comments!

A newer controller would have seperate registers for H and D so then H1 and D1 would normally be associated with T1.

Fun, no?

[Zuma]

Under your offset page is where you will put the value. The H's and D's both come from that screen. If memory serves me correctly, depending on how a parameter (5001.2 for 16i don't know which one for O) is set is whether you use an H or a D for diameter offset. Which means it might be:
G41 G91 X1.0 D51 F5.0 or
G41 G91 X1.0 H51 F5.0
and the value is place in offset 051 (or what ever offset number you like)
Just remember that if you are using H1 for a length offset, don't use D1 for a diameter offset.

[venomgrrrl]

so correct me if i am wrong but I program in the D51, then in my offset pg in # 51 I can imput my Diameter,
The H value works according to tool, ex. T16 = H16, and it pulls its info from offset tool length #16
Is 51 the only Dia setting I have?
Sorry for all the quetions...and none the solutions





BTW
( my offset page only has 2 colums 1= No. and second= Data, where i imput according tool length, just incase that is unclear)

[Zuma]

You can use any offset for any data. Most people use H1 for tool 1 length, H2 for tool 2, etc... just to keep it simple. The offset for length is called up in your G43 line. Ex: G0G43Z1.0H1 You don't have to use H1 for tool1. you could use H53, but this would get confusing for your operators. What I like to do for a little 10 tool machine we have is I will use H1-H10 for tool lengths, and D21-D30 for Diameter comps. (my parameter is set to use D for dia. comp. not H) all of the values (data) are put into the offset table under the correct number field. So 001 would have a tool length value in it such as 5.732, and 021 would have a diameter value in it such as .005 which is the value of the difference between programmed tool size and actual tool size. I program actual tool size. I will tell the operator what size tool to use and he will mic it and put in the difference in the offset table. So my program would have lines in like this for tool 1:
G0G54X0Y0
G43Z.1H1
Z-.5
G1G41X.625D21F10.
G3X.625Y0I-.625J0
G1G40X0F100.
G0Z1.
etc...

[venomgrrrl]

Wow, this is relly...um...fun, according to dryrun I am now succsefully milling a hole of some size..somewhere, wich may sound bad, but I was thinking this m/c could only drill and tap...so im leaps and bounds ahead of where I was yesterday!
I am currently trying to get away with out programing cutter comps as my hole size (for now) is not as important as just making the freakin hole! LOL
Newtexas thanx so much for the Haas manual...im will keep that link to forward onto others BTW haas manual is like going back to CNC school!
Because my current program is so weak im not going to post it until I work out some more *bugs* (I dont want to shame myself, LOL)
But I will post the results when I get some

Thank you all sOO much
Stephanie!