New Onecnc user!!

[Rekd]

IrfanView

It's very quick and extremely powerful. Does slide shows and all kinds of things. Including screen capture.

http://www.irfanview.com/

'Rekd

[smitty]

Downloaded that Click5, works pretty slick!
Spent some time with HFD last night, thank you very much.
I guess this is just a little over my head, 'cause still making air chips. Sorry to waste your time HFD, but I am not doing something right. I will play with it later today, frustration is getting a little high, time for a break!
Thanks again HFD, you are a true asset to this group!
Smitty

[wms]

Smitty,

If you could get a file posted here or a picture then we would have a better idea of how to help.

Sounds like you and Hu have hooked up, so maybe you have sent him a file, if so he will, I'm sure, get you up to speed.

Don't get discouraged, all new things take a little time to get a hold of. Plenty of help here. Lots of good people to light the way.
You are no different than anybody else, we all went thru a "learning" curve.

[HuFlungDung]

Just keep at it Smitty, it will click pretty soon, there is just something that you don't know that I can't seem to pick up on just yet. The software is simple to use, but you do need some general understanding of how programs are written for any cnc lathe.

Were you able to get any results similar to the screenshots I sent to you?

If you are cutting air, where and why? Do you even have a method of defining the work's reference position on your machine? I assume you home the machine on startup, or do you just set all coordinates to zero, wherever the toolpost happens to be?

It is common to define the tool position relative to the workpiece end face with a G92 command. The distance from the lathe centerline is also defined in this command. Suppose your toolpost is Z2.25 to the right and X5. from the centerline. Define this position near the beginning of your program:
G92 X5. Z2.25

This does not cause any kind of machine movement, it merely defines the work coordinate system from which all the rest of your nc code will be referenced. After this, then a command:
G00 X.5 Z.1 will move your tool to the 1/2" diameter position, and .1" from the end of the work stock.

Of course you need to set tool offsets for this tool as well, which will be used to make small adjustments to your tool position, in the likely event that your G92 definition is slightly inaccurate. The tool offset must be called, however your controller is set up to handle it.

I presume by now that you do have some kind of toolpath going on. Once you have created your roughing toolpath, you can backplot the code to get a "hard copy" of the toolpath drawn on screen. Save it on layer named "backplot". Then email your file to me, or you can zip it and post it here for anyone with Onecnc lathe to download and look at.

At times like this, I look forward to the Lathe XP series when it comes out, because it will be so much easier to show you how to set up the process in the nc manager. However, we will make do for now.

[smitty]

What little hair I have left, is running for cover!! HAHA
When I set the tool at the beginning, I set both Zand X at zero. X just touching the material, same in Z. Then I back them both off .1 for clearance and reset both to zero.
Go to run the program, and the program thens backs the tool of an additional .320 and then starts to run the program. Again, air chips.
I will play with it again later today, and see where my mistake is at. At this point, I just would like to see something being cut. I have a piece of Delrin just begging to be machined!
Thanks again
Smitty

[wms]

Smitty,

I noticed that you said that after you "touch off" the material, you back off the cutter .100 and then reset your Zeros.

Well....this may be why you cut so much air. Onecnc lathe will put .100 default clearance to your Zeros. ( you can change this, it's under the "Boundary selection" dialog box.

Check what value is in this clearance box, sounds like maybe you have a value of around .220. (your .100 plus .220 in dialog box = .320 clearance)

[smitty]

The boundry/countour section is set at zero. The BOUNDRY has me confused. What does it do, and how do I adjust it. I will try and post my drawing and NC file. If this comes through, I can render the drawing fine, and pull the G codes fine, but once on the machine all goes to heck.

[HuFlungDung]

Smitty, you will need to set your nc driver for incremental output if you want to touch off as you have been doing. If X0 is anywhere else but on the lathe centerline, you will be screwed in absolute mode.

Typically, we create start lines for our machines. There is a box in NCPost Output settings, Save options, which allows you to create and save some code for the start and end of your program. This is where we put stuff that we will always call:

G80 (safety cancel any drill in case of a program abort and restart)
G40 (cancel tool compensation in case of abort and restart)
G90 or G91 (sets your controller for an upcoming program written with absolute or incremental values).
G92 X___Z___
T___ M6(tool change command or tool offset call out)
There could be other codes for tool offset, but they should all be described in your controller manual.

Note: your controller will have a default mode upon startup, either incremental or absolute. Consult your manual. But regardless, it is imperative to define how the program is written within every program itself.

G90 or G91 mode affects your NC Post general settings for G02 /G03. You may have to change these settings depending on what you do. Check your controller documentation about it.

Typically, in incremental G91mode, all arc outputs will have to be incremental, but in absolute G90, they could be either absolute or incremental, depending on how your controller software is configured and designed.

Note: onecnc will not output a G91 or G90 code when you switch the NC Post from one mode to the other. YOU will have to make sure the proper code appears in your nc code after it is produced.

[wms]

Smitty,
The boundary box is where you tell the program what you want to machine.

You can use a boundary box, (you have to draw this prior to opening the tool wizard), or most commonly you would use contour.

With contour, you select the "chain" or tool path that you want to machine, in the direction you want.

With boundary box, the program would machine every thing inside the box.

The clearance is set here. This adds clearance to your model, so the tool has room to rapid back to start the second, third, ect.... passes.

Normally you would "touch off" your part, in x and z, then set that as zero. Then add clearance in the boundary box.

[wms]

Smitty,

HU brings up a good point.

If you are using anything but the centerline of the spindle for X zero, then there is going to be problems with absolute programing.

It is most common to use the spindle centerline as x Zero, as this is also most common the x zero for your drawings and parts.

Looking at your drawing that you posted, your part is drawn with the centerline at x zero. Then when you touch off the outside and add .100 to that, then set x zero there, you are (half the diameter of your stock + .100) to far above where you should be.

Example diameter of stock = .500

.250 + .100 =.325 (to far in X plus) = (lots of air and no cutting action!)

[smitty]

Ooohhh,
I think a light bulb just came on!!!
Be right back, time to go do some testing!
Smitty

[smitty]

Ok,
Pulled the tail stock back, and measured from the center line of the Spindle. Now that got me VERY close, but I still am unable to change the .3208 value, (thats how far the X pulls back before any maching takes place) without editing the G-code. I will edit the code and see what happens next!
Smitty