4th Axis Horizontal.. Help.

[Nathan G. Baldwin]

First of all, I'm in X3, using a modified MPmaster post with an Okuma Horizontal. 4th axis is a tombstone (index to Angle). Post has worked great with a few changes but everything I've done so far has been for 3 axis work, so I've been programming in top wcs and

 

The part I'm working on has several angled sides that I need to index to and cut. As I understand it (thanks Jim) I need to be in the front WCS, but it seems no matter how i set my planes I get the same result, B axis indexes only in 90° increments. My MD/CD 4th axis is set to index and the units are in .01° Is there anyone out there who can walk me through this rodeo?

 

BIG thanks.Z-4162-A.Z2G

[Guest]

Try a TOP WCS and a Front Plane setting, the rotate about the Front for new planes

[K2csq7]

Some like the "Front" plane method for horizontals, some don't. Personally I have been programming horizontals for about 7 yrs. I like Top/Top. Generic Mpmaster 3/4 axis vertical MD (yes vertical) with the 4th axis in the MD set to rotate about the Y axis. Mpmaster control def & post. Top is B zero, right is B 90, B 180 ( back plane) is tricky and left is B 270.

Here is some code for simple drilling

 

%
O0000 (T)
(MCX FILE  - T)
(PROGRAM   - T.NC)
(DATE  	- APR-18-2011)
(TIME  	- 8:58 AM)
(T157 -  3/4 DRILL   		- H157 - D157 - D0.7500")
N1 G00 G17 G20 G40 G80 G90
N2 G91 G28 Z0.
N3 T157 M06 ( 3/4 DRILL)
N4 G00 G17 G90 G54 B0. X.8221 Y1.2402 S356 M03
N5 G43 H157 Z.1
N6 G94
N7 G99 G81 Z0. R.1 F4.28
N8 G80
N9 M05
N10 G91 G28 Z0. 123 M09
N11 M06
N12 M01
N13 T157 M06 ( 3/4 DRILL)
N14 G00 G17 G90 G54 B60. X1. Y2.5 S356 M03
N15 G43 H157 Z7.1 T157
N16 G94
N17 G98 G83 Z3. R3.35 Q0. F4.28
N18 G80
N19 M05
N20 G91 G28 Z0. 123 M09
N21 M06
N22 M01
N23 T157 M06 ( 3/4 DRILL)
N24 G00 G17 G90 G54 B90. X1. Y2.5 S356 M03
N25 G43 H157 Z7.1 T157
N26 G94
N27 G98 G83 Z3. R3.35 Q0. F4.28
N28 G80
N29 M05
N30 G91 G28 Z0. 123 M09
N31 G28 Y0. C0.
N32 G90
N33 M30
%

[Nathan G. Baldwin]

Thanks Guys,

 

So you 4th axis Gurus.. A general machining question.. how are you guys setting your zeros? I believe I am supposed to work from a Z zero as the center of the tombstone.. how do I measure that so I can offset my work origin in MC?

[K2csq7]

Measure the overall of your tombstone, then use an indicator and your relative zero to figure out if the faces are equal distance from the center. (Touch 1 face, set zero, move 180, touch face, compare relative reading...)

[Hardmill]

Thanks Guys,

 

So you 4th axis Gurus.. A general machining question.. how are you guys setting your zeros? I believe I am supposed to work from a Z zero as the center of the tombstone.. how do I measure that so I can offset my work origin in MC?

 

 

all depends on what your machining, multi parts on different faces wouldnt warrant

programming from center of rotation.

 

Much better to use work offsetts and prog to a part zero

 

 

 

 

 

 

 

 

PEACE

[Nathan G. Baldwin]

The parts I'm machining are setup in one vise with a flat milled on one side with an 8° shoulder on one side with two thru holes. In the other side of the vise, the part is flipped with two different angles for the back side of the part. view MCX file for more info.. And thanks a lot fellas.

[K2csq7]

Its your call, I would just use a different work offset as Hardmill suggested.

[delete]

Hi Guy's hope you don't mind if I chime in too

 

With one Month under my Belt of 4 axis Hortz...

 

I have been using Top / Front and A WCS off my stock modeled exactly how and where it will sit in the vice or Fixture.

From the Pallet C/L orgin

 

But My Last job was a casting so I really didn't know where it was so

I programmed the whole thing from the C/L of the Pallet until it was Faced /Doweled

To go unto pallet # 2.

Sometimes (Being a casting) the Spot drill went .200 in sometimes it just nicked the part?

It all worked out but Being a Moldmaker / CNC guy I feel like I cheated and fudged the whole job to get it to work.

Quite a bit of Hand editing at the control.

The Code and offsets are saved and with the fixturing were turnkey.

Thanks Nathan & Guys

 

Tony

[dforsythe]

I have always used local work cord for hz programming unless im using a mushroom fixture and the part is running on c/l of the pallet. I find that if you try and use numbers that are in model land you can really run into problems holding tight toll locations ( mainly depths as a hz comes up to temp). just finding the g54 and B location its really easy to use a dynamic work cord system like you will see below. the operators love it when and it makes for a fast setup. also this allow you to run the job on any tombstone, vise combo you have with zero re-prog.

 

my 2 cents

 

Damian

 

 

O3311 (1F333-1H.OP1)

(UNPROVEN PROGRAM)

(MPMASTER HAAS EC-500)

(1F333-1H.OP1.NC)

(POST - HAAS EC-500)

(DATE - APR-11-2011)

(TIME - 10:31 AM)

(****G10 INFORMATION START****)

G90

M98 P9002

G10 L2 P1 X2.00 Y9.5. Z12.557 ******you find your location of G54

G65 P9018 A54. B45. C55 X.001 ****the macro will do the calc and set g55........also you can place an inc X like the x.001

G65 P9018 A54. B90. C56 Z-.002 ***the macro also sets the rest of your work cord and allows full controle in an inc style of x y or z.

(****G10 INFORMATION END****)

M01

M31

(T2 - MITSUBISHI-SHELL-BXD4000R0203,1.5.031C/R,PROJ 4.5)

(T5 - MA FORD 135715001N .75 2F REM,1. LOC, .73 RD, 2.9 RL, 3.5 PR )

(T10 - MA FORD 13875004 .750 3F EM 1.625 LOC 2.25 PR)

(T29 - .500 X 90 DEG SD, 2.25 PR)

(T51 - .302 LETTER N JBR DRILL PRO 3.250)

(T52 - .2055 DIA JBR DRILL PRO 2.6)

(T16 - MA FORD 13825005 .250 3F EM 1.0 LOC 1.250 PR)

(T53 - .250 DIA X 100 CSTK )

(T54 - #40 DRILL )

(T32 - .250 X 45 DEG CM 1.4 PR)

(T55 - .3125 HSS REAMER PRO 1.75)

(OVERALL MAX - Z10.)

(OVERALL MIN - Z-4.6423)

G00 G17 G20 G40 G80 G90

G91 G28 Z0.

(FACE TOP OF STOCK)

T2 M06 (MITSUBISHI-SHELL-BXD4000R0203,1.5.031C/R,PROJ 4.5)

G90G10L12P#3026R0

(MAX - Z10.)

(MIN - Z-4.1313)

M11 (UNLOCK)