G41 / G42 feed compensation

[skillalot]

Hi,

Let's say you cut a straight line with a 10mm end mill, with a feed-rate of 1000mm/min. No problem.
Then you cut a same straight line, also with that 10mm end mill at 1000mm/min feedrate, with cutter compensation on, still no problem.

Then you cut a 20mm hole with a 10mm end mill. In the gcode the 20mm circle is programmed at 1000mm/min feedrate.
Cutter compensation is turned on, and the center of end mill will not move in a circle of 20mm, but in a circle of 10mm instead, but still with that 1000mm/min feed-rate
This means that the speed at the programmed contour, the 20mm circle to be cut, is not 1000, but 2000mm/min.


How does the cutter compensation in UCCNC work, is this feed-rate compensated to keep the cutting speed of the tool at the correct value ?

[cncdrive]

Feedrate means movement speed on the movement path and so ofcourse it is not compensated by the CNC control software, you have to take care of that in your g-code file if you need that.
Usually the g-code program is written with the feedrate for the tool radius offset path taken into account already and so when the tool wears then it is slighly adjusted with e.g. 0.005, 0.01 etc. and so because the adjustment is small the feedrate change is also small and so it is usally not a problem...

[skillalot]

Yes, speed on movement path. And with radius compensation the moving path is the edge of material where you cut.
But the radius compensation changes movement path, and so the feedrate should be changed accordingly as well.
On proffesional machines this is a standard feature with cutter compensation.

So, what cam software automatically programs a 20mm hole with 10mm end mill at 500mm/min feedrate if it should be 1000 normally?

[cncdrive]

The movement path is different with an offset and so the feedrate is then on the modified toolpath. The feedrate is always understood on the toolpath if it is offset or not does not matter.
When you offset with radius then the toolpath changes and the feedrate is understood on that modified toolpath.
Please give me one example of a "professional machine" which doing what you say?
I don't think any CNC controllers would do that, but let me know if you know one.

[cncdrive]

I forgot to answer your question: I don't know any CAM softwares which using G41/G42, CAM softwares generate the fixed toolpath which you can offset if you want using G41/G42.
Maybe there are CAM softwares which doing what you saying, but I don't know any...

[ger21]

I forgot to answer your question: I don't know any CAM softwares which using G41/G42, CAM softwares generate the fixed toolpath which you can offset if you want using G41/G42.

I think that most "better" CAM programs can use G41/G42. Fusion 360 is one example.
There's nothing special happening when the CAM uses G41/G42. It just outputs the g-code on the line, exactly as drawn in the CAD program. And adds the G41/G42.

This is the first time I've ever heard of what's apparently called "feedrate scaling" with Cutter Comp.

I'm not sure why you would use this.
If you were programming without using G41/G42 (CAM doing the offset), then you'd enter your desired feedrate.

But when you program using G41/G42, then you program with a different feedrate, making the assumption that the control will change it? That makes no sense to me.

[cncdrive]

Hi Gerry,

Yes, I know that Fusion recently offered G41/G42, but I think it works simple, it just offsets the path and puts a G41/G42 in the code.
I've also never heard of any CNC controllers to do a feedrate adjustment. If it has to be done like that then I'm sure the standards book would describe it in details, but it is not even mentioning that.

And one more thing is that in CNC machining the important is the pheripherial speed of the cutter and so if the CNC controller would adjust the feedrate as the OP suggests then that speed would change which could easily lead to broken tools and burnt in materials etc.
I think the logical and proper way is to still keep and not adjust the feedrate at all and this is how CNC controllers like the UCCNC and others that I know work.

[cncdrive]

Yes Terry, it would be unlogical and would create problems only if the feedrate is changed by the G41/G42.

[ger21]

It looks like the "feedrate scaling" I saw when Googling was a feature independent of G41/G42.
What I saw was a Fanuc setting that controlled accel/decel when going around corners.

I couldn't find any other reference to feedrate scaling with G41/G42.

[skillalot]

Deckel Dialog 4 control from 1986 has it for example, enabled with M62.
It's manual is in german, it says "Vorschub optimierung", the M62 makes " Vorschub an der Werkzeugschneide constant".
Meaning that the feedrate will be constant at the edge of the cutter instead of the center of it.
This way your chipload stays constant, and you'll actually save tools. If you double the chipload intended your mill will break!

For conventional slot milling not necessery, as you have different parameters there, but for trochoidal milling paths where you use the full cutting length this is pretty important. The tools I use have a manual where all the parameters are in, it says how many chipload for different Ae values. So if I want 0.069mm chipload, and my speed on the outside of the cutter increases, the chipload also increases.