What's new
What's new

Pros and Cons of TOOL EDGE vs TOOL CENTER

If the program will run with a smaller cutter without breaking it, it wasn't optimized for the larger one
But it will still run now don't it?
At the same time, the program won't run with a larger tool and scrap it now does it?

That said, me thinks you're just trying to make an argument for your style of programming.
How many here optimizes the very last bleeding 1% out of their programs?
Not that I use many regrinds for finishing ( they are typically relegated for roughing with comp ), but often I switch to a metric EM for finishing in tight corners, all that without having to repost or change anything in the program.
 
But it will still run now don't it?
At the same time, the program won't run with a larger tool and scrap it now does it?

That said, me thinks you're just trying to make an argument for your style of programming.
How many here optimizes the very last bleeding 1% out of their programs?
Not that I use many regrinds for finishing ( they are typically relegated for roughing with comp ), but often I switch to a metric EM for finishing in tight corners, all that without having to repost or change anything in the program.
I use cutting parameter calculators like HSMAdvisor, define a specific tool making a specific cut, and use the different results for each operation. If I put in a smaller cutter, it'll probably snap. If I put in a larger cutter, it usually won't fit in the inside corners, and the higher SFM will dramatically shorten tool life. The program is made for a specific cutter, chosen to be the best cutter for the job at hand; just use that cutter. What possible home-shop-Harry reason could one have for doing anything different when most cutters are available same day?

If your programs are de-tuned to the point where you can throw in the next size up or down cutter and still have it work, then you're wasting a lot of machine time.
 
Feed rate difference for the same chip on c/l vs tool radius programming on a mill doing G02 or 3?
Some controls now can adjust actual motion as needed to keep the feedrate at the OD of the tool constant.
If you lie to the control about tool diameter it can not help you.
Talking milling here so think about profiling a one inch hole with a 7/8 endmill and a 1/4 endmill.
One of these circles is not the same size as the other. Same/same when profiling outside with radii on the part.
 
Last edited:
Lathe tool edge and mill tool center seems natural to me.
I am of the same opinion.

The advantage with using the imaginary tool tip as the reference point of the tool is that machining without radius compensation and without calculating offset profile, is not too inaccurate. At least straight diameters/shoulders would be correct.
 
Mill and lathe both, tool edge + wear comp.

I do not use full diameter comp when milling for a multitude of reasons, but they all boil down to one - changing the tool diameter negates the cam program. Cutting data is no longer correct, you don't know that your bigger cutter is going to clear clamps or fixtures or or cut an internal radius fully, or that your smaller cutter is going to clean up a floor properly, adaptive paths will no longer have correct load distribution, leads will be different to what is shown in the simulation, etc. etc.

I really can't see any upside to using full diameter comp for cam programs unless there are some legitimate reasons that you can't easily repost your program.
 
btw, It's not "tool edge", it's part surface programming and has been for forty years, since it first came out. CL has been called center line and cutter line but center is probably the original meaning. It's nicer to use standard definitions, that way everyone can agree on what we are talking about.
 
btw, It's not "tool edge", it's part surface programming and has been for forty years, since it first came out. CL has been called center line and cutter line but center is probably the original meaning. It's nicer to use standard definitions, that way everyone can agree on what we are talking about.
Ok, I will put it differently - tool radius/diameter compensation is calculated in my cam software and not on the machine control. This correlates to centreline toolpaths for milling and "imaginary tool corner" toolpaths for turning.

+ wear offsets to get everything the right size.
 
It’s a concession to the fact that 90% of folks running CNCs slept through 7th or 8th grade geometry and trigonometry classes.
For sure in spades. Did you get the above above circles and feedrates of tool centerline vs tool OD and the chip cut?
BUT.. when you have people... whose job is it to teach them now what is needed to know.
Now we just expect others to understand such things as what works in my brain.
The employees are no longer loyal and will jump ship for another dollar but what happened to training and teaching?
This math and above or viewing things in both 2 and 3D world was just so simple for me.
Took a bit of life to understand that my brain does not work the same as others. I was brutal at one time... an arrogant ass.

If the student or machinist fails is the boss,teacher or the guy at the machine?
Recent fail. Oh shit, $10,000 down the tubes.
Guy who did it is all "I am so sorry and will turn in my quit notice today".
Me..
"Not gonna happen... (pause for 10 seconds plus for the look), I just spent 10 large on teaching you. You will be on that machine tomorrow as I know you can do it and be the best "
 
Last edited:
I really can't see any upside to using full diameter comp for cam programs unless there are some legitimate reasons that you can't easily repost your program.

Gregor, I can offer one.
If you ever write some programs by hand, it is likely done with full dia comp.
If so, then you better make sure to enter the diameter into the offset BEFORE you run that program, and you better erase AFTER you ran it.
In my case, approx 10% of my mill programs, 100% of my lathe and 90% of EDM programs are hand-assist ( not hand trigged, but CAD drawn and hand coded ).
I also hand edit many ( most?) of my programs, where full dia just make much more sense.
As such, it would be an absolute nightmare to use two different methods.

Thankfully Featurecam creates full dia ( part line ) programs flawlessly even for roughing, so it is not yet an issue.
Might end up as an issue when I decide to move on from FC though.
 
Gregor, I can offer one.
If you ever write some programs by hand, it is likely done with full dia comp.
If so, then you better make sure to enter the diameter into the offset BEFORE you run that program, and you better erase AFTER you ran it.
In my case, approx 10% of my mill programs, 100% of my lathe and 90% of EDM programs are hand-assist ( not hand trigged, but CAD drawn and hand coded ).
I also hand edit many ( most?) of my programs, where full dia just make much more sense.
As such, it would be an absolute nightmare to use two different methods.

Thankfully Featurecam creates full dia ( part line ) programs flawlessly even for roughing, so it is not yet an issue.
Might end up as an issue when I decide to move on from FC though.
Last time I hand wrote a program was 25 years ago. I haven't had parts simple enough in most of that time, so it's an unused skill, and what's not used is lost. 90% of my parts use dynamic milling, surfacing, 3D roughing, four or five axis stuff, that would take much longer to do by hand. For my work at least, hand coding is a long obsolete skill.

And no, even back when I hand coded, I didn't use full diameter comp, because I knew what size cutter I'd be using.
 
And no, even back when I hand coded, I didn't use full diameter comp, because I knew what size cutter I'd be using.
Who gives a shit what size cutter you'll be using?
Hand coding a simple profile is still, by far, a fuckton easier using full dia and part dimensions than trigging shit out for no friggin' reason!
Silly argument against full dia.
You don't like it? Fine!
You don't need it? Fine!
But claiming that your center line + wear comp is somehow superior is ...
 








 
Back
Top