Y axis problem

[Raymond AscroftParticipant @raymondascroft71629]

Could someone point me in right direction please. Milling an internal triangle shape with 9mm corner rads with the Seig KX3 the cutter did not go round rad but returned along the path it came, when trying to cut rad the usual up & down sound of the motors was different mainly just one level sound, stopped m/c & returned axis to zero & Y axis was out by about 3mm the axis were all running OK manually but Y axis sounded a bit rough. the Mach 3 simulation showed correct path. Is there a minimum rad size these m/c's can handle it was 4mm dia cutter.

[Raymond AscroftParticipant @raymondascroft71629]

Seig KX3

[JasonBModerator @jasonb]

What feed, speed, DOC and material? Material and quality of cutter and any lubricant/coolant and or air/vacuum?

[Anonymous]

It's either a G-code problem, or an interpretation error. Look at the G-code and in particular any G02/G03 codes to see if they make sense. There could be a disconnect between the way the G02/G03 parameters are specified in the code and the way Mach3 expects to see them as there are several variants.

Andrew

[Former MemberParticipant @formermember32069]

[This posting has been removed]

[Raymond AscroftParticipant @raymondascroft71629]

Jason

DOC 0.2mm to check shape then 2.0mm, L61 Al, Brand new centre cut Carbide Garryson 4.0mm endmill, dry cut

Andrew & Barrie

N010 G0 G21 G49 G40 G17 G80 G50 G90
N020 M6 T3
N030 G64
N040 M03 S3000
N050 G00 G43 H3 Z30.0
N130 G00 X-28.84 Y14.74
N140 G42 G00 X-28.84 Y11.74
N150 Z2.0
N160 G01 Z-0.2 F10.0
N170 G01 X-53.2347
N180 G02 X-55.2074 Y20.2845 R4.5
N190 G01 X-30.8127 Y32.1831
N200 G02 X-24.34 Y28.1386 R4.5
N210 G01 Y16.24
N220 G02 X-28.84 Y11.74 R4.5
N225 G01 X-29.5 Y10.5
N230 G00 Z3.0
N240 G40
N250 G00 Z30.0
N260 G00 X0 Y0
N270 G00 G53 G0Z0
N280 G49
N290 M5
N300 M30
N310 %

[martin perman 1Participant @martinperman1]

Andy, Jason,

I dont wish to highjack this thread but Ive never worked with this machine code before but is it as simple as I think it is.

Nxxx line no

T type of cutter

S speed

G coordinates

X,Y,Z Axis

R radius

% end program

F feedrate

M Motor

H home position

 

Martin P

Edited By martin perman on 13/02/2019 21:08:00

Edited By martin perman on 13/02/2019 21:10:11

Edited By martin perman on 13/02/2019 21:12:11

[Anonymous]

Posted by martin perman on 13/02/2019 21:07:14:

I dont wish to highjack this thread but Ive never worked with this machine code before but is it as simple as I think it is.

Nxxx line no

T type of cutter – cutter number, used for toolchangers, it doesn't say anything about the type of cutter, simply where to find it

S speed – correct

G coordinates – Gxx are general commands which may, or may not, relate to a move. G00 is goto specified position at rapid rate, G01 is goto specified position at specfied feedrate, G02/G03 perform a circular motion clockwise or counterclockwise

X,Y,Z Axis – specifies the points in each plane to be used

R radius – correct

% end program – more an end of file marker, somewhat obsolete now that programs are normally stored in memory rather than loaded on the fly from tape

F feedrate – correct

M Motor – miscellaneous commands for controlling spindle direction, coolant on/off, program end, and much more

H home position – tool length offset, ie, relative length of each tool, and where to find it in the tool table

Nearly but not quite – see annotations above

Andrew

[geoff adamsParticipant @geoffadams14047]

a quick look at your code cutter comp line g42 does not have a d number so the control dos not know the cutter dia and number

have run the code on mach 3 with and without cutter comp with comp 4mm dia cutter it does so funny moves on the bottom left corner do you have a drawing i will try on my machine later

Geoff

[JasonBModerator @jasonb]

First thing that looks wrong to my very little G-code knowledge is that a cut of R4.5 won't give the 9.0mm radius corners mentioned in the first post. If R is the ctr line of the cutter then 7.5 would be needed.

Also looking at the first two lines where the table moves

N170 G01 X-53.2347

N180 G02 X-55.2074 Y20.2845 R4.5

First line starts from Zero and moves -53.2347mm in X

Next like has a 4.5mm radius cut ending -55.2347 in X and 20.2845 in Y but that is further than the diameter of the circle away from where the previous cut stopped?

 

Edited By JasonB on 14/02/2019 07:36:16

[Ex contributorParticipant @mgnbuk]

Nearly but not quite – see annotations above

"T type of cutter – cutter number, used for toolchangers, it doesn't say anything about the type of cutter, simply where to find it" Depends on the system – some use the T number to call the tool offsets as well, so also applicable to machines without an ATC

% end program – more an end of file marker, somewhat obsolete now that programs are normally stored in memory rather than loaded on the fly from tape Still used on Fanuc

H home position – tool length offset, ie, relative length of each tool, and where to find it in the tool table Not on all systems, as above.

Nigel B

[geoff adamsParticipant @geoffadams14047]

Jason it looks like Raymond is using cutter comp in which case you programme the profile as seen on the drawing not the cutter path

the control will work out the tool path a drawing of what he wants would help

Geoff

[JasonBModerator @jasonb]

Posted by geoff adams on 14/02/2019 08:04:59:

Jason it looks like Raymond is using cutter comp in which case you programme the profile as seen on the drawing not the cutter path

 

In which case should he have entered R9 if that is the radius he mentions in his first post? and even then how can the end of the arc cut be over 20mm away from where the first straight cut ended I would have expected 18mm at the most.

Edited By JasonB on 14/02/2019 08:20:30

[geoff adamsParticipant @geoffadams14047]

Jason

not knowing were his xy zero is it looks like if you look at line 260 it goes back to zero then line 130 goes to a start pos of x-28.84 y14.74 then a move to put cutter comp on to y11.74 so you 20.285 will be a move of 8.5 likewise in the x starts at x-28.85 to x-53.234 gives a move of 24.38 i will go and run it on my machine and post some pics

Geoff

[geoff adamsParticipant @geoffadams14047]

Jason you can download mach3 demo and run 500 lines of code with no licence i use this to check my code

Geoff

[Raymond AscroftParticipant @raymondascroft71629]

Good morning all
must apologise for error it was a long day yesterday, the part is a steady for 3 x 9.0mm dia rods so corner rads are 4.5mm it is a internal right angle shaped pocket, the prog uses cutter comp G42 cutter offset right conventional mill.The cutter was originally 6mm dia hence allowance of 3mm to start comp in Y axis lines N130 & N140 tried 4mm cutter to see if giving m/c more room to move round rad would help. Line N225 above is wrong Y should be 12.5 it is 5 years since I have done a prog and had forgotten that prog can't finish with an arc so entered line manually was changed before running it. Unfortunately there is no drawing I was given X & Y projected dimensions of a right angled triangle and told to blend corners with 4.5mm rads over the phone I think sizes measured with CMM m/c. The missing lines N050-N130 are for tool no.2 a 10mm slot drill plunge cutting out surplus

[Anonymous]

I imported the code into my backplotter program (NcPlot) and it generated the expected toolpath shape and stepping thorugh the code the tool stepped round exactly as I'd expect. So it may be an interpretation problme in Mach3.

Having said that there are some odd features of the code. Presumably it was hand written? I've never felt the need to use cutter compensation, I just let the CAM software sort that out given a stock allowance and a tolerance.

Andrew

[Former MemberParticipant @formermember32069]

[This posting has been removed]

[Anonymous]

If I read the OP correctly the tool returned down a previous move, but with an offset. I wonder if it's getting it's knickers in a twist with cutter compensation and is trying to mill the outside side of the slot?

As an aside I've never heard of the limitation of a program not being able to end on an arc. Presumably that means you can't end on G02/G03?

I just fudged one of my programs to end on G03 and the backplotter didn't throw a wobbly.

Andrew

[Raymond AscroftParticipant @raymondascroft71629]

Just tried again & Y axis ballscrew just turned a few degrees & motor sounded like it was struggling while cutting rad it stopped as it started up the angle face although the readout showed movement of both axis the cutter returned along path of 1st cut, stopped it after about 10mm homed m/c & Y axis moved normally manually
Andrew Home posn is intersection of X & Y sides of component

[JasonBModerator @jasonb]

Have you tried it without actually cutting to see if the table will move OK around the shape with no load.

[Martin ConnellyParticipant @martinconnelly55370]

In certain situations you should avoid using the radius format with G02 and G03 as it can cause problems according to the Mach3 programming notes. Small errors due to rounding of coordinate values can cause large variations in the path the cutter takes.

Martin C

[Raymond AscroftParticipant @raymondascroft71629]

Jason set Z inhibit to 10mm and also swapped I&J for R to define circle centre with no difference when run ballscrew stopped turning. Looking at Seig parts diagram confident I could replace stepper motor but if it didn't work as plug & play I'm lost electronics might as well be written in Chinese. Notice that helpline finished now too

[blowlampParticipant @blowlamp]

Cutter compensation can cause problems with some controllers if there is insufficient lead-in to the start of the cut – you need to be something like a tool diameter away from the intended toolpath for some controllers to work as expected.

Here's some code from CamBam for use with Mach3 with tool radius (assumed 3mm diameter tool) already accounted for i.e. no G40, G41 or G42 Origin is at lower-right arc centre.

( Made using CamBam – http://www.cambam.co.uk )
( triangle 2/14/2019 6:28:13 PM )
( T3 : 3.0 )
G21 G90 G91.1 G64 G40
G0 Z3.0
( T3 : 3.0 )
T3 M6
( Profile1 )
G17
M3 S1000
G0 X-25.7102 Y2.6963
G0 Z1.2
G1 F10.0 Z-0.2
G1 X-1.3152 Y14.5953
G2 X3.0 Y11.899 I1.3152 J-2.6963
G1 Y0.0
G2 X0.0 Y-3.0 I-3.0 J0.0
G1 X-24.395
G2 X-25.7102 Y2.6963 I0.0 J3.0
G0 Z3.0
M5
M30

Martin.

[JasonBModerator @jasonb]

Before you start pulling the steppers out it may be worth just doing a simple code such as an external square, that would eliminate problems with the code and radius cuts and show if the y axis is playing up.

[Author]

Posts