Need thread cutting help

[Larry Myers]

Hi all,
I am looking for some advise concerning internal thread milling. I have a Sharp 2412 VMC. Fanuc oi.
I am wanting to thread a 1”-8 hole, 1” deep. (aluminum) I have the hole already bored out to 7/8”.
I have a 6 flute single point carbide bit that is 0.695” dia. I wasn’t going to use cutter comp to begin with. Below is the part of the program that I am having trouble with:

T4M06(THREAD MILL);
G00G17G20G40G80G90;
G54X0Y0M03S1000;
M08;
G43H4Z0.1;
G01Z-1.0F20.;
X0.150F10.;
G91G03X0.15Y0I0.15Z0.125F10.L10;
G01X0Y0M09;
M05;
G00G28G91Z0;
M30;
%

I think my problem is in the feedrate however I am not sure what to do. Thanks in advance for any help!

Larry

[Geof]

As far as I can see your helical part is okay. You go to the bottom, set X at 0.15 then start circling your way out 0.125" per turn. Your speed is a bit low at 1000rpm, in aluminum with that dia cutter you could go several thousand rpm.

Actually looking at it again you move X0.15 then have I0.15; I should be negative? I program on Haas and the I or J has a sign opposite to the X or Y move so for X0.15 I would use I-0.15 but I don't know if your machine needs this. Also with Haas I can omit the X and Y in the G03 and just have

G91 G03 I-0.15 J0.0 Z0.125 F10. L10

[dcoupar]

Larry,

You don't say what problem you're having!

Geof is correct... your I should be -0.150, and you can omit the X and Y coordinates.

[Larry Myers]

Hey Guys

I suppose it would help if I said what the problem was! Thanks
I added the negative sign and that helped.

The problem is that I generate one large spiral (helix) that stops at 0.125” above the top of the part. I thought that by adding the G91 it would travel up incrementally by only 0.125” and the L10 would tell it to repeat 10 times so that I generate a 1”-8 thread.

Hope this helps! And thanks again!

Larry

[Geof]

Originally Posted by Larry Myers Hey Guys I suppose it would help if I said what the problem was! Thanks I added the negative sign and that helped. The problem is that I generate one large spiral (helix) that stops at 0.125” above the top of the part. I thought that by adding the G91 it would travel up incrementally by only 0.125” and the L10 would tell it to repeat 10 times so that I generate a 1”-8 thread. Hope this helps! And thanks again! Larry

I saw a different thread on this same topic a while back and they had the opposite problem; it only went up one thread then just round and round (I think) Some one posted that the helical interpolation was an option that had to be turned on...sounds like this may be your problem.

You should be able to get around it by doing absolute G03 lines with Z-.875, Z-.75, Z-.625, etc, etc. Not too tedious for only ten lines.

Or get a Haas which comes standard with the G91 Z increment and L count for G03 and G02.

Had to be a naughty boy and put in that plug.

[andyt]

Try eliminating the G91 and replacing the Z.125 with a W.125. Delete the L10 and see if it will run at least one revolution correctly. If that doesn't work, then your control doesn't have the helical interpolation option. If it does, just add the L10 or repeat the line 10 times.

[Larry Myers]

Thanks again guys,

I replaced the z0.125 with a W0.125 and it did not recognize the address. And for some reason it does not do the G91. It looks like I will try doing 8 circles going up 0.125 at a time that Geof suggested. I don’t foresee a problem there as there are only 8 iterations I need to be concerned with. I was just kind of hoping there would be a cleaner way of doing it.
Thanks all

Larry

[dcoupar]

Larry,

W won't work. That's an incremental Z command for a lathe.

You could use a sub. M98 Pnnnoooo calls sub oooo nnn times

T4M06(THREAD MILL);
G00G17G20G40G80G90;
G54X0Y0M03S1000;
M08;
G43H4Z0.1;
G01Z-1.0F20.;
X0.150F10.;

M98P0101001(CALL SUB 1001 10 TIMES);

G01G90X0Y0M09;
M05;
G00G28G91Z0;
M30;
%

O1001 (HELIX SUB)
G91 G03 I-0.15 Z0.125 (oops)
M99

[extanker59]

Hi guys,
dcoupar, nice compression. Our Haas wants the sub call out like this: M98 P1001 L10
Also don't forget the G03 in the sub. I'm also paranoid so I like to rapid up to Z.1 before going home (I make it move the Y axis closer to the operator so he can check it out during set up). I prefer G53 Y0 Z0 over G00G28G91Z0;
Larry- don't forget the G90 in your first post "G01X0Y0M09;" , otherwise it'll sit there in contact when you rapid up.
Chris

[Larry Myers]

Thanks guys, I really appreciate the help. I will try this afternoon.

Larry

[dpark1]

I ran this same thread today on fadal-program works fine


N1O6970(THREAD MILL)
N2(D1=.77)
N3(D2=.757)
N4(D3=.748)
N5(FOR 1"-8 PITCH TAP)
N6M6T1(3/4 CAR. THREADMILL)
N7G0G40G80G90S600M3
N8X0Y0E1
N9Z0.1H1D1M8
N10G1Z-0.95F10.
N11G91G41X0.5F12.
N12G3I-0.5Z0.125L8
N13G90G1G40X0Y0
N14G1Z-0.95F10.D2
N15G91G41X0.5F12.
N16G3I-0.5Z0.125L8
N17G90G1G40X0Y0
N18G1Z-0.95F10.D3
N19G91G41X0.5F12.
N20G3I-0.5Z0.125L8
N21G90G1G40X0Y0
N22G0G49Z0M5M9
N23X0Y0E0
N24M99
N25M30