[mbm]

Hey guys, i'm trying to cut a 17mm x 1.50 thread on my lathe and i'm having some troubles. I only have enough experience to write programs with IGF feature then i am able to go back and edit.I typically machine everything in inches and now I have a job that requires a metric thread and i'm stumped!!! I got my IGF scren to display metric on every dimension ,however when it asks for thread dimensions it asks for TPI and you cant input a decimal point for the pitch of 1.50. Could someone look at my line of programming and point me in the rite direction: G71X16.2Z-13.5H0.0866D0.5U0.1B60F1J1.5M22M73M32

[phx]

Hey guys, i'm trying to cut a 17mm x 1.50 thread on my lathe and i'm having some troubles. I only have enough experience to write programs with IGF feature then i am able to go back and edit.I typically machine everything in inches and now I have a job that requires a metric thread and i'm stumped!!! I got my IGF scren to display metric on every dimension ,however when it asks for thread dimensions it asks for TPI and you cant input a decimal point for the pitch of 1.50. Could someone look at my line of programming and point me in the rite direction: G71X16.2Z-13.5H0.0866D0.5U0.1B60F1J1.5M22M73M32

easy;-)
G97 SXXXX M§
G00 x18 z20
z5
G71 X17 Z-13.5 H2 F1.5 M33 M74 u 0.03 D0.2
you did not tell about material so you as to change maybe.

[mbm]

Ha ha, its only easy when you know it.Thank you for your help it was very much appreciated!

[OkumaWiz]

You could also do this if you are running in inch by using F1.5/25.4.

I see that you are running metric instead of our inch mode, but thought that you'd be interested to know that math can be used in the program virtually anywhere.

So leave the J value at 1 and use whatever is easiest for you for your F value.

One of the reasons to use the math is that the control will calculate out the pitch to a much smaller value (more decimal places) which will give you a more accurate thread. even if you are only off by .00005, it adds up to .001 error after 20 rev's or so.

Best regards,

[Algirdas]

isn't it better to switch to metric mode? therese are just a couple parameters to change.

[OkumaWiz]

isn't it better to switch to metric mode? therese are just a couple parameters to change.

Yes and no. Here in the good ol USA, all of the inspection equipment and prints are in inch, so no it's much more than a parameter change to make parts.

But yes, your machine will actually position finer in metric than inch.

I've asked Okuma to give us 5 decimal places in inch as a standard spec, but no positive response yet...we do have one lathe with it as an option and yes, it kicks a$$! We held a +- .0001" tolerance with few problems.

Best regards,

[Algirdas]

sorry for off-topic, but
all of the inspection equipment and prints are in inch
United States is the first empire in the world, pronounced to establish SI (=metric measurement system) as a only standard long ago ... how that could be?

[Superman]

sorry for off-topic, but
all of the inspection equipment and prints are in inch
United States is the first empire in the world, pronounced to establish SI (=metric measurement system) as a only standard long ago ... how that could be?

Hey Al, you talk crap---remind me to send over some toilet paper to clean up your dribble
United States customary units - Wikipedia, the free encyclopedia

[broby]

sorry for off-topic, but
all of the inspection equipment and prints are in inch
United States is the first empire in the world, pronounced to establish SI (=metric measurement system) as a only standard long ago ... how that could be?

Oh come on Al, you can not be serious with a stupid statement like that!
The US is IMPERIAL through and Through!
Everything is measured in Miles down to Inches...
All units are Imperial.
Speed=MPH
Thread sizes for US threads are all IMPERIAL!
They think they know Metric, but hey, remember one of the last probes sent to Mars? They, the esteemed egg heads in NASA, screwed up a simple unit conversion between Metric and Imperial and then lost the probe somewhere between here and there! Pretty dumb and very expensive screw up!
BTW... did you not know that SI is French in origin?

As for programming threads in IGF... (going on memory here so some details might be slightly incorrect)
Entry of the thread pitch is in the field "Lead" or "F" as specified on the drawing... 1.5 in your case.
Lead is output on the G71 line as the value "F"
Leave the value for TPI as 1, this value if set other than 1, will be output as "J"
To program an Imperial thread on a machine set for Metric you set the lead to 25.4 and the TPI to the number of threads per Inch.
Now, before you go on about not being able to input a value of 1.5 in the TPI field do this:
Multiply the TPI value by what ever amount you need to obtain a whole number.
ie if you require 11.5 TPI Multiply this by 2 to get 23
Now multiply the lead by the same amount i.e. 25.4x2=50.8
Now enter the Lead as 50.8 and TPI as 23
This will output F50.8 J23 in the G71 cycle.
The machine will then cut 23 threads per 50.8mm, or in other words 11.5TPI.

As for cutting Metric threads on a machine set up in Imperial...? Have never done that so can not help.

I hope this helps,
Regards
Brian.

[Algirdas]

I would not say 25,4mm = 1". It is not accurate. There are information sources where more digital places are used.
I would advice to not fear of switching control parameters. Maybe numbers will look wierd at the begining. Okuma has no problems with different measurement systems. A lot of our clients are making parts according imperial units on Okumas along with metrics and no problem. They just switch the parameters.

[MCR-B II]

To mbm and to phx
I think thread height H is wrong and should be 1.624mm

[OkumaWiz]

I would not say 25,4mm = 1". It is not accurate. There are information sources where more digital places are used.
I would advice to not fear of switching control parameters. Maybe numbers will look wierd at the begining. Okuma has no problems with different measurement systems. A lot of our clients are making parts according imperial units on Okumas along with metrics and no problem. They just switch the parameters.

Al, are you for real? I post on here to help people. I'm convinced that you post to try to increase your number of post to try to gain some sort of credibility for yourself. It isn't working. You keep on sticking your foot in your mouth and come off looking like an idiot.

Everyone else on here understands that we PRIMARILY use inch in this country, and MOST of our inspection equipment is also inch. Why do you try to make off-post comments that don't help anyone? Is it just to increase your post count?

Unless you are helping solve the problem. DON'T POST! You only succeed in irritating those of use trying to sincerely help others.

[littlerob]

To mbm and to phx
I think thread height H is wrong and should be 1.624mm

Meanwhile back at the ranch (American sorry): MCR your H value should definitly NOT be 1.624. Maybe you are thinking finish X. But your using IGF so someone much smarter than I will chime in to get your proccess right.

But to get the machine running and build parts, use this formula for "H"- from where the tool begins to cut subtract where it finishes the thread diameter, divided by two, that will be what your program wants to hear for thread Height.
Start X-Finish X/2=H

Algirdas your stupidity leaks out into the screen, your posts are an unexpected hijack and outside what we think of as constructive, in fact the reason people flame you is more to compensate for your asinine posts than to argue. Remember most of your posts are degressive.

Robert

Get my alter ego out here!!

[phx]

To mbm and to phx
I think thread height H is wrong and should be 1.624mm

omg, sorry i made a mistake, (chair)(chair) but not H is wrong, X must be 15,

mcr-b, we cut from 17 to 15, so thats 2mm = H

[cncserveng]

I think "Al's" comments are lost in translation, I cant really grasp what point he is trying to make. The 1" = 25.4mm is easily accurate enough for any turned or milled part, it is however dangerous to use G20/ G21 or to switch parameters. A mm is a lot less than an inch and if you make a mistake and run a metric program in inch mode, you will for sure have a big crash.

[MCR-B II]

I think "Al's" comments are lost in translation, I cant really grasp what point he is trying to make. The 1" = 25.4mm is easily accurate enough for any turned or milled part, it is however dangerous to use G20/ G21 or to switch parameters. A mm is a lot less than an inch and if you make a mistake and run a metric program in inch mode, you will for sure have a big crash.

I agree with you. No need to change parameters.

To phx : You are wrong. Pitch doesnt depend on X Diameter. Check one more.

[littlerob]

After rereading this thread again I made a mistake in my post!

1. Thread height is represented by the H value as the radial thread height from root to crest. If your start diameter is 17 and your finish is 15 than your thread height is 1. (17-15/2).

2. If you are going to use Customary units <(I know, I see the oxymoron, calling it Customary but that is what their called) the feedrate or F value needs to be .059 (1.5/25.4=.05905)

To phx : You are wrong. Pitch doesnt depend on X Diameter. Check one more.

3. I don't think phx ever stated that pitch is determined by X diameter.

snip>I think "Al's" comments are lost in translation, I cant really grasp what point he is trying to make.

4. I agree, but these have been the same ignorant, unfounded comments about "Americans" for 2 years, it's getting so I personally don't like visiting the site because of his posts, he is a trolling vampire. (flame2)

Robert

[Superman]

it is however dangerous to use G20/ G21 or to switch parameters. A mm is a lot less than an inch and if you make a mistake and run a metric program in inch mode, you will for sure have a big crash.

Correct me, if I'm wrong

but having the G20/G21 at the head of the progam IS a good idea. Think of it as a safety code that is drummed into any person just getting into CNC

-this does not alter the units the machine is running in, but it it would stop the program from running if the machine units are reversed.

It would halt a metric program from running on a machine set to imperial.

The G-code is only a checking code

[MCR-B II]

You can see here

Metric Fine Thread Data

[phx]

You can see here

Metric Fine Thread Data

what u want to say with this?
you mean 15.16?