Pros and Cons of TOOL EDGE vs TOOL CENTER

[BillStephan]

Hello All,

We had a spirited debate this morning regarding the merits programing styles: Tool edge vs Tool center.

We've always used tool edge, but some say industry standard is tool center so I'd thought I'd poll the best forum I know of and get some feedback. What's your preference, why and what are the pros and cons of both.

Thanks in advance, -Bill

 

[Vancbiker]

Lathe or mill? Manual or CAM programming? Both will alter the answers.

 

[BillStephan]

Both lathe and mill and CAM programing. However, today most lathe programing in done at the machine (supplemented with CAM for live tooling). We're looking for the best practice moving forward with the long term goal of eliminating on machine changes (golden source code - repost for changes).

 

[Mtndew]

Tool edge.
1) your programs will be point to point with almost no math required.
2) your comp will be zero for an on size tool using tool wear.

 

[Hebrewhammer8]

Mill Only: If you do anything other than dead simple parts its TCP all the way!

TCP!

TCP!

TCP!

GOOOOOOOOOOOOOOOOOOOO TCP!

 

[DDoug]

Hello All,

We had a spirited debate this morning regarding the merits programing styles: Tool edge vs Tool center.

We've always used tool edge, but some say industry standard is tool center so I'd thought I'd poll the best forum I know of and get some feedback. What's your preference, why and what are the pros and cons of both.

Thanks in advance, -Bill

With whom did you have this "Spirited Debate" ???

 

[Volitan]

Tool Edge - I did tool center back before cadcam, and would put the radius of the tool in the wear column. Made it easier to program.
Since using cad, there's really no reason I can think of to program that way.

 

[mhajicek]

Oh, are you talking about radius compensation styles? From the OP I was thinking it was about touching off tool length; if you touch off at the center it, larger endmills can sometimes cut a bit deep, since they're actually cupped a bit on the bottom.

For radius compensation styles, wear is hands down better than computer (what Mastercam calls them), for too many reasons to discuss quickly.

 

[Vancbiker]

Lathe; No CAM and part profile with tool radius comped in the machine.

Mill; CAM program and tool center. Some CAM systems (or posts) do not post tool edge well causing alarms when comp values are tool radius values. If manual programming on a mill then tool edge as it reduces amount of math one needs to do.

 

[usolutions]

How is that even a question? Tool center for roughing, tool edge with in-machine or dedicated tool presetter for finishing.

 

[Volitan]

I feel like this is going to turn into a spirited debate here as well.

 

[Booze Daily]

Every shop I worked in and also in my own shop I’ve used tool edge. Mostly because if you’re milling a, say, .625 hole with a .500 endmill the lead-in move won’t be big enough to get all the comp in and it will alarm.

I suppose it’s all what you’re used to. I don’t think it matters much as long as it’s consistent across all programs.

 

[alek95]

It's a matter of personal preference.

I prefer tool edge compensation on a mill. That way you can easily use any size end mill, just input your tool diameter.

I haven't been running lathes long enough to form an opinion either way.

 

[Volitan]

It's a matter of personal preference.

I prefer tool edge compensation on a mill. That way you can easily use any size end mill, just input your tool diameter.

I haven't been running lathes long enough to form an opinion either way.

That would be tool center then, right?

 

[guythatbrews]

Lathe tool edge and mill tool center seems natural to me.

But I never played with mill tool edge enough to work out all the compensation issues.

 

[SeymourDumore]

Isn't this an interesting question?
We can't even agree on the fucking definition of "edge" vs "center", let alone what to use!

Just look at the responses:

Tool edge.
1) your programs will be point to point with almost no math required.
2) your comp will be zero for an on size tool using tool wear.

Tool Edge - I did tool center back before cadcam, and would put the radius of the tool in the wear column.

Oh, are you talking about radius compensation styles? For radius compensation styles, wear is hands down better than computer

Tool center for roughing, tool edge with in-machine or dedicated tool presetter for finishing.

Every shop I worked in and also in my own shop I’ve used tool edge. Mostly because if you’re milling a, say, .625 hole with a .500 endmill the lead-in move won’t be big enough to get all the comp in and it will alarm.

Lathe tool edge and mill tool center seems natural to me.

My preference is this:

It's a matter of personal preference.

I prefer tool edge compensation on a mill. That way you can easily use any size end mill, just input your tool diameter.

I haven't been running lathes long enough to form an opinion either way.

I don't know how one wants to name it. I call diameter comp on a mill and TNR on lathe
Lathe or mill, rough or finish, the control has the tool diameter ( mill ) or tool nose radius (lathe) information and it controls how the tool needs to move to get the part done.
Every part, every feature, every single move (when on a contour ) is using full diameter or tool nose radius compensation with print dimensions!
In my view, anything else is just asinine.
But, as said, it is a personal preference.

But of course, you also get these kind of posts:

Mostly because if you’re milling a, say, .625 hole with a .500 endmill the lead-in move won’t be big enough to get all the comp in and it will alarm.

Let me assure you that a .500 dia endmill is very happily accepted to make a .5004 dia hole, let alone a .625 on any machine made in the last 40 years. using full diameter comp.
Put .500 in your offset for the tool, and run the following code:

G00 X0 Y0
G01 Z-1. F100.
G01 G41 X.2502
G03 I-.2502
G01 G40 X0 Z1. F200.
M30

Let me know if your control poops on it!

 

[13engines]

Every shop I worked in and also in my own shop I’ve used tool edge. Mostly because if you’re milling a, say, .625 hole with a .500 endmill the lead-in move won’t be big enough to get all the comp in and it will alarm.

I suppose it’s all what you’re used to. I don’t think it matters much as long as it’s consistent across all programs.

Damn... Seymour just beat me to it.

The last statement is certainly valid, but the first is really no problem at all. Tool Center (Feature Line) programing all the way all the time for all finish passes. Though not for most roughing.

Run this in a Fanuc machine with anything up to 0.274 in D2 and be reminded of how much you use to love real Cutter Comp. :-)
%
O1234 (1/2 EM DOING 5/8)

T2M6 (1/2 END MILL)
G17G20G40G49G54G80G90G98

G0X0.Y0.
G43Z0.1H2D2S1000M3
G1G41Y-0.275F20.
X0.0375
G3X0.3125Y0.I0.J0.275F10. (LEAD IN)
I-0.3125J0.
X0.0375Y0.275I-0.275J0. (LEAD OUT)
G1X0.F20.
G40Y0.
G0Z1.
G53Z0.M5
M30
%

Not that you'd want to, but you could even squeeze a 15mm in there with a couple tweaks.

 

[SeymourDumore]

Some CAM systems (or posts) do not post tool edge well causing alarms when comp values are tool radius values. If manual programming on a mill then tool edge as it reduces amount of math one needs to do.

Two things to note here:

1: If CAM cannot post properly comped programs using full diameter ( or edge as some calls it ), then said CAM must be discarded immediately with extreme prejudice.
2: There is no way to remain consistent throughout your operation if CAM code is center and hand code is edge.

 

[mhajicek]

Wear comp = nominal tool radius offset register contains a value of 0. Far less chance of manual error. You shouldn't be using regrinds or sizes of cutter other than what's on the setup sheet for so many reasons; SFM will be off, cutter will have different rigidity/deflection. If the program will run with a smaller cutter without breaking it, it wasn't optimized for the larger one.

 

[13engines]

Wear comp = nominal tool radius offset register contains a value of 0. Far less chance of manual error. You shouldn't be using regrinds or sizes of cutter other than what's on the setup sheet for so many reasons; SFM will be off, cutter will have different rigidity/deflection. If the program will run with a smaller cutter without breaking it, it wasn't optimized for the larger one.

I always use nominal size cutters and use comp to bring features to size and position in the tolerance zone I want to work in. In my software, offset paths have to be created and then programmed to. The feature lines are already there. Though as I said, I tend to rough with offset paths that leave behind material for finishing.

Many times these same paths can be used for other cutters like chamfers. Generally only needing a Z height change and a feed and speed jack up.

But hey... I've seen a couple of your parts. Whatever you're doing is doing just fine!