Tool compensation

[ssozonoff]

Hi All,

Can anyone point me to a good explanation of "Tool compensation" (G41 and G42)?

I have been reading around a little but it has not crystallized for me yet.
When and/or why would one use the Tool compensation feature.

I have cut some profiles (with rounded corners) in a 1.5mm GFK sheet without tool compensation and it looks just fine.

Thanks for any pointers.

Serge

[dcoupar]

G41 and G42 allow you to program the part profile, without the bother of calculating the cutter centerline coordinates. Or, if you program the cutter centerline, G41 and G42 allow you to adjust for oversize or undersize cutters. G41 will offset the tool to the left of the programmed path by the amount (+/-) stored in the offset register. G42 will offset the tool to the right of the programmed path.

[warfreak]

you also have to take into account if your cutting arcs (G2 G3) that it also affects the compensation direction

[ssozonoff]

Hi Guys,

Thanks, so if my CAM software does all the cutter centerline coordinate calculations for me I don't really have to worry about this offset?

Also I am assuming that the CAM software properly calculates the centerline when cutting for example a radius of 5mm on a corner with a tool having a dia. of 2mm ?

What I am trying to understand is if G41, G42 are used much less today because of better Tool path software? (or when G coding by hand)


Thanks,
Serge

[laszlozoltan]

Hi All,

Can anyone point me to a good explanation of "Tool compensation" (G41 and G42)?

I have been reading around a little but it has not crystallized for me yet.
When and/or why would one use the Tool compensation feature.

I have cut some profiles (with rounded corners) in a 1.5mm GFK sheet without tool compensation and it looks just fine.

Thanks for any pointers.

Serge

ok, you might have cut some shapes that look just fine, as you say, but how would you cut say a 3.015 inch box profile with a half-inch endmill that was about 0.003" undersize AND the box profile must not be undersize or 0.001 over ?
manually write out the g-code for that without cutter compensation
then suppose the end-mill you were going to use broke so you only have on hand a 5/8" endmill that is .002 undersized. that's a lot of work redoing the calculations isn't it ? and just making sure you didn't forget or miss anyhting. wouldn't it be easier to just be able to plug in the actual size of your tool somewhere to account for all the variations and have the controller do all the calculations while it runs ? that's cutter compensation in a nutshell.

[ssozonoff]

This was sort of what I was trying to get at in my earlier post.

If I have a good CAM software that does all the calculations for me where I can simply go and change the size of the tool and re-calculate I don't need to worry about tool compensation that much?

Thanks,
Serge

[laszlozoltan]

yes you can rely on the software to do the whole thing; but you have to update the program everytime your tool size changes, or it's effective tool size. that means you perhaps initally write and run the program in my example with .500 " em; but then you get to the machine and measure the tool and discover it was reground and is actually .497", so instead of changing the tool offset in the machine (using tool compensation) you have to plug in the real size .497" into your cam software, re-run the cam program; sometimes you have to edit the output (perhaps there's text in the output to aid checking that the controller doesn't accept) and then run it; while all you would have had to do is plug in the tool size (or the tool size difference) at the controller and run that.
Now if you are on your own at a shop it won't be too much of a problem to do everything on you cam software- but if you realize most shops have to pay a hefty price for each instance of that cam software so naturally will run as few instances as possible- perhaps just one. So if you are working with more than one machine, or more than one operator, you will start having an overlap in needing the cam software just to plug in a new tool size each time. Again, it is much easier to plug in the tool size (or tool size difference) at the controller.

[bborb]

You can make adjustments in your CAM program and repost, never having to fool with tool nose compensation. This practice is fine for a hobbyist but a machinist would be frustrated at the inability to make simple adjustments at the machine. It's one of the most powerful features of a CNC control. To be employed in the industry you must be able to incorporate tool nose compensation in your programs and manipulate offsets at the machine.

[ssozonoff]

Great guys Thanks.

This is exactly the answer I was looking for!

Serge