What's new
What's new

I'm curious... Do you use in-control diameter compensation when milling?

Do you use in-control diameter compensation when milling?

  • Yes (for all tools)

    Votes: 5 11.1%
  • Yes (for finishing tools only)

    Votes: 29 64.4%
  • No (my parts don't require tolerances that tight)

    Votes: 3 6.7%
  • No (other reasons)

    Votes: 8 17.8%

  • Total voters
    45

aarongough

Stainless
Joined
Oct 27, 2014
Location
Toronto, Canada
A thread the other day piqued my curiosity about this: do you use in-control diameter compensation when milling?

I don't use it at all, all my diameter comp is done in CAM as the tool tolerances themselves have always been tight enough for my needs, but I'm really curious what the percentage is of people who do actually use it...

Bonus points for letting me know if you use wear compensation only or total tool diameter offsets :)

-Aaron
 
I use wear comp on finishing for bores and contours only. Otherwise I do not use in control compensation.
 
Wear comp. Not sure if Fadal supports a negative offset, but Mastercam has a setting for reverse wear if not, meaning a +.002 would make the tool .002 smaller.

Also, in Haas controls you can set it for diameter or radius. All of our machines are set for diameter so whatever comp you set is total.
 
Yes.

It's nice when you have to hold a bore tolerance of +/- 0.0005 and your EM might be a bit undersize......:D Or when threadmilling......my calculations usually come out a bit wrong and I tweak the comp at the control. I've also used it to cut a profile using a roughing and finishing pass in FingerCam. For example, the first pass with a 1/2" EM has the D value set to 0.600", second pass is actual size with the same code. :D


I use total tool diameter (D value). What I started doing (Haas machine) is using G10 to set the offset from the program. That way you don't have to worry about someone changing it down the road and proceeding to make scrap. :eek:

For the example above using T1 D1, I would have code like so:

G10 L12 P1 G90 R.6

*roughing code*

G10 L12 P1 G90 R.5

*roughing code used for finishing*
 
Wear comp on finishers. Best case scenario, you never touch them and you wouldn't even notice a difference from what your doing now. Worst case scenario, you have wiggle room and can easily troubleshoot or back a tool off.
 
Wear comp on finishers. For critical tolerances I'll sometimes put in a +.001 and then skim it in. I'm usually cutting hard materials so over the life of a tool it goes to minus a couple thou until the tool is dead.

I tried doing resharps once, but found once you factor in the time to sort, package, do the paperwork, ship, receive, then deal with a cutter that's not the same as you programmed for, it's cheaper to use a new tool.
 
I use a mix of both.

For roughing and planar finishing operations, I use g40 and rely on cam software for the tool diameter. I would imagine this allows older controls to work a little bit faster without needing to do the comp calculations, though it probably doesn't matter.

When finishing a 2d profile, I almost always use cutter comp. Its convenient for me because I have a library of set tools (100+, I also use fadals, info for tools over number 99 are stored in the cam software). If you use new tools for every program, its easy to get burned if you forget to set the new tool diameter in the control.

If I really want to hold a profile tightly, I take it a step farther. In the cam side of things I added a checkable option for high accuracy profiles. It creates a loop in the main program that lets you cut, recut, and adjust the cutter comp until the profile you are machining to is the exact size you want without ever needing to exit, rewrite, reload, or resume from a line the program.

COMP.JPG
COMP_2.JPG

This is a sample code I pulled from a program



(0.375 2 FLUTE LONG REACH)
T1 G43 M06
M00
(Place Tool No 71 in the spindle)
H71 Z0.2500
S2547 M03
M08
G00 X-14.5180 Y26.8393
(TOOL NO 71 -- 0.375 2 FLUTE LONG REACH Coolant Flood)
(1 Passes Per Profile )
(0.5000 Target Depth)
G40
G10 L12 P71 R0+0.3810 [Here we set the cutter so it will leave 0.003 stock per side on the first pass]
#:RERUN1 [here is where the loop starts]
H71 Z0.2500
S2547 M03
G04 P2000.0
M08
F10.2
G00 X-14.3265 Y26.8393
G41 X-14.5180 Y26.8393
G00 Z-0.5000
G01 X-14.5180 Y26.3143
G03 X-13.7430 Y25.5393 I0.7750 j0.0000
G01 X-11.2360 Y25.5393
G03 X-10.6686 Y25.7864 I0.0000 j0.7750
G02 X-8.6918 Y25.7864 I0.9884 j-0.9196
G03 X-8.1244 Y25.5393 I0.5674 j0.5279
G01 X-5.5615 Y25.5393
G03 X-4.7865 Y26.3143 I0.0000 j0.7750
G01 X-4.7865 Y26.8393
G00 Z0.2500
G40
M5 M9
M00
(CHECK POCKET SIZE)
#WAIT
(ENTER STOCK TO REMOVE FROM WALLS ON NEXT PASS -- POSITIVE NUMBER ONLY)
(ENTER 0.0 IF WALLS ARE TO SIZE)
#INPUT V3
#IF V3<=0.0 THEN GOTO :DONE1 [if no stock remains, profile is done]
# D71 = D71 - (V3*2) [if stock remains, adjust the tool diameter]
#WAIT
#PRINT D71
#INPUT V99

#GOTO :RERUN1 [loop back thru and recut profile]

#:DONE1
G10 L12 P71 R0+0.3750 [reset tool to nominal diameter when done]

M05 M09
G28
 
Wear on finishers. I believe that is the one were if you don't have a value in the control it just uses the CAM toolpath but if you put something in the comp tables it will tweak the CAM calculated path by that amount.
 
I used to program everything with wear comp, and then I got a machine that did
not have a lot of memory, so to save code, I went to only using it when I absolutely
had to. And thats kind of where I'm at now.

I use wear because if I forget to change my wear back to zero in the control, its only
going to be a small problem, it its full 'D', there could be some big problems.

I only use any type of comp, only when I absolutely need it, other than that.. F'it.
Even a Fadal can hit ±.001 first shot. Its one more place I can make an error, its
one more thing I can forget, so I just try to eliminate it.

I do have one program that required a lot of hand coding, and in that program I run full
D comp. The only reason I did it that way was that I wasn't sure which endmill was going
to work the best. I've run it with necked down halves, 5/8, 3/4 and HSS 1 inchers. I've
had that program for over 15 years now...

But I guess that could bring up another question. How many of you save your programs, and how
many of you re-post them every time you need them. I only save the ones that require a lot of
hand work, other than that I repost to a file named "Delete Me" there is also Delete Me 2, 3, and 4.
 
I program in the comp but most of the time (99%) it just is set to zero.
Since my CAD/CAM is at most eight steps from the machine tool I leave it open and repost.
Helps that both are networked PCs, the CAM posts to the machine's hard-drive and the machine sitting idle knows a new file has shown up with the same name and asks for an okay to load it.

Many people avoid tool comp like the plague due to frustrating leadin problems.
Wear comp and tool dia or radius comp are the same thing, the two are added together in the processing of the path and become one number.
Bob
 
I don't know why anyone would avoid it unless the comp begin move gets in the way?

Well, yeah, now that you mention it ...

For helix bores, my Mastercam post puts the G41 on the G2/G3 of the lead-in for the finish pass, which my Speedio's control balks at. Control seems to only accept G40/G41 on G1's (maybe also some 4th-axis G-something).

So no wear comp on helix bores. I have to go back with a contour toolpath and give it a linear lead-in before the arc lead-in.

Regards.

Mike
 








 
Back
Top