Centerline Toolpath

[Holomon]

The previous programmers here have always programmed toolpath to "print" dimensions rather than centerline of tool. This practice has lead to countless correcting of programs due to "TOOL DIAMETER TO LARGE" errors on our Fadals.I am considering a change to tool centerline programming and would like to know if anyone can share any pros or cons to either method..

[Steve Biehl - Cimquest Inc]

tool center or wear comping as MC calls it, works fantastic in MC. It allows MC to be a lot more intelligent, as far as where the tool will fit or not.

 

It can still cause you problems at the machine if the operator tries to comp to much. Like using a .625 dia EM when it is programmed in MC for a .5 dia. Still, if you use a long enough lead-in and don't have any tight corners, that would still work on the machine

[KMaynard]

I use it on my Fadal and it works great ..I've never had an issue ...

[Guest CNC Apps Guy 1]

quote:

---

...The previous programmers here have always programmed toolpath to "print" dimensions...

---

Sounds like "Old School" guys that won't let go of the past.

 

Wear or Computer COmp is far better IMHO.

[?Mark]

quote:

---

programmed toolpath to "print" dimensions rather than centerline

---

The only time I'd would use this method is for simple engraving. Everything else is centerline of a tool with wear comp. It's fool proof. Besides RPM and Feed rate for 1/2 and 5/8 end mills is so different...

 

 

Mark

[Mgrenier]

Here we program the part and put a comp equal to the radius of the tool. That makes it a lot more easy for the machinist to check if everything is good prior to machining and it is very easy to change the tool diameter on the machine without the programmer having to redo the PGM.

 

Have a nice day,

[Oppiz]

quote:

---

Here we program the part and put a comp equal to the radius of the tool. That makes it a lot more easy for the machinist to check if everything is good prior to machining and it is very easy to change the tool diameter on the machine without the programmer having to redo the PGM.

---

This how I used to do it. I found that it's so easy to redo a program in MC, that if tool dia needs changed I do it MC. This save that annoying tool radius error.

[Code_Breaker]

I live in a world of using both the print dimension/geometry and wear cutter's paths.

 

This cutter's path uses print geometry and offset the path a distance equal to the radius of thc cutter. You use a diameter of .000 on the tool page of the Fadal under "perfect" machining. You can the comp + or - as needed. Also, your lead in/out does NOT have to be larger than the radius of the cutter. In fact, I have use leadin/out as small as .005 with an 3/8 end mill.

In some cases, I have use .000 for my lead in/out. Still works OK. No more worrys about "TOOL DIAMETER TO LARGE".

 

Just my take of all of this . . .

 

Code_Breaker

[Teh Bear without Brains kinda idiot]

This is an old story we covered it many times and I and Iskander_teh_owl said a lot about it and

argued not once .

I like compensation to radius ,but every one of the ways has it`s minuses and pluses and you can succesfully make or scrap parts with any one of them .

I will not object at the new place to work with wear and I do worked once .

Make a search in forum on wear compensation you will get a lot of info .

 

Teh radius compensation

[chris m]

We were all about using part-path or 'blueprint' programming until we started using Mastercam, now everything we do is Wear comp because it allows you smaller lead moves and generates many fewer errors in the machine.

 

The added benefit is that if the guys 'forget' to put the radius values in the machine you still have a chance of the part being right [or having stock left on to remachine] where with straight control comp the part is immediately boned with a zero in the register..

 

C

[Thad]

+1 to wear comp.

 

Thad