[hkfanatic]

ok im haveing a stupid beginner problem thats causeing my brain to melt.

im trying to cut a 180deg radius on the out side of a blocks sides

heres the blocks dimensions x 2.5 y 1.0 z 3.0

zero is in the dead center of the block.

im useing a 1.0dia endmill

heres how im programming it.

(starting at zero Assuming m3 and etc.. has been done)

N001 G0 Y-.938
N002 G01 Z-1.0 F2.0
N003 X1.250 (THIS IS WHERE THE ARC WILL START FROM)
N004 G03 Y.983 R1.001 (i want it to do an arc the same spot on the op side)
N005 G01 X-1.250
N006 G03 Y-.938 R1.001
N007 G01 X 0.0

so essentially it cut an oval shape into the out side of the block 1 inch deep

my machine acts like its a G01 cammand and doesent arc.

im not too proficiant at Gcode they only touched on it in school.

help!

thanks

[CNCRim]

ok im haveing a stupid beginner problem thats causeing my brain to melt.

im trying to cut a 180deg radius on the out side of a blocks sides

heres the blocks dimensions x 2.5 y 1.0 z 3.0

zero is in the dead center of the block.

im useing a 1.0dia endmill

heres how im programming it.

(starting at zero Assuming m3 and etc.. has been done)

N001 G0 Y-.938
N002 G01 Z-1.0 F2.0
N003 X1.250 (THIS IS WHERE THE ARC WILL START FROM)
N004 G03 Y.983 R1.001 (i want it to do an arc the same spot on the op side)
N005 G01 X-1.250
N006 G03 Y-.938 R1.001
N007 G01 X 0.0

so essentially it cut an oval shape into the out side of the block 1 inch deep

my machine acts like its a G01 cammand and doesent arc.

im not too proficiant at Gcode they only touched on it in school.

help!

thanks

N001 G0 X0 Y-.938 (Insert start position)
N002 G01 Z-1.0 F2.0
N003 X1.250 (THIS IS WHERE THE ARC WILL START FROM)
N004 G03 Y.983 R1.001 (Typo should be Y.938)
N005 G01 X-1.250
N006 G03 Y-.938 R1.001
N007 G01 X 0.0

[hkfanatic]

thanks, that was'nt a direct copy of my program (i've read through it there are no typos, at least none that i've found yet i'll go back through)

my concern was that im not inputing the right perameters for the G03 command do i have to dictate X on that line as well???

i have this: N004 G03 Y.983 R1.001

should it be: N004 G03 X1.250 Y.983 R1.001 ???

[scadvice]

Most of my programming is via CADCAM now, but every once in awile I will hand input a program (25 yrs of it) And.... I still can get caught on a simple error that is stareing me in the face... S### happens...
This forum is a good way to fix being stupid ...grin...and save the blood pressure and alot of time when we brain fade! Steve

[beege]

ok im haveing a stupid beginner problem thats causeing my brain to melt.

im trying to cut a 180deg radius on the out side of a blocks sides

heres the blocks dimensions x 2.5 y 1.0 z 3.0

zero is in the dead center of the block.

im useing a 1.0dia endmill

heres how im programming it.

(starting at zero Assuming m3 and etc.. has been done)

N001 G0 Y-.938
N002 G01 Z-1.0 F2.0
N003 X1.250 (THIS IS WHERE THE ARC WILL START FROM)
N004 G03 Y.983 R1.001 (i want it to do an arc the same spot on the op side)
N005 G01 X-1.250
N006 G03 Y-.938 R1.001
N007 G01 X 0.0

so essentially it cut an oval shape into the out side of the block 1 inch deep

my machine acts like its a G01 cammand and doesent arc.

im not too proficiant at Gcode they only touched on it in school.

help!

thanks

I'm not sure what you're trying to end up with here.
Y-.938 is going to take .062" from the minus side of your block.
X1.25 is going to put the cutter centerline on at the edge of your block
G03 Y.938 R1.001 is going to cut air to the far edge of your block
G01 X-1.25 puts the centerline of the tool again on the left edge of the part, taking .062" of material with it. (Finish dimension of the block (Y) will be .875)
G03 Y-.938 cuts air again to the near left corner
G01 X0 will finish the circuit, and take the rest of the .062 from the block.

Are you STARTING with a block that size, or are you FINISHING withthe block that size?
Do you want convex arcs on the ends, or concave? (concave gives you very sharp corners, the other doesn't).

Perhaps a better description of what you want is needed, as well as what you're starting with.

Good luck, lotsa brains to help in here.

[scadvice]

A little more detail... Steve

[tauntdesigns]

If I got this right you are setting the X,Y zero in the center of the block(1.25 from left edge of part and .5 from the lower edge) and wanting 1. radius starting at the bottom edge to top of part then a .5 flat on top and then 1. radius to the bottom edge again.

The z move at 2." a min may be a slow air cut but here's my code for it. It comes to the right bottom of part then ramps onto the part with a G2 move then cuts a G3 move cutting the radius then G1 move to the start of the next G3 radius cut and then a G2 move ramping off part.

g0x2.y-.5
g1z-1.f2.
g2x1.75y-.5i-.125j0
g3x.25y1.i-1.5j0
g1x-.25
g3x-1.75y-.5i0j-1.5
g2x-2.y-.5i-.125j0
g0z0
m30

Hope this helps,
Jack

[tauntdesigns]

After re-reading your post........are you looking for a .5" radius or 1" radius?

a picture would help(even if drawn with pen)

I also notice you were using R's.......... I used I&J incremental

[scadvice]

also tell us what control your using. S

[tauntdesigns]

thanks, that was'nt a direct copy of my program (i've read through it there are no typos, at least none that i've found yet i'll go back through)

my concern was that im not inputing the right perameters for the G03 command do i have to dictate X on that line as well???

i have this: N004 G03 Y.983 R1.001

should it be: N004 G03 X1.250 Y.983 R1.001 ???

I missed this post!

G2 and G3 need an X and Y unless your finishing point is the same as your starting point.

The X and Y is the finish point of the move (telling it where to go)
The I,J describes the distance to the center of arc from the starting point.(I being X direction and J being Y direction)
R describes the radius

Is that what you wanted.

Cheers,
Jack

[hkfanatic]

ok a little more info is definetly needed. im posting a pic of the finished part the reason the radiuses are cutting air and only skimming the corners is because its a progressive cut inward to help keep deflection and tool breakage down, its cutting mild steel and im running 2 ipm just to keep things slow right now once i get the program right i'll mess with the feed and speed.

heres a pic of the finished part, zero is at x1.25 y .5 from the left lower corner. the reason is at one point there is a peck drill cycle to drill the center out and its just easier (at least for me to do it that way)




the final diameter/ thickness of the parts is .630, the shelf is going to be done with a shell mill so i can under cut the stock.

its the outside im haveing a problem with again the tool doesent want to arc it just go's straight and by the last post i think i know what it is i didint put the X starting point into the G03 command

its a bunch of counter clockwise circles takeing .062 off until final dimension, a tool change to a shell mill then the under cut for the shelf. tool change to a 3/4 end mill to do the peck drill in the center, tool change to a letter O drill and peck drill holes at x.75 and x-.75, tool change to a 1/4 end mill and circle mill holes to final dimension at .75 and -.75 at .525 deep

the slot happens afer i cut the parts off the block and reset fixtures

im useing a bridgeport BTC-1 with a 24 Atc fanuc control.

im useing an old copy of master cam i got from school but the program crashes when i tried to do the outside profileing so i wrote the code by hand and thats where im getting tied up.

hope this is a little helpfull, i REALLY need to start making some chips. i'll post the full program tonight when i get home if needed

[beege]

So it looks like the radius end points in X are all X.750, X-.750, to get them concentric with the drillled holes. X1.25 just won't do... I'm not giving you all the answers, just hints to help you learn...

[tauntdesigns]

[/QUOTE]
by the last post i think i know what it is i didint put the X starting point into the G03 command
[/QUOTE]

The X and Y in a G2 or G3 line is the finish point
Thr X and Y starting point is from where the arc cut starts

Example: The code I put in earlier just for example.......
g0x2.y-.5 Starting point (X&Y)
g1z-1.f2.
g2x1.75y-.5i-.125j0 (X,Y finish point)
g3x.25y1.i-1.5j0 (X,Y finish point)
g1x-.25 (this x moves to next starting point: Y is there already)
g3x-1.75y-.5i0j-1.5 (X,Y finish point)
g2x-2.y-.5i-.125j0 (X,Y finish point)
g0z0
m30

Cheers,
Jack
P.S. starting point is always the position of the spindle before the next G2/G3 move. Above: after the first G2 move, that position becomes the start point for the next G3 move.

[hkfanatic]

ok i think i realized what i might be doing wrong, when i orginally wrote the code i had the bit traverse from zero to X.75 then start the arc, but i didint compensate for the size of the tool so i added an extra 1/2 " if i go x.75 from zero with a 1in bit and then start and arc wouldent it shave 1/2" too much off? i think that was my reasoning behind it. mainly because when i got to X.75 it started going to Y-.938 with out cutting an arc and it broke my only piece of machineable wax

but as i think about it now haveing X go to .75 and y.938 then start the arc would remove the right amount of material anyways if i start the arc at x1.25 it really would cut nothing but air and would throw the whole thing off.

now then the G03 command should read like this inorder to make a half circle on the outside of the stock


Nxxx G03 X.75 Y-.938 R1.001

or because i compensated for the tool on the X dimensions i also compensated on the radius's, wouldent i need to revise those also???

[tauntdesigns]

This starts at the bottom left of part

G0 X-2.Y-.938
G1Z-1.F2.
X.75
G3X.75Y.9385I0J.938
G1X-.75
G3X-.75Y-.9385I0J-.938
G1Y-1.
G0X-2.
Y-.876
G1X.75
G3X.75Y.876I0J.876
G1X-.75
G3X-.75Y-.876I0J-.876
G1Y-1.
G0X-2.
Y-.815
G1X.75
G3X.75Y.815I0J.815
G1X-.75
G3X-.75Y-.815I0J-.815
G1Y-1.
G0X-2.Y-.938
G1Z-2. next Z depth
copy and paste above code between the 2 Z moves

I'm not real good with R's
Jack

[Abacus]

Been a awful long time since i had the need to program for arcs since its all 3d now but wth heres what i came up whether its right or wrong i dunno...

G00 G90 X1.5 Y1.5
G91 Y1.
Z0

SUB CALL

G1 Z-.062 F__?
Y-.185
X.935
G2 Y-1.13 R.815 (could be minus i forget with the G2)
G1 X-1.87
G2 Y1.13 R.815
G1 X.935
Y.185
rinse n repeat

Some controllers may not read R's (extra money feature) or if they are in absolute, then ya have to go with I's and J's.

[tauntdesigns]

I'll have to edit an earlier post where I was talking about the R (-) or (+) meaning something about direction. I couldn't remember the R stuff and it got to me, so I had to figure it out. I wrote some code and tried it with (-) and without and it didn't seem to matter.

Here's what I came up with....3 passes(.06", .06", and .059") I wrote it as if the middle area was uncut (sq block)

G0X-2.Y-.938
G1Z-1.F2.
X.75
G3X.75Y.938R.938
G1X-.75
G3X-.75Y-.938R.938
G1Y-1.
G0X-2.
Y-.876
G1X.75
G3X.75Y.876R.876
G1X-.75
G3X-.75Y-.876R.876
G1Y-1.
G0X-2.
Y-.815
G1X.75
G3X.75Y.815R.815
G1X-.75
G3X-.75Y-.815R.815
G1Y-1.
G0X-2.Y-.938
G1Z-2. (next Z)

I tried it in Mach3

I glad you asked the question, I had fun re-learning something I hadn't done in a while.

Jack

[beege]

I'll have to edit an earlier post where I was talking about the R (-) or (+) meaning something about direction. I couldn't remember the R stuff and it got to me, so I had to figure it out. I wrote some code and tried it with (-) and without and it didn't seem to matter.

Jack

The reason the sign on the R word doesn't matter here is because of the 180° arc. Less than an 180° arc requires a positive R value, and greater than an 180° arc needs a negative value.

I like to see CAPITAL address words, as that's all Fanucs can read (X0, not x0)
And on line 4 you have R.928 where it should be R.938, not that it's going to make a difference in the finished product.

Otherwise that program should work okay for the OP

[tauntdesigns]

Thanks,

I have always used I and J for my programs and had always wondered about the R rules.

Also, thanks for catching my oops (Capital & R.928).... I just typed it off the top of my head, and I need new glasses, yea, that's the story I'm sticking with...

Thanks again,
Jack
P.S. I'll go back and edit that post...... again, thanks for the catch.

[hkfanatic]

ok thank all of you guys that helped out i really appreciate it. im posting my complete program for those of you who have the time to go through it and tell me what i may have missed, from tool 3 on it was done with mastercam.
i didint have a shell mill that was shallow enough to do the under cut for tool 2 but i put a 3/4" end mill with a 1/2" shank on the precision grinder and cut a flat shoulder on it so i hope that will work. all of the T/# is for my machines tool length offset its how it wants you to imbed it into the programming so it can understand it. (for those that may be wondering)

here it is! ZERO is in the very center of the stock (from lower left corner x1.25 y.75)

(FORWARD ASSIST )
(DATE=DD-MM-YY - 14-07-08 TIME=HH:MM - 09:01)
(MCX FILE - C:\DOCUMENTS AND SETTINGS\TECHUSER05\MY DOCUMENTS\INVENTOR\WORKSPACES\PROJECT1\FORWARD ASSIST HOUSEING\HOUSEING READY TO BE MACHINED.MCX)
(NC FILE - C:\MCAMX\MILL\NC\FORWARD ASSIST DONE.NC)
(MATERIAL - MILD STEEL 1X1)
( T1)| 1.0 FLAT ENDMILL | H0 )
( T2)| 3/4 FLAT ENDMILL NO SHOULDER | H0 )
( T3 | 3/4 FLAT ENDMILL | H0 )
( T4 | LTR. O DRILL | H0 )
( T5 | 1/4 FLAT ENDMILL | H0 )
T1/1.350
T2/2.230
T3/2.250
T4/1.860
T5/3.210
N100 G20
N101 G0 G17
N102 G92 X0.0 Y0.0 Z0.0
N003 T1M6
N004 M3 S3500
N005 M8
N006 G0 X0.0 Y0.0 Z0.0
N007 G01 Y-.938 F3.0
N008 Z-1.0 F1.0
N009 X.750
N010 G03 X.750 Y.938 R.938
N011 G01 X-.750
N012 G03 X-.750 Y-.938 R.938
N013 G01 X0.0
N014 Y-.876
N015 X.750
N016 G03 X.750 Y.876 R.876
N017 X-.750
N018 G03X-.750 Y-.876 R.876
N019 G01 X0.0
N020 Y-.814
N021 X .750
N022 G03 X.750 Y.814 R.814
N023 X-.750
N024 G03 X-.750 Y-.814 R.814
N025 X0.0
N026 Y-.938
N027 Z-2.0 F1.0
N028 X.750
N029 G03 X.750 Y.938 R.938
N030 G01 X-.750
N031 G03 X-.750 Y-.938 R.938
N032 G01 X0.0
N033 Y-.876
N034 X.750
N035 G03 X.750 Y.876 R.876
N036 X-.750
N037 G03 X-.750 Y-.876 R.876
N038 G01 X0.0
N039 Y-.814
N040 X .750
N041 G03 X.750 Y.814 R.814
N042 X-.750
N043 G03 X-.750 Y-.814 R.814
N044 X0.0
N045 Y-.938
N046 Z-2.395
N047 X.750
N048 G03 X.750 Y.938 R.938
N049 G01 X-.750
N050 G03 Y-.750 Y-.938 R.938
N051 G01 X0.0
N052 Y-.876
N053 X.750
N054 G03 X.750 Y.876 R.876
N055 X-.750
N056 G03 X-.750 Y-.876 R.876
N057 G01 X0.0
N058 Y-.814
N059 X .750
N060 G03 X.750 Y.814 R.814
N061 X-.750
N062 G03 X-.750 Y-.814 R.814
N063 X0.0
N064 G0 Z1.0 Y2.0
N065 T2M6
N066 M3 S3500
N067 M8
N068 G0 Z0.0
N069 G01 Y-.938 X0.0 F1.0
N070 Z-2.395
N071 Y-.580
N072 X.750
N073 G03 X.750 Y.580 R.580
N074 G01 X-.750
N075 G03 X-.750 Y-.580 R.580
N076 G01 X0.0
N077 Y-.530
N078 X.750
N079 G03 X.750 Y.530 R.530
N080 G01 X-.750
N081 G03 X-.750 Y-.530 R.530
N082 G01 X0.0
N083 G0 Y-.750 Z0.0
N084 G0 X0.0 Y2.0 Z 0.0
N085 T3 M6
N086 G0 X0.0 Y0.0 Z0.0 S2000 M3
N087 M8
N088 G99 G83 Z-2.125 R1. Q.1 F3.42
N089 G80
N090 M5
N091 G91 G28 Z0.0 Y2.0
N092 T4 M6
N093 G0 X-.750 Y0.0 S846 M3
N094 M8
N095 G99 G83 Z-1.875 R1. Q.1 F4.2
N096 G80
N097 G1 Z0.50 F4.2
N098 X.75
N099 G99 G83 Z-1.875 R1. Q.1 F0.
N100 G80
N101 M5
N102 G91 G28 Z0.0 Y2.0 M9
N103 T5 M6
N104 G0 G90 X-.75 Y0.0 S2139 M3
N105 M8
N106 Z.1
N107 G1 Z-.560 F6.42
N108 G3 Y.1692 R.0687
N109 Y-.1058 R.1375
N110 Y.1692 R.1375
N111 Y.0317 R.0688
N112 G1 Z.1
N113 G0 Z1.
N114 X.75
N115 Z.1
N116 G1 Z-.560
N117 G3 Y.1692 R.0687
N118 Y-.1058 R.1375
N119 Y.1692 R.1375
N120 Y.0317 R.0688
N121 G1 Z.1
N122 G0 Z1.
N123 M5
N124 G91 G28 Z0.
N125 G28 X0. Y0.
N126 M30
%