Dia offset 'Wear' Not working

[killall-9]

Im scratching my head wondering why my code is exactly the same when posted with Computer or Wear selected ??

 

X4 MPMASTER

 

I've included the mcx

[Guest CNC Apps Guy 1]

Do you have lead in/out active?

[Allan]

The code would be Identical....except for the inclusion of the G41 or G42.

[killall-9]

yes, tangent

[killall-9]

The x and y coordinates are not changing.

[Allan]

Exactly...the X Y co-ordinates will be the same...the only diffrence will be that with wear there will be a G41 or G42

 

The intent is that you will have a small offset in your dia offset table..

[Guest CNC Apps Guy 1]

They won't change on wear. Only Control.

[CJep]

The x and y coordinates are not changing.

 

???

I did not have your custom post for the OKK/Fanuc, I used gen Fanuc 4axis VMC,

 

N102 G0 G17 G40 G49 G80 G90

N104 T7 M6

N106 G0 G90 G54 X3.1945 Y-.8125 A0. S3422 M3 <<<< here is your initial position

N108 G43 H7 Z.25

N110 Z.1

N112 G1 Z-.52 F6.16

N114 G41 D7 Y-.6953 F12. <<< here is the G41 cutter comp call with the Y lead-in

N116 G3 X3.0773 Y-.5781 R.1172

N118 G1 X1.3549

N120 G3 X1.203 Y-.6696 R.1719

N122 G2 X.836 Y-1.1102 R1.3914

N124 G1 X4.7216

N126 Y-.5781

N128 X3.0773

N130 G3 X2.9601 Y-.6953 R.1172

N132 G1 G40 Y-.8125 <<< here is the comp cancel and return to the initial Y position

N134 Z-.42 F6.16

N136 G0 Z.25

N138 M5

N140 G91 G28 Z0.

N142 G28 X0. Y0. A0.

N144 M30

%

[Oscar R.]

Im scratching my head wondering why my code is exactly the same when posted with Computer or Wear selected ??

 

X4 MPMASTER

 

I've included the mcx

 

If your trying to add comp through your toolpath with "Wear" you might try entering a number value in the "Stock to leave" in your cut perameters on your toolpath.

 

Like Allan said above, "Wear" will simply add a G41/G42 on your lead-in/lead-out code lines.

With that, the diameter offset will have to be added on the control at the machine.

[Aaron Eberhard]

There's been a lot of discussion about this, but I think it's one of the things that's most confusing for a lot of people.

 

Help says "When this option is selected, Mastercam calculates the compensated tool positions just as if Computer was selected, but also outputs the G41/G42 codes. This lets the operator adjust for tool wear at the control. Enter the difference between the selected tool size and the reground tool size at the control as a negative number."

 

Basically, if you have a tool diameter entered in Mastercam (Say, a 1.000" diameter), Whatever you're trying to cut will still be offset by .500" (the radius), but in the control you're supposed to have a tool diameter of 0. If you adjust that tool size + or -, your control will now compensate for wear of the tool. If you compensate by entering, say, -.002 (meaning, the diameter is actually .002" smaller than .500"), The control will adjust the line to .502".

 

The idea is that the operator can quickly measure the part, say it was wrong by X, and only enter X as the compensation amount and the control doesn't have to do crazy tool comp calculations, it only has to adjust the toolpath by (generally) a few thou at most. There have been a lot of problems over the years caused by a control having to do a huge cutter comp in a very short amount of time, or the control choosing the wrong side, etc. Wear makes it way easier for everyone involved.

[Bill Henderson]

Wear also allows a verify because MC will be using the diameter of the tool used. (have they changed this yet?)

 

Some places that use alot of regrinds will sometimes use a probe for tool dia. Leaving it at control gives the operator a chance to use alternate tooling if need be because the code is posted to the arc size. The tool table needs a tool dia./radius.

 

Posting to wear will give you a verify that is "accurate" but in some instances give you errors with too large or small lead-ins. at the machine