live tools and C

charlie/c · Jun 18, 2003

Hi
I own and run a small precision engineering shop. We have 4 VMC's and 4 CNC lathes. The latest lathe has live tooling with full "C" axis. We have worked out how to produce a hexagon on the end face of turned parts using an axial tool. We can also do radial/axial bolt holes on PCD's no problem.We now want to produce just one flat on the outer edge, again with an axial set-up. We have calculated everthing just as with the hex but with only two points, ie the start and end of one flat only. We have tried with and without cutter comp (hex uses comp ok ) but with no success.Tool type is set to 0 in tool geometry page, than one took some understanding !
Machine is a CMZ 1450 TB with fanuc OC control.
This thing is just going all over the show, it's doing our heads in.

Ox · Jun 18, 2003

I'm thinkin' that your tool comp should be "9". I have found it best to make the first line of C command to be C0. I do this during other x and z movements. Then go about your business.

BTW, I have no idea what machine you are on, and mine is an 18-T.

Think Snow Eh!
Ox

[This message has been edited by Ox (edited 06-18-2003).]

Tom · Jun 19, 2003

Charlie,
Tool quad should be 9.Post your code, size of outside diameter, depth of flat and endmill size and I can check your code. I am an applications engineer for a us machine tool builder and am very fluent with live tooling and c axis on lathes with any fanuc control. In addition if you post your email address I can forward to you the c axis examples and format that we instruct our customers on.
Tom

charlie/c · Jun 19, 2003

Tom
The part is 88mm dia with one flat 42 from centre.There are 6 bolt holes in the front face, one being lined up with the centre of the flat.Cutter dia = 15mm. We have started the pcd at 30 deg to miss a chuck jaw.We can't see how we can shift the datum for C0 so we positioned the holes long-hand.Ideally we would like to do the flat at 30 deg also.
This is the code we tried just to do the flat centred on the 3 o'clock pos'n.

G0 G40 G69 G98 T0808
X110 Z2 M8
M80
G0 C0
M84 S1000
G1 Z-9 F500
G112
G1 G42 X84 C-40
X64 C40
G40 X110 F1000
G113
M85
M81
G0 X200 Z150 T0800

My e-mail add is [email protected]

Would very much appreciate the examples.
This looks like it should be so easy but it has been a stuggle all the way so far.

many thanks
Charlie

Ox · Jun 19, 2003

G1G112

(Fanuc book shows both of these in same line for some reason. I always try to not use more than 1 G or M in one line. Sometimes it won't read one of them.

Also, untill you get your programm figured out, it is best to not run your Z in - so you don't crash or even waste the blank. Run it through in Z+ untill you think it looks right. Then change your Z value.

If you are going from C- to C+ shouldn't you be in G41? (Just cheating off a proven prgram here. LOL!)

G0 G40 G69 G98 T0808
X110 Z2. M8
M80
M84 S1000
G0 C0
G1 G112
G41 X84 C-60. F500 (tool clearance, just for grins)
Z-9 (when ready)
C60. F-whatever you decide
Z2. F500
G40 U0 G1 H-7.5 (not sure why G1 is in there, I doubt it is necessary)
G113
M85
M81
G0 X200 Z150 T0800

I say try this and see whatcha get.

Hey Tom, should I try to guess your last name and where you work?

Think Snow Eh!
Ox

[This message has been edited by Ox (edited 06-19-2003).]

Tom · Jun 20, 2003

Charlie,
With the dimensions you have given to machine a flat at the 3 o'clock position following are the numbers I come up with. I am assuming you are programming in diameter mode.

your format and codes

G0X100.Z25.C0
G1G98G112
G1G41X90.Z1.F150.
C-42.
Z-9.F10.(cutting feedrate)
X-90.
Z1.F150.
G40U25.H25.
G113

return to your index position

note that the X90. can be changed in the above as long as both X words are the same value and signed as above, this is for clearance only.

Tool quad should be 9 and make sure you place the cutters radius in the geo. tool file only (not in both wear and geo. as this will double the size of the radius).

I will e mail to you the examples, keep in mind you may need to change the format slightly for your machine.

Hope this helps,
Tom

PS. Ox no need to guess, I think you have it figured out and to machine from C- to C+ it should be G41.

Ox · Jun 20, 2003

I see you changed the C and X around. I have no idea where my code would of put the flat. LOL! (3 O'clock)

Think Snow Eh!
Ox

Tom · Jun 20, 2003

Ox,
You would have been at 12 o'clock, high noon at the O.K. Corral.
Tom

charlie/c · Jun 21, 2003

Hi Tom & Ox
Thanks for the replies. We havn't tried them yet m/c on a long run. Why the incremental moves at the end ? and why do you call comp prior to plunging and approaching edge of work.
Take a look at this, it does a 13 a/f hex ok for us.
%
:7777(18 A/F HEX')
G21
G50S1500
M13
M23
G0G40G69G98X250Z250.T0800
X40Z2.T0808
M80
G0C0
S1000M84
G1Z-5F1000
G112
G1G42X13F200
X13C3.753
X0C7.5
X-13C3.753
X-13C-3.753
X0C-7.5
X13C-3.753
X13C0
G40X40F1000
Z2
G113
M85
M81
G0X250Z250.T0800
M30
%

Any answers on shifting the C0 to a more convenient pos'n ?
It's Saturday morning here and we should be able to give your solutions a try before we go home and cool our heads in a bucket of water.

Charlie

Ox · Jun 21, 2003

It's sat morn here too Chuck! We are GMT - 5 not 25! LOL! (6 with daylight savings time eh?)

Anyhow, I would want to get all my tool comp done before I go Z-, just so that you don't mistakenly crash out. (especially if you want to maybe single block the first time through) Once your program is verified, I guess you could do it the other way if you want. This is how the book shows it, and I like it that way anyhow. What is your reason for NOT wanting to do it that way?

I was wondering why Tom made such a big H move at the end myself. In my code, I just use an H movement equal to the R of the cutter that I intend to use. (VMC too) This should actually save movement of the turrett altogether, and most importantly assure that your turrett doesn't go crashing into the part once you take the Tool comp away. As long as you are clear of the part it shouldn't matter. I guess Toms 25. would just send the turrett farther away yet is all.

Tom, why did you have a U 25. in there?

Personally, I think that C axis programming (at least on the Fanuc) leaves a lot to be desired. It would seem like it wouldn't have to be quite so daffycult! But it is what it is. LOL!

Think Snow Eh!
Ox

Ox · Jun 21, 2003

On your hex prog, your going from C0 to C+ making your G42 OK.

On your initial flat prog, you are going from C0 to C- which means that you shoulda changed to G41. Get it? Got it? Good!

Tom:

note that the X90. can be changed in the above as long as both X words are the same value and signed as above, this is for clearance only.

If he fed from X90 to X-70 and then rapid (or feed at higher rate, b/c it would be done cutting on the exit sooner than it would on the entrance) to X-90, the flat won't be square with the world will it? You actually need to cut air to get it square, don't you?

Think Snow Eh!
Ox

[This message has been edited by Ox (edited 06-21-2003).]

charlie/c · Jun 21, 2003

Ox / Tom
It worked, The cutter path seems to be in and out like a fiddlers elbow before it actualy cuts anything, but with a bit of tweaking it did it. Thanks.
My reason for doing tool comp after 'z' is simply that i'm a miller !
I think your right 'C' axis programming shouldn't be so difficult.
I run Teksoft cad/cam for which I have a live 'C' post for a different m/c. It doesn't do G112/3 and I have only used it a few times for 'A' axis work on the mill.
Hope that will cope because anything slightly complicated is going to be a nightmare this way.

Tom · Jun 23, 2003

Ox,Charlie,
The H25. move was made as I was not sure of the cutter size, and I did not think he would be using a 2" dia. cutter. Normally I would make this move the size of the cutters radius. On some controls if you do not move 2 axis when canceling the comp you will generate a 197 alarm. As for the x axis movements if you were to go from X90.to X-70.
you would cut a taper and the flat would not be swuare. You could go from X70. to X-70. and that would work.

Charlie, I will try to email you my examples today, I could not get on to our network on friday to get the file.
Tom

Tom · Jun 24, 2003

Charlie,
Do you have the ability to get to the "W.SHFT" page. If you can get there you can workshift the "C" and/or any programmable axis were you want it.
Sorry did not have time today to email you the examples, I will try the next time I am in the office.
Tom

charlie/c · Jun 25, 2003

Tom,
Yes we can get to the w-shift page,it works, it's obvious really, just like a mill.
Thanks

Charlie

Search

Largest Manufacturing Technology Community on the Web

Search

live tools and C

charlie/c

Plastic

Ox

Diamond

Tom

Cast Iron

charlie/c

Plastic

Ox

Diamond

Tom

Cast Iron

Ox

Diamond

Tom

Cast Iron

charlie/c

Plastic

Ox

Diamond

Ox

Diamond

charlie/c

Plastic

Tom

Cast Iron

Tom

Cast Iron

charlie/c

Plastic

Similar threads