Corner Rounding on TM1

having trouble with the corner rounding on our haas tm-1. i used to run a bridgeport with prototrak controls, and when ever i was profile milling (x and y only) when ever going around a corner i would program a .020 conrad. so that there was no burr or sharp corner. when reading in the haas manual i find what im lookin for, but it doesnt do work. i even copied the example right out of manual and it doesnt work. is there a parm or a setting i need to turn on? and if so please would someone help me out. the example in the manual shows either a R value, for radius, or a C value for a 45deg. corner champfer at the end of a G01 line (G01X3.00Y.0R.02F50.) but nothing happens.

are you using cutter comp?

i've tried with comp and with out. no luck. makes it a longer proces to figure out tan. points and use a g02 or g03

Are you putting the line with the R or C value between G01 commands that do not have this included? The way I read the manual it seems that just putting one line with the C or R may not work.

you have to make sure you've got a G02 or G03 in the line that you want the radius to occur, otherwise it won't read that R move.

Quote:

---

Originally Posted by rbest27

you have to make sure you've got a G02 or G03 in the line that you want the radius to occur, otherwise it won't read that R move.

---

It appears that Haas has now included corner rounding or chamfering as one of the moves that can be done using G01. I copied this from the Haas Mill Manual with the picture below.

A chamfer block or a corner-rounding block can be automatically inserted between two linear interpolation blocks by specifying ,C (chamfering) or ,R (corner rounding). There must be a terminating linear interpolation block following the beginning block (a G04 pause may intervene). These two linear interpolation blocks specify a corner of intersection. If the beginning block specifies a C, the value following the C is the distance from the intersection to where the chamfer begins, and also the distance from the intersection to where the chamfer ends. If the beginning block specifies an R, the value following the R is the radius of a circle tangent to the corner at two points: the beginning of the corner-rounding arc and the endpoint of that arc. There can be consecutive blocks with chamfering or corner rounding specified. There must be movement on the two axes specified by the selected plane, whether the active plane is XY (G17), XZ (G18) or YZ (G19).

R U Sure You Put The "," Before The C Or R?

Quote:

---

Originally Posted by big_mak

R U Sure You Put The "," Before The C Or R?

---

Why " " ? The example from the Mill Manual just has C or R followed by a dimension.

If you look at the pic, there is a "," just before the C or R even in the tesct that you sent it's ,C or ,R

Sorry, I misread your post. I though you wanted " " but you meant "comma" :o

I see now; in the picture it is ,C or ,R in the text it has both ,C and C, and ,R and R,

Does it work on your machine?

Did you have a contination move in the non motion axis and direction of your corner rounding in the next line. If you want to make a radius in the "X" posiitive direction at the end of a "Y" axis move as in line N110 then the next line must have an "X" value at least the value of "R" + .0001 larger than the "X3." start point. This works only on 90 deg corners.

N100 G01 X3. Y0.
N110 Y3. R.02
N120 X3.1 (this line needs positive move in X at least .0001 larger than the R word)
N130 Y4. R-.02
N140 X2.9 (this line needs negative move in X at least .0001 larger than the R word)

I think the ",R/C" allows 2 lines at 90 degrees and also not at 90 degrees to be joined by a C/R word but the same continuation principals apply. I think the ",R/C " is pretty new though we don't have it on any of our older controls.

i think the "," is where my problem lies. i will try it again today at work. i really would like to thank everyone here for all your help. this forum really has helped make me a better machinist. as far as the continuied, yes there is one. i full understand how it works, as i used it for yrs on a prototrak control. just was having trouble getting it to work. but i really think its that little coma that was hanging me up. never noticed it before. never used a coma in a line of code. i hand g-code almost everything, i do cam some stuff but im still trying to teach myself mastercam.