O/T: Radius programming

[RStuart]

I'm sorry to bother you guys with something so simple, but I was looking through some posts and just comparing and I posted a file for Okuma mill, which we have, and one for a HAAS mill which we don't have. I see in the HAAS post it uses I and J in the radius. I have seen these before, but unfortunately have never had the oppurtunity to use them. Upon comparing the two I really couldn't figure out where these I and J numbers were comming from. Could someone clue me in.

[gcode]

Normally I and J represent the incremental

distance to the center of the arc from the start of the arc.

[RStuart]

I being x and j being y or vise versa?

[crazy^millman]

These for the most part are the incremtal distacne from the end of the arc to the center of the arc. draw square where the center is the orgin. Make the square 4" outside. Then put 1" fillets on each corner. Then do a contour toolpath no cutter comp. Thne post the code and I think it will make more sense to you. The distance is from the end of the arc becuase you already have the beginning because that is where you started.

 

Here is that code.

code:

---

G00 G90 G154 P20 X-2. Y1.

G43 H8 Z.8

Z.73

G01 Z.63 F5.

Y-1.

G03 X-1. Y-2. I1.

G01 X1.

G03 X2. Y-1. J1.

G01 Y1.

G03 X1. Y2. I-1.

G01 X-1.

G03 X-2. Y1. J-1.

---

I also find that this gives you much tigher and better looking 3d surface machining that trying to use R for the posts.

 

Hope that is right and makes sense.

 

[Tim Aydt Prototek Engineering]

I is associated to the X location

J to the Y

K to the Z ( helical arcs)

[crazy^millman]

Tim or K to Z for G18 plane or G19 plane arc moves not just helical moves but can be arc moves in different planes as well.

 

 

HTH

[Teh Bear without Brains kinda idiot]

I and J preferable ,JMHO ,especially on Sinumeric when it gets crazy with message error arc calculation or sorta .

I and J are less informative ,butthis is little thing I trig fast in mind (LOL).

 

JM@D

[BernieT]

There is a question in the post processor that allows you to use either R or I, J, K for arcs. Some time ago we had a discussion on which is best. I strongly prefer I, J, K. I also don't like 'Break arcs into Quadrants'.

[gcode]

quote:

---

I also don't like 'Break arcs into Quadrants'.

---

Some older controls require this feature.

They do some real ugly stuff if you try a 90+

degree arc with one block of code.

[Roger Martin from CNC Software]

Read the quotes closely...

 

quote:

---

Normally I and J represent the incremental distance to the center of the arc from the start of the arc.

---

quote:

---

These for the most part are the incremtal distacne from the end of the arc to the center of the arc.

---

Not to bust anybody, but....

 

Usually (since there are always exceptions when talking about CNCs!) the 'I' (X axis) & 'J' (Y axis) values are the incremental distance from the start of the arc to the center of the arc.

 

 

From MPFAN.PST (and MPMASTER.PST) ->

 

Note the "direction" is set with the 'arc type' variable. (2 = START to CENTER)

 

code:

---

arcoutput   : 0     #0 = IJK, 1 = R no sign, 2 = R signed neg. over 180

arctype : 2 #Arc center 1=abs, 2=St-Ctr, 3=Ctr-St, 4=unsigned inc.

---

and...

quote:

---

I also don't like 'Break arcs into Quadrants'.

---

If your machine does not need this, don't break at quadrants, 'cause it's not doing anything for you except making additional NC code. But, it you are running 'R'adius format instead of I&J - be careful about changing ->

 

breakarcs : 2 #Break arcs, 0 = no, 1 = quadrants, 2 = 180deg. max arcs

 

 

If this switch in your PST is set to '1' and you change it to '0', you may have problems when using the 'R' arc format. You'd want to either: Leave this setting alone or change it to '2'.

[Thad]

quote:

---

Usually (since there are always exceptions when talking about CNCs!) the 'I' (X axis) & 'J' (Y axis) values are the incremental distance from the start of the arc to the center of the arc.

---

I noticed the previous posts also, but I just wasn't in the mood to rattle anyone's cage. Thanks for pointing that out, Roger.

 

Thad

[crazy^millman]

Thanks Roger had that backwards in my head for some reason but it all good. Gald you corrected my mistake sorry about that guys. Yeah I also just cut soem tooling board about 4" to short for a tool so just one of them days I guess.

 

Dooooooooooooohhhhhhhhhhhhhhhhhh

 

Just alwasy think of it as where I want the arc to quit at and just had it in my head as ushc espically since on most machine you only need the I and J to make a full circle and nothing else. Thinking to myself if it is the start then how can it be the end also so just without thinkign ad going back and reading my note put up what I thought was the right answer oh well not the first and will not be the last mistkae I make can promise you that.

[Nominal]

Since we're being picky.

I've seen it as an incremental distance from the start of the arc to the center, from the center of the arc to the start, and as an absolute position. For example Allen Bradley ( remember those? ) could use a G75 76 and 77 to give you either of all three methods.

[Teh Bear without Brains kinda idiot]

If you say g3 x3 y6 r5

your machine controller will check ,if the arc possible to build with R5 through two points _start and end

If it is not (radius less than a distance between points/2 ,for example )controller will check a difference and if it will be greater then possible aprovable in controler parameters settings even for 0.00001 you will get an alarm and go correct in 3 d movements 10-50 arc movements or start to check controller side and tweek post ,even for such a difference while setting I and j ,or k and so on machine will calculate radius and you will never get alarm .

That`s one of the reasons ,there are others .

HTH

WTHH