What's new
What's new

Fadal cutter comp. issue

garychipmaker

Cast Iron
Joined
Dec 2, 2005
Location
ia
Hi guys I haven't used cutter comp much but I don't know what I did wrong here I get error cutter dia. too large @ N45 Thanks for the help. I find examples in the manual but they aren't using a fixture offset. I have the cutter dia. entered as .380 a .375 +.005. The machine stops @ X.-190 Y.190 I think it was so it did pick up the cutter comp.
N5 609
N10 G0 G17 G40 G70 G80 G90 Z0 H0
N15 M6T4 S4000 M3
N20 E2
N25 H4 D4 Z1.
N30 G1 Y.25 Z.995 F10.
N35 G41
N40 G1 X0 Y0 F10.
N45 G1 X2.625
N50 G2 X3. Y-.375J-.375
N55 G1 Y-2.375
N60 G2 X2.625 Y2.75 I-.375
G1 X1.375
G2 X1.375 Y0 J1.375
G1 Y.25
 
Last edited:
I had this once, toolpath radius might be smaller than your cutter dia. After changing my toolpath I could use the G41 or G42 for tool comp.
 
Hi guys I haven't used cutter comp much but I don't know what I did wrong here I get error cutter dia. too large @ N45 Thanks for the help. I find examples in the manual but they aren't using a fixture offset. I have the cutter dia. entered as .380 a .375 +.005. The machine stops @ X.-190 Y.190 I think it was so it did pick up the cutter comp.
N5 609
N10 G0 G17 G40 G70 G80 G90 Z0 H0
N15 M6T4 S4000 M3
N20 E2
N25 H4 D4 Z1.
N30 G1 Y.25 Z.995 F10.
N35 G41
N40 G1 X0 Y0 F10.
N45 G1 X2.625
N50 G2 X3. Y-.375J-.375
It would help if your were to list more of the program after N50, as an error may be raised before the actual problem area due to the Look Ahead in Cutter Radius Comp. However, lets say the next move after N50 isn't causing an issue, because the Tool Path is going around the outside of the Radius Feature, the cutter diameter can't be too large for the Radius Feature.

Are you sure that the cutter offset data should be registered as Diameter and not Radius? If its supposed to be in Radius, then that would be a viable explanation for your issue because there is only 0.25 in Y to apply a 0.380 offset if the control is treating that value as Radius.

Its also better form to include the G41/G42 Cutter Radius Comp start up commands with an end target coordinate; as in the following example:

N35 G41 G1 X0 Y0 F10.

Regards,

Bill
 
Even though Fanuc does not have this limitation, some controls may require that the startup move in radius compensation should be longer than the radius of the tool, along both axes.
 
I didnt find the issue yet. I was just posting that I added the rest of the program that wouldn't run as angelw had asked me to do. I'm @ my real job today till 8p.m. so I'll try when I get home.
 
I didnt find the issue yet. I was just posting that I added the rest of the program that wouldn't run as angelw had asked me to do. I'm @ my real job today till 8p.m. so I'll try when I get home.
With the additional code listed for your program, I suspect you have a typo when listing the program on the Forum, as the "Y2.75" in N60 G2 X2.625 Y2.75 I-.375, should be Y-2.75 for the tool path to work.

Your tool path is fine (with N60 G2 X2.625 Y-2.75 I-.375) ; accordingly, your issue will be the Cutter Radius Comp start up distance is less than the specified Radius of the Tool being used. This would point to the Tool Data registered for use in Cutter Radius Comp should be specified in Radius and not Diameter. In your case, the 0.380 that you have specified as the Diameter of the cutter, is being regarded as Radius by the control.

As a test conducted in fresh air, modify your program as follows:

N30 G1 Y.25 Z.995 F10.
N35 G41 G1 X0 Y0 F10.
N45 G1 X2.625

and register the Tool Radius Comp value for D4 as 0.19.


Regards,

Bill
 
Update parts are done I made the changes angelw suggested to put the xoyo on the same line as the G41, my machine uses diameter in the tool catalog so that part was fine
 








 
Back
Top