New Onecnc user!!

[smitty]

Now, the tool I am using is what I call small. Total thickness of the tool is .040 with a full radius on the end.
Now, when I lied to the lathe and re-set my X zero .0425 past my first Zero point, the part cam out just about perfect, except the main shaft is to thick, but the balls are just right.
So if I can get this small problem figured out, I'm in bussiness!
Thanks to everybody for helping me out!!!
Smitty

[HuFlungDung]

Smitty, I think you accidentally unchecked diameter programming in your NC Post Output settings. However, it would appear that your nc code looks like it was done with diameter programming on.

So, where in your nc program do you tell your controller that you are using G90 absolute mode? If you say the lengths are right, it must be running in absolute, but the appropriate Gcode for the mode (absolute or incremental) should always be near the start of your program.

You also have not established a G92 work home which means we have no way of knowing where you are starting from. If you touch up to the end of the part, right on center, this is X0Z0 as you are already doing. Back off to X.5 Z.1 and then edit in this line near the beginning of your program:

G90
G92 Z.1 X.5
T0909
S(spindle speed command, if you have a variable speed spindle drive)
M3 (spindle on, forward command)

All the rest of your nc program should then run in relation to this "virtual G92 home".

Second, you should not keep reconfiguring the default config, because it is a default. Configure it as you like, then click save as, and give it a meaningful name.

Apart from that, I looked at the last line of your nc code, which would be the finish cut, and it appears like the X diameter values are correct: .170" + (.02"tool radius *2) = .210".

So, I would think it is something you are doing in setting up your tools or zeroing. Do you know how your controller calls up tool offset commands? We do not rely on zeroing our tools all the time, in order to make slight (or major, for that matter) corrections to the all-over cutting diameters. This is what the tool offset tables are for. Chances are when the command T0909 is read, your controller software is checking for a value in an offset table somewhere, and adjusting your tool position. If you have a zero (both in X and Z) in that table right now, no adjustment will be made to the tool, but if there is a value in there, then you need to know if it is being applied or not.

[wms]

Smitty,
Turn off your nose compensation (select none).
And try one. But set your x zero at centerline before you do.

If I use auto nose comp with the setup you have it outputs code that is .040 to big. ie the shaft dia. ends up .210.

[HuFlungDung]

Yes, Ward has a good point. The reason your parts are too big is because you are zeroing the edge of your tool, but the program is writing code for the center of your tool! The correct zero for your tool is farther in than you thought !

However, programming to tool radius center is correct for the offset you need to make the balls the right size. Let me check something.

Okay, it does produce the correct offset code whichever way you choose to do it. The X values will be different because of the zeroed position though. Sorry for the confusion. I forgot, Onecnc won't let you gouge the part

Tool offsets would be the best solution to modify your tool position. What you can learn from all this, is that there are a few different ways to create the code, based on where the tool reference point is. "Mixin' 'em up will not work

[smitty]

I made the change to Turbocnc INI file. Changed it to 0.5 instead of 1.0
Removed Nose comp. Ran the part again, and the only thing that was re-cut where the balls. Shaft Diameter is at .210, balls are at .312.
Now, I am only taking .010 per cut, should I take .020 off. I see the program made the changes to the depth per cut, just wondering if that might make the change I need. Random thoughts again!!!

[wms]

Smitty,

Take a screen shot of the last 15-20 lines of your code and post it here.

[HuFlungDung]

I'm starting to get dizzy, now

I think you should just turn Comp back on to Auto, and adjust your tool X zero position in the X- direction by .04" Thats all that was wrong with your method, was the X zero was no good. When zeroing the center of the tool radius, it is physically impossible to "touch up" to the center line of the toolnose, so you have to touch up on the edge, and then keep going further towards the lathe axis by the amount of the tool nose radius.

Or, as I said, do this in your tool offset tables, from the zero point you have already established. Is any of this tool offset stuff getting through?

Then run the program as you posted above.

[smitty]

I think the dizzyness is over!!!
The last thing I changed was the CONTROL POSITION of the tool.
At first I had it at Nose center, and changed it to Tool edge Tangent, and made a run. Came out just fine, so I was thinking that with the tool at Nose center, the program was over compensating for the radius?
Anyhow, it works great. Thanks to everybody that chipped in, Esp
HFD and WMS. I know I tested their patiance, but I learned much about this program through their help and advice!!
Thanks,
Smitty

[wms]

Way to go Smitty.

I thought we had lost you there for a minute.

Glad things are going your way.

Glad to have helped.

Now go make some parts.

[smitty]

Lost me you did! But you guys stuck with me, so I thought I better do the same!!
Hey, I see from your Avatar you are into Sleds?
If so, very cool. Grew up on the darn things!
Smitty