Hurco cutter comp issue.

[kappullen]

We have a "new" Hurco from another department with
very few hours.
Everything else is tied up so I decided to give it a try.
I've tried all day to get the cutter comp G41 to work with no success.
Here's a snippet of a program.
Our Hurco post is no good having I, J issues but that is another problem.
That is why I used the Mastercam Robodrill post.

%
O441 (POST2T)
(MASTERCAM - X)
(MCX FILE - T)
(POST - T-21IEL)
(MATERIAL - ALUMINUM INCH - 2024)
(PROGRAM - POST2T.FNC)
(DATE - OCT-05-2010)
(TIME - 9:29 AM)
(POST DEV - IN-HOUSE SOLUTIONS)
(T1 - 3/8 FLAT ENDMILL - H1 - D1 - D0.3750")
(T2 - 3/8 FLAT ENDMILL - H2 - D2 - D0.3720")
(OVERALL MAX - Z2.)
(OVERALL MIN - Z-.687)
N100 G00 G17 G20 G40 G80 G49 G90
N110 T1 M06 ( 3/8 FLAT ENDMILL)
N120 (MAX - Z.25)
N130 (MIN - Z-.687)
N140 G17
N150 G00 G90 G54 S2500 M03
N160 X-.2337 Y.3266
N170 G43 H1 Z.25
N180 G94 G01 Z0. F5.
N190 X-.0975 Y.2918 F12.
N200 G03 X-.051 Y.2859 I.0465 J.1816
N210 X-.0541 Y.259 I.0558 J-.0201
N220 X-.0291 Y.1417 I.6144 J.07
N230 G02 X-.0228 Y.0732 I-.1397 J-.0474
N240 G01 X-.026 Y.0364 Z.0006
N250 X-.029 Y.0014 Z.0037
N260 G00 Z.25
N270 X-.6235 Y-.1875
N280 Z.1
N290 G01 Z-.125 F5.
N300 G41 D1 X-.436 F12.
N310 G03 X-.2485 Y0. I0. J.1875
N320 G02 X.2485 I.2485 J0.
N330 X-.2485 I-.2485 J0.
N340 G03 X-.436 Y.1875 I-.1875 J0.
N350 G01 G40 X-.6235
N360 Z-.025 F125.
N370 G00 Z.25
N380 X-.6205 Y-.1875
N390 Z.1

I've put wear values in as well as fiddled with the mill size
on the tool page with no success.

Where am I making my mistake?

Thank You for your help.

kap Pullen

[bloke]

Have a look down the thread list for one called "Hurco G-code" about a dozen threads on from yours. There's some examples that will show you formatting.

[glovebox20]

Here's The Link to "Hurco-G-code"

Hurco g-code

Here another thread that might be worth looking at

http://www.cnczone.com/forums/hurco/...ive_value.html



Here's the mill format I'm familiar with


N6T6M6(3/4 ROUGH)
S1569M3
G90G0X24.3707Y-3.952
Z4.M8
Z-.14
G1G41Y-4.202
Y-5.2131
G2G17X24.3456Y-5.3866I23.7595J-5.2131
G1X24.0243Y-6.4714
G40X23.9959Y-6.5672
G0Z4.
M9
M25 (Home Z-axis, Orientate spindle)
N4T4M6(ANGLE CUTTER)

This is a "Basic NC" (.HNC) format for a Ultimax 3/4 control. If you opted for the Industry Standard NC (ISNC) option, Your machine will probably be different. Note: I And J moves are Absolute, not relative from start point like "Fanuc" (ISNC?).

If your Running a Ultimax, just fill out your part and tool offset like "normal", however, there will be an extra "Diameter/wear field" in the tool setup page where you would use to adjust for cutter wear. The extra "Diameter field" only shows up when your in NC mode, not Conversational. Make sure you turn off Cutter Comp. before moving in a rapid move to avoid troubles. The mill knows what offsets to use base on the tool in the spindle and defaults to the part offset in your part setup page.


If your going to use G43, workoffsets, D #'s, etc, it may look like this.

N6T6M6(3/4 ROUGH)
S1569M3
G90 "G56" G0X24.3707Y-3.952
"G43 H6" Z4.M8
Z-.14
G1G41 "D56" Y-4.202
Y-5.2131
G2G17X24.3456Y-5.3866I23.7595J-5.2131
G1X24.0243Y-6.4714
G40X23.9959Y-6.5672
G0Z4.
M9
M25 (Home Z-axis, Orientate spindle)
N4T4M6(ANGLE CUTTER)

Now when you setup your offsets, there should be a Soft key in your Part/Tool set up page for "additional NC offsets". Not sure what it is labeled exactly, but it should be there somewhere. Go into the "additional NC offsets" and fill in your offsets here. If your familiar with "Fanuc OM controls", it should look somewhat familiar. The D # cannot equal the H # because there's only one column for each tool offset. I just add a constant number the the tool number to get the D offset (ex. T6 + 50 = D56) I believe the "Store position button" is still functional.

If you have ISNC or the WinMax control, this may be different for you.

good luck

glovebox20

Please reply with your progress and correct me if I'm wrong.

[kappullen]

Thank You Glove Box and others.
That dia comp screen comes up behind the extra
length comp screen.
It did the trick.
I'm doing 4-40 thread milling in A286 and couldn't hold size
without you.
Kap

[glovebox20]

That's what CNCZONE is here for.