I was hoping someone could shed a little light on the tool compesation issue. I've read through the pdf file in turbo cnc but am still confused. I think the closest match is g54 -g59 for fixture offsets. Some other programs have a g42, I believe, for tool radius compensation tool left or tool right with a diameter variable. Could someone give a simple step -by-step on this issue. Also what is incremental mode? Maybe I need a copy of the RS-274D. any links to this?

Flute Head,
At this time, Turbocnc does NOT support tool offset (diameter/radius) compensation. You have to do the offset yourself (either in the drawing or in the cam program). In my case, my solution has been to draw the part in cad, export as a dxf and then run it though Sheetcam (presently in beta, but should be released at the end of the month). Another option would be to draw the part in cad, do your offset there and then run it through Ace converter (available at the Turbocnc site [freeware]).

Hope this helps.

Bubba

Hey thanks, what about using g54 for a tool offset. Might just be easier to offset in autocad. After all, thats what I do for a living is run autocad.

Flute head, G54 is OK for a tool length offset, but not a tool diameter offset.

If you use Autocad you already know what incremental mode is: In Autocad it is called relative Cartesian coordinates;

Absolute means all dimensions are given from 0,0 (home)
Incremental means dimensions are given from the last point.

Cutter compensation: What you are calling tool offset (diameter)
What you do here is draw your part in Autocad. You have to decide which way you are going to cut the part. Is the cutter going to be going clockwise around the part perimeter on the left side of the part, or is it going counterclockwise around the part on the right side of the part.

This is cutter comp right G42 or cutter comp left G41
Cutter comp off is G40.

You would use cutter comp for a few reasons.
1. Let's say you normally use a 1/2" dia router bit to cut out your parts. You break your last bit and you only have 3/8" dia bits. If you programmed using cutter comp, you simply have to enter the diameter of the bit in a table and the program adjusts itself. Without cutter comp, you have to rewrite the entire program.

2. You have a high volume shop and you send out router bits for resharpening. When they come back, they are slightly small in diameter. Cutter comp allows you to keep your finished parts to perfect size.

G54 is used for fixture offsets on your router bed. Its like setting up a UCS in Autocad. You can have more than 1. They are named, G54, G55, G56, etc. But you can use these for tool length offsets if you need them.

Alot of people cannot imagine programming without G41/G42 cutter comp. Other people cannot imagine why you would need to. I use it at work religiously, but at home I never need it.




Here's a site with a good program to help you learn all this stuff
http://www.betatechnical.com/autonc.htm

Despite my best efforts so far, I cannot get cutter comp working, at least with the simulation program I am using (CutViewer).

So yeah, I am rewriting programs A LOT. It stinks, but I was really meaning to get more familiar with my calculator :rolleyes:

At least its bearable to rewrite everything by hand if you have a visual simulator. Without that, it seems that programs are written at great peril.

Swami

THanks everyone, actually the g41,42 made sence to me. I thought there would be something similar in turbocnc. Can't wait to try-out the freebe program.

Swami, If you are writting G code by hand, I feel for you.
Download Sheetcam immediately, do not pass GO!

Im guessing that program will trace the contour of a part, and channel cut through a sheet of material in whatever depth path I choose?

Those channel cuts just keep building up chips in front of the cutter, and requires constant babysitting in my experience to keep it from loading up. Is that what happens to you?

I wouldn't mind writing programs a bit, if I could just program to the LINE in the drawing, instead of having to manually cutter compensate all the time.

Swami

Swami, you can do several things to minimize chip loading in the channel. Upcut spiral bits will bring the chips to the surface. An air nozzle pointed into the cut channel will help blow the chips out of the path.

You are essentially correct as to what Sheetcam does, but it takes that human error out of the equation, plus speeds up the programming so its a breeze, not a pain.

Anyway, upgrade to Mach2 and you can use cutter comp and program just the way you want.

Anyway, upgrade to Mach2 and you can use cutter comp and program just the way you want. I liked all your tips, but really honed in on this one.

I use Mach2 now (Trial Version). Are you saying I can write a program that would cut "to the line" and have Mach2 compensate? I know that it supports using traditional G43/G42 codes, but are you referring to something more sophisticated?

Thanks,
Swami

Yes, with Mach2, you can program " to the line" and use G41/G42 offset commands.

You will have to program in a lead in/lead out though.

I am not referring to anything else.
t

sigh. This is the part I am not having the best luck with. One thing that would help me troubleshoot: When using cutter comp in Mach2, will the DRO report the correct position of the cutter, or does it report the line?

Swami

I don't know because I don't use cutter comp in my home programs.

But if you want to troubleshoot, you need to stay simple. Write a program that will cut a 2" x 3" square for example. Use your cuttercomp and test it out.

You have to call out the proper tool along with cutter comp otherwise MACH2 doesn't know which tool in your tool table to use.

You might want to start your own thread or post another way to get more responses than just me.

I was hitting up the Yahoo Mach2 group. And yes, the DRO will show you the compensated value of where the cutter is.

I got Mach2 to work using G42 just now, but then mysteriously, it stopped working after I changed the feedspeed (which should have no bearing!!)

Thanks man,
Swami