Radius??

[Tuz]

I have a Heian Router 180im-b Fanuc Controller

I am trying to take a standard downshear bit and do an x,y,z, movement while also following a specified radius. Then follow it back up the same way it came down.
I have been told by a few different people it can't be done. But it seems so simple??
I have come up with nothing but error messages though when trying myself.
Help anyone??

[ProProcess]

Not really sure about the control or machine put it sounds like you are trying something more complicated than you think. Especially if your control is erroring out.
Sounds like you want to move from XYZ point A to XYZ point B, all the while generating a radius. If that is the case you either need to generate the path using CAD/CAM or author your own macro to calc the XYZ per any given step along the radius and interpolate to that point then calculate again.

[Tuz]

I want to go from X2.25 Y2.25 Z .3865 to X 2.444 Y 2.444 Z-.2615 while following a .219 radius then back again.

[ProProcess]

What (G17-G19) plane are you in?
Does your machine have Helical interpolation?

[Tuz]

g17.

How can I tell if I have that option or not. I have some experience but not a whole lot.

Thanks!

[beege]

If you want the radius to be in the XY plane and ramping up and down (straight line from the side) you need to have helical interpolation turned on. You just might. If you want your radius to be in a plane other than XY, XZ or YZ, then helical will still work, but you need to change panes (G17, G18 and G19) Any other planes, you need coordinate rotation (maybe it would work, never tried it) AND helical interpolation. Other than that, have someone write some code from their CAM system in pure linear that you could cut/paste in your program.

[Tuz]

tHE BOLDED PART IS WHAT I AM WORKING ON...

N10G0G17G20G40G49G80G90Z0
M211
M400
M401
T3M6
G08P1
N20G54M91S20000X[#500-3.0]Y3.155
N30G43H3Z.25
G42D19
G90G1Y2.155F150.
N40G1G90Z-.3865X[#500/2]F243.75
X2.155F325.
N50Y[#501-2.155]
N60X[#500-2.155]
N70Y2.155
N80X2.9175
N90G40G49G0G64Z0M95
M400
M402
T3M6
N100G55M91S20000X[#500-3.0]Y3.155
N110G43H35Z.25
G42D51
G90G1Y2.155F150.
N120G1G90Z-.3865X[#500/2]F243.75
X2.155F325.
N130Y[#501-2.155]
N140X[#500-2.155]
N150Y2.155
N160X2.5575
N170G40G49G0G64Z0M95
M400
M401
T4M6
G54M91S20000X[#500-3.0]Y3.155
N190G43H4Z.25
G42D20
G90G1Y2.155F150.
N200G1G90Z-.125X[#500/2]F187.50
X2.155F250.G61
N210Y[#501-2.155]
N220X[#500-2.155]
N230Y2.155
[B]G91G2X.194Y.194R.219Z-.2615
G3X-.194Y-.194R.219Z.2615
N240G1X2.2331
Z1.0
G0G40X6.Y6.
N250G0G49G64Z0M95
M12
M22
/G53Y0
N260G08P0
/M212
M99

[ProProcess]

g17.

How can I tell if I have that option or not. I have some experience but not a whole lot.

Thanks!

Run this code or something like it.

G17
G0X0Y0Z3.
G1G91X1.F50.
G2I-1.(THIS.SHOULD.RUN.FINE)
G2Z-.1I-1.(THIS.WILL.ONLY.RUN.WITH.HELICAL)
G1G90X0

[Tuz]

Thanks for your reply,what will this tell me when I run that code? What am I expecting it to do?
I run can run a program like this: (Is this Helical?)

N20G55M3S18000X3.75Y2.75
N30G43H24Z0.25
N40G1Z-0.4F100.
N40G62G91G2J1.F200.
G2J1.F400.
G2J1.Z0.5F400.G61
G90X3.75Y3.125
G1Z-0.4F100.
G91G62G2J0.625F200.
G2J0.625F400.
G2J0.625Z0.5

[ProProcess]

Thanks for your reply,what will this tell me when I run that code? What am I expecting it to do?
I run can run a program like this: (Is this Helical?)

N20G55M3S18000X3.75Y2.75
N30G43H24Z0.25
N40G1Z-0.4F100.
N40G62G91G2J1.F200.
G2J1.F400.
G2J1.Z0.5F400.G61
G90X3.75Y3.125
G1Z-0.4F100.
G91G62G2J0.625F200.
G2J0.625F400.
G2J0.625Z0.5

I'm not a mill guy so I'm not sure what the G61 and G62 are doing but...

if these lines...

G2J0.625F400.(cut a circle using XY)
G2J0.625Z0.5(cuts the same XY circle while moving in Z)

then you have Helical and you "should" be able to do what you want.

Provided that the Sarting point A and Ending point B are valid starting and ending points along the selected plane at the given radius.

Good Luck!

[Tuz]

If I start at X 2.155 Y 2.155 Z-.125 and I want to go to X 2.349 Y 2.349 Z -.3865 while following the .219 radius will this work??

G91G2X.194Y.194J.194Z-.2615
G3X-.194Y-.194J-.194Z.2615

Where does the radius call out go?

Sorry I am failry new to all this, and I have no cad software to work from. I learn as much as I can by writing them by hand. But I am running out of time to complete this project.
Thanks for your help!!

[dcoupar]

If you use I and J to specify the distance from start to center, you don't need a radius call out. I'm pretty sure your above example will not work (it will create a 3/4 moon shape). J.194 in the G02 block puts the center +.194 in Y from the start point. J-.194 in the G03 block puts the center -.194 in Y from the start point.

I would replace the J.194's with R.219's. I back plotted it and it worked fine with R's.

What alarm are you getting?