copy and rotate, help (okuma)

[zooloader]

hi guys, this is my first post.
i'm using an okuma osp5020m controller down here in australia, and i'm stuck.
i need to machine a spherical "bowl" type shape into a 25mm plate with a 100mm radius, to a depth of 10mm at the centre.(not the actual dims.)
using the COPY and COPYE commands works fine if i substitute the radius for a straight line, and i get a cone shape.
but when i try the real thing, i get a problem.
here's my code:
G15 H1
T17 M6
G90 G0 X0 Y0 S2000 M3
G56 H17 Z50 M8
Z3
COPY Q359
G0 X0 Y43
G1 Z0 F100
G19
G2 X0 Y0 Z-10 R100
G17
G0 Z3
X0 Y43
COPYE P1
G0 Z100
M2

as i said before, when i replace the lines G19 thru G17 with:
G1 X0 Y0 Z-10
everything works fine. the problem is in the plane selection.
by the time it has rotated thru 90 deg. the plane that the arc is on has also rotated 90 deg. and is visible in the XY plane.
please help and thanks in advance!

[Kiwi]

Hi zooloader,

I'm not familiar with okuma but can you arc defined by 3 points. End point and a intermediate point.
I use a Fagor which would use G09
(Starting from X43.589 Y0 Z0)
eg G09 X0 Z-10 I24 K-7.077
(I = X intermediate point and K = Z intermediate point at 100mm radius)

KIWI

[zooloader]

hi KIWI,
I dont think the okuma uses G09 like that, at least i havnt used it anyway. I'll check it out.
do you think it would help?
how would you rotate and repeat the arc to get the bowl shape on your Fagor?

btw, how do you like the Fagor controllers anyway? i've only used them (briefly) retro-fitted to older machines, and they seemed to be quite powerful function wise.

[Kiwi]

Hi Zooloader,

This is my thoughts as I haven't tried the code.
If you use your equivalant to G09 you won't need to use G19.
FAGOR eg:
N10 G00 X43.589 Y0 Z3
G01 Z0
G09 X0 Z-10 I24 K-7.077
G00 Z3
N20 G73 Q1
(RPT N10, N20) N359

With this technique you will get a coarse (.75mm) finish near the outer edge and radial lines all converging in the centre.
I did a job similar to yours in which I used a cam program to generate a file which contained about 200,000 blocks. The path circled around from the outer edge and stepped down to the centre. These were all very short G01 moves with no G03. I could only run the feed at 30% as I couldn't download from my PC fast enough.
My thoughts now would be to create a profile path and add G93 I0 J0 (defines polar centre) and with a macro add to the block every .5mm along the profile G03 Q360 to do a revolution at that Z level.
(this could be done manually but may take a little time as there will be about 90 lines to change.)
I have only used a Fagor so unable to give a comparison. I have found the language very friendly.
Cheers
KIWI

[Kiwi]

Hi Zooloader,

Tried the code I posted but it didn't work as expected. I had problems like you. I haven't got my head around G18 and G19 yet.
Also tried the profile technique and it worked great. I believe this way will give much better finish.

Cheers
Kiwi.

[zooloader]

hi Kiwi,
thanks for the suggestions/ideas.
I've been pouring over the okuma manual to find anything, but it might as well be left in japanese for all the sense it makes.
Time ran out for this job hours ago, so i just stuck it in the lathe and bored it out!
I'll have to tackle it my own time now.
thanks again.

I think i saw some of your photos before, man, that looks pretty cool.

[Kiwi]

Hi Zooloader

If you want to send me a private message with the dims of your bowl I will send you a file with the co-ords. You may have to modify to suit your machine but what I see of your code it doesn't look too different.
Thanks for your compliments.

Cheers
Kiwi

[zooloader]

it's been nearly a week since i got your file, Kiwi, thanks.
changed the Q360's to I-xx.xx, and the start up stuff, and all was well.
i was wondering how you got the co-ords?
each step didn't look equally spaced, almost like it was skipping every 3rd (projected)step.
the customer brought in some more of the same but different radii, so i drew it on autocad and got all the co-ords from that(took a while!).
you were right about the finish too, i think trying to do it the way i started would have been lousy.
thanks again.

[Kiwi]

Hi Zooloader,
I got the coords from my CAM program.
The macro I wrote alters the points that are close to .5mm along the path as some of the points are very close together which would mean you are doing extra revolutions. This spacing can be altered as required.
The profile is based on a nominated Diameter Ball Nose Cutter as this PATH is not parallel with the DRAWN profile as the cutter starts cutting on its EDGE when near the outer diameter and on its BOTTOM when in the centre.
If working from you autocad drawing this needs to be taken into account.
I believe you would have had the same outcome using you original method.
It may be possible to Radius Compensate from the Centre of the Ball Nose Arc. (1/2 the dia from the end point as well as left or right radius)
I haven't found a G code in my Fagor manual, only G41 and G42 for left and right.
Somebody else who knows more than me may be able to say if this is possible.

Drop me the specs of your jobs with cutter dia. and I will send you the file if you wish.
No Problem.
Cheers Kiwi

[Egar Twins]

real simple ...have it retofitted to a CAD CAM system and draw it!

[zooloader]

G44 is the code our Okuma uses for 3D tool offsets (this was an optional card fitted, and it's only been used twice in 10 years!). Apparently, you specify the radius of the cutter in I,J and K. I dont know why, I've never seen an elliptical, or variable radius tool before.

Yeah... simple! All I gotta do is tell my boss to fork out the cash for a cad/cam program that will hardly get used.

[Egar Twins]

All I use is CAD/CAM system programming...while I totally respect those that GCODE (and I must admit that I am in the process of searching for a media source for G-COde training; any ideas?) as it is where our trade began, the CNC world is moving towards CAD/CAM systems that do the work for you...you have to evlove with technology or be replaced.