[geoffeyles]

Anyone have any ideas why i am getting this arc while milling squares or hexagons
using g101 and no dia offsets machine is LR10M 5020L

Thanks

[deadlykitten]

hy pls check if :
... the material is rotating during machining : before machining, use a marker to mark a line on part & collet, and compare line position after machining
... x_offset is at tool center, x_wear is 0
... radius value = tool radius, and p quadrant ( considering that you use rad comp )
... toolholder is concentric with the spindle when G0 X0 T is executed

do you wish to obtain a piramid, thus several squares, or what is that ? kindly

ps : i also messed it up recently : i have measured the tool towards x-, but i should not have measured it like that

[geoffeyles]

material is not spinning in collet and all different sizes was just a test for a (NCMT) technician (he had no idea either)

x offset was at tool centre, no wear offset , no radius value set, and p quadrant left on zero

i programmed square as i would on a fanuc control

[deadlykitten]

no radius value set, and p quadrant left on zero

• method 1 : you may ignore the value of those 2 (rad & p), only if you also avoid g41/42 inside your code

• method 2 : you may declare rad=0 and p9, only if you use g41/42, and the toolpath is generated on tool center

• method 3 : you may declare rad=tool_radius and p9, only if you use g41/42, and the toolpath is generated not on tool center, but it reflects the size/geometry of the part

• method 4 : when using g41/42, you may entirely ignore p ( by leaving it always p=0 ), by using signed radius ( includes negative values), but this is not so common

when it comes to miling, i like to use method 1, so to 'lock' the code on a specific tool size, and requiring the operator to measure the tool only on Z ( X offset is generated from code )

i programmed square as i would on a fanuc control

considering that you are testing, i would suggest to reduce your tests to cutting a single line, not 4, thus 1st of all you should remove the 'arch', and only after that you may go polygonal

for your reference, i may give you a quick code, if you share your material & tool size / kindly

[geoffeyles]

the arc is the problem ... in getting this when cutting a straight single flat on a part and it will not program out using g102 or g103

I think its more a machine fault than a programming fault

but fire away with you code and i will give it a go..

thanks

[machinehop5]

...from the looks of the burr on the edges....maybe the tool is dull or to long.

[deadlykitten]

next code uses a tool o10 to cut a flat located at 12 from center, inside a material o30, using a radial clearance of 2.5 ( attached image )

if it works nice, i will make it cut a square

run it easy, in front of your part, since i can't test it right now you may have to add some %, maybe a program name, etc, i don't know, i don't have experience with your controller / kindly

(
  declare x_offset=-40 and measure tool on z; wear values to be 0; r & p does not matter
  i am not sure if -40 is ok for your machine, but it should be the x_value where your toolholder is concentric with the spindle
)


    V1 = 75 * 320 / 10 ( rpm )
    V2 = 4*0.010       ( feed g95)
    V3 = 05            ( tool )  


    G00 X500 Z250
    T+V3*101
    M110
    G137
    G00  X+14.739 Y17 Z-0.678
    SB=V1 M13 (M08)
    G101 X-14.739             F+V2 G95
    M12
    G136
    M109
    G00 X500 Z250 T+V3*100 M09
M02

[geoffeyles]

hi machinehop

no it happens with brand new cutters as well

the tool that cut the squares was 10mm dia and 25mm long

[OkumaWiz]

You will see this exact thing if for example a 3/8” cutter is used in place of a 10mm. It basically means the tool cutter diameter is wrong as compared to what is programmed. Tool comp should be used and adjusted until error is corrected.

This is not always in the tool but can be in theoretical tool centerline vs actual.

Guaranteed comp will fix this issue.

Best regards,

[geoffeyles]

Thank you

Okuma Wiz will have a go